Altium Designer Documentation

PCB Placement & Editing Techniques in Altium Designer

Created: November 21, 2022 | Updated: December 16, 2022

A variety of objects are available for use in designing a PCB. Most objects placed in a PCB document will define copper areas or voids. This applies to both electrical objects, such as tracks and pads, and non-electrical objects, such as text and dimensioning. It is therefore important to keep in mind the width of the lines used to define each object and the layer on which the object is placed.

There are two types of objects in the PCB editor – primitive objects and group objects. Primitive objects are the most basic elements and include: tracks, pads, vias, fills, arcs, and strings. Anything that is made up of primitives and identified as a design object is a group object. Examples of group objects include: components, dimensions, coordinates, and polygon pours.

Object Placement and Editing Commonality

In Altium Designer, the process of placing an object is roughly the same regardless of the object being placed. At its simplest level, the process is as follows:

  1. Select the object to be placed from one of the toolbars or the Place menu.
  2. Use the mouse to define the location of the placed object in the PCB editor design space and its size (where applicable).
  3. Right-click (or press Esc) to terminate the command and exit placement mode.

Editing Prior to Placement

The default properties for an object can be changed at any time on the PCB Editor – Defaults page of the Preferences dialog. These properties will be applied when placing subsequent objects.

Use the Primitives column to access properties for objects and edit default values as required.
Use the Primitives column to access properties for objects and edit default values as required.

Default values for the objects are saved, by default, in the file ADVPCB.dft. Optionally, values can be saved in a .dft file with a different name. Controls are available to save and load .dft files, enabling you to create favorite default object value 'sets'. All settings saved in and loaded from .dft files are user-defined defaults. Should it be necessary, original default values can be brought back at any time using the Set To Defaults or Reset All options. The original default values are hard-coded.

Editing During Placement

A number of attributes are available for editing at the time an object is first placed. To access these attributes, press the Tab key while in placement mode to open the associated Properties panel. Pressing the Tab key pauses placement in order for you to make any required edits for the object.

Example properties dialog for a Pad object. 
Example properties dialog for a Pad object.

After edits have been made, click the design space pause button overlay ( ) to resume placement.

Attributes that are set in this manner will become the default settings for further object placement unless the Permanent option on the PCB Editor – Defaults page of the Preferences dialog is enabled. When this option is enabled, changes made will affect only the object being placed and subsequent objects placed during the same placement session.

Editing After Placement

Once an object has been placed, there are a number of ways in which it can be edited. These are described below.

The Associated Properties Panel or Dialog

This method of editing uses the associated Properties panel mode and dialog to modify the properties of a placed object.

After placement, the associated dialog can be accessed by:

  • Double-clicking on the placed object.
  • Placing the cursor over the object, right-clicking then choosing Properties from the context menu.

After placement, the associated mode of the Properties panel can be accessed in one of the following ways:

  • If the Properties panel is already active, select the object.
  • After selecting the object, select the Properties panel from the Panels button at the bottom right of the design space or select View » Panels » Properties from the main menus.
If the Double Click Runs Interactive Properties option is disabled (default) on the PCB Editor – General page of the Preferences dialog, when the primitive is double-clicked or you right-click on a selected primitive then choose Properties, the dialog will open. When the Double Click Runs Interactive Properties option is enabled, the Properties panel will open.
While the options are the same in the dialog and the panel, the order and placement of the options may differ slightly.
Press Ctrl+Q to toggle the units of measurement currently used in the panel/dialog between metric (mm) and imperial (mil). This only affects the display of measurements in the panel/dialog; it does not change the measurement unit specified for the board, which is configured in the Units setting in the Properties panel when there are no objects selected in the design space.

PCB Object Selection Commands

Besides the standard object selection/deselection commands, the PCB editor includes a number of special commands facilitating object selection/deselection operations. These commands are accessed from the Edit » Select and Edit » DeSelect sub-menus of the main menus. The selection commands can also be accessed from the  button menu in the Active Bar.

  • Select overlapped - use to single select the next design object in a set of co-located (overlapping) objects without utilizing a selection pop-up window. Selection obeys the following fixed order priority, cycled through successive use of the command:

    1. Pad
    2. Via
    3. Track/Arc
    4. Component
    5. Polygon
    6. Region/Fill
    7. Text

    Additionally, while using the Shift key to add additional objects to a current selection, you can use Shift+Tab to cycle through selection of the overlapping objects without losing your original selection.

    • To use this command, ensure that the Display popup selection dialog option is disabled on the PCB Editor - General page of the Preferences dialog.
    • Selection order also takes into account the current layer first before progressing to those objects on other layers.
    • Double-clicking on an area of co-located objects will always provide access to the pop-up selection window.
  • Select next (shortcut: Tab) - with an initial object selected in the design, this command is used to extend the selection to include the next higher-level object (or objects) based on logical hierarchy. The following cyclic logical selection 'flows' are supported:

    • Track Segment ---> All Connected (Contiguous) Track on the Same Layer ---> All Connected Copper ---> All Electrical Objects in the Associated Net
    • Connected Pad ---> All Connected (Contiguous) Track on the Same Layer ---> All Connected Copper ---> All Electrical Objects in the Associated Net
    • Unconnected Pad ---> All Electrical Objects in the Associated Net
    • Via ---> All Connected (Contiguous) Track on Layers Associated with Via ---> All Connected Copper ---> All Electrical Objects in the Associated Net
    • Copper (Region/Polygon Pour/Fill) ---> All Connected Copper ---> All Electrical Objects in the Associated Net
    • Free Pad/Via ---> All Connected (Contiguous) Track on the Same Layer as Pad, or on Layers Associated with Via ---> All Connected Copper ---> All Electrical Objects in the Associated Net.
    • Component ---> Via Fanouts, Escapes, Interconnect

    Via Fanouts - if a short enough trace connects a pad to a via and there is no other pad connected to this via by a shorter trace, then this trace and the via are considered this pad's Fanout.

    Escapes - a short enough antenna connected to a pad is considered this pad's Escape.

    Interconnect - a trace connecting two objects already picked up (for example, pads or fanout vias) is considered Interconnect.

    In addition, the feature caters for selection extension across multiple objects, selected across different nets in the design.

    Example selection across multiple nets, extending from the initially selected track segments, up the higher-order logical hierarchy.
    Example selection across multiple nets, extending from the initially selected track segments, up the higher-order logical hierarchy.

    This command is particularly useful when selecting routed nets. Learn more about Strategies for Selecting the Routing.

  • Board - use to select all objects that reside within the boundary of the defined board shape.
  • Net - use to select all electrical objects associated with a particular net.

    After launching the command, you can click an electrical object or connection to select all electrical objects in the associated net, or, if you know the name of the net you want to select, click on an area of the design away from any objects; the Net Name dialog will open. From there, you can enter the desired net name; that net will become selected when you close the dialog. If you are unsure of the net name, type ? then click OK to open the Nets Loaded dialog, which lists all currently loaded nets for the design.

  • Connected Copper - use to select all electrical objects that are connected to the same piece of copper.
  • Physical Connection - use to select all physically routed track between pad objects. Click on a track, pad or via; all contiguous track up to another pad will become selected, including any vias (the pads themselves will not be included in the selection).
  • Physical Connection Single Layer - use to select all physically routed track between pad objects on a single layer. Click on a track or via; all contiguous track on the same layer and up to another pad will become selected (the pads and vias themselves will not be included in the selection).
  • Component Connections - use to select all routed connections emanating from the pads of a chosen component (including tracks and vias) up to the next encountered pad in each case. The pads themselves will not be included in the selection.

    The command can also be accessed by right-clicking over a placed component then choosing the Component Actions » Select Component Connections command from the context menu.

  • Component Nets - use to select all nets (and member net objects therein) attached to a chosen component in the current document.

    The command can also be accessed by right-clicking over a placed component then choosing the Component Actions » Select Component Nets command from the context menu.

  • Room Connections - use to select all pad-to-pad routed connections that lie completely within the boundaries of the chosen room on the current document.

    The command can also be accessed by right-clicking over a placed room then choosing the Room Actions » Select Room Connections command from the context menu.

  • All on Layer - use to select/deselect all objects on the current layer.

    A component may be placed on a certain layer, but may not be deselected using the DeSelect » All on Layer command. This is because not all of the primitives that compose the component are placed on the same layer. For example, designator and comment text might be placed on the Top Overlay layer, while constituent pads are Multi-Layer.
  • Free Objects - use to select all free primitive objects within the design. Component objects, coordinate objects, dimension objects, length tuning objects, OLE objects, and polygon pour objects are all group objects, and will therefore not be affected by this command.
  • All Locked - use to select all design objects that have their Locked property enabled.
  • Off Grid Pads - use to select all pads that are not placed on the current snap grid.

Note that in the PCB editor, the Lasso Select / Lasso Deselect command provides two modes of operation:

  • Free-form - like a true lasso, you can draw a free-hand selection area to incorporate the design objects required.
  • Polyline - providing a polygonal 'lasso', this mode may be preferable to the free-form mode when there is a need to deselect objects more precisely. This mode is quite useful on designs that have components rotated at 45 degrees or when working on flex when the design isn’t always orthogonal.

You could even use a combination of both modes to get the deselection area exactly the way you want it. The current mode is reflected in the Status Bar. Press the Spacebar to change between Free-form and Polyline modes.

Hold the Ctrl key while using the Lasso Select, Inside Area, Outside Area, Touching Line or Touching Rectangle command to target the primitives of a component object.

Graphical Editing

This method of editing allows you to select a placed object directly in the design space and change its size, shape, or location graphically. Modification of shape and/or size (where applicable) is performed through the use of editing 'handles' that appear once the object is selected.


Example editing handles for a selected Fill object.

Click anywhere on an object away from editing handles (where they exist) to drag the object to reposition it. Depending on the type of object, it may be rotated and/or flipped while dragging.

  • Press Spacebar to rotate the object counterclockwise or Shift+Spacebar for clockwise rotation. Rotation is in accordance with the value for the Rotation Step defined on the PCB Editor – General page of the Preferences dialog.
  • Press the L key to flip the object to the other side of the board (where applicable).
  • Press the X or Y keys to flip the object along the X-axis or Y-axis where applicable.
  • Press the Alt key to constrain the direction of movement to the horizontal or vertical axis depending on the initial direction of movement.
  • Nudge the object by small amounts (according to the current snap grid value) by pressing the arrow keys while holding down the Ctrl key. Nudge by larger amounts (10 x snap grid value) pressing the arrow keys while holding down the Ctrl+Shift keys.
The number of primitives displayed when dragging multiple selected objects is controlled by the PCB.Rendering.MultiselectionDrag option in the Advanced Settings dialog. The Advanced Settings dialog is accessed by clicking the Advanced button on the System - General page of the Preferences dialog. If any changes are made in the Advanced Settings dialog, the software must be restarted in order for the changes to take effect.

Movement Commands

Object position can be changed using commands of the Edit » Move sub-menu of the main menus or the movement sub-menu in the Active Bar.

  • Move - this command is used to move any object in the current document. Any nets associated to an object will remain connected and the connection lines will follow the object when it is moved (displayed or not in accordance with the connect mode in force). Any routed track connected to the object will not be moved.
  • Drag - this command is used to move any object in the current document. If the object has connected tracks and/or arcs (for example, a component, pad or via), these will remain connected as the object is moved.

    • For connected track to move with a component, the Comp Drag mode must be set to Connected Tracks on the PCB Editor - General page of the Preferences dialog. If this mode is set to None, the command behaves just like the basic move command.
    • When using this command to drag a component with the Comp Drag mode set to Connected Tracks, the rotate and flip key commands become unavailable. Also note that smart movement actions (dynamic alignment and pushing) also are not available.
  • Component - this command enables you to move components in the current document. After launching the command, click the component in the design that you want to move and move it to the required position then click. Alternatively, click within the design space away from any objects to open the Choose Component dialog. Use this dialog to locate the component you want to move (either by jumping to the component or having the component brought to the cursor) and then reposition in the same way as described above. Note that this feature will work only if the target component is not locked.

    The command can also be accessed by right-clicking over a component in the design space then choosing the Component Actions » Move Component command from the context menu.

    Learn more about Component Placement.
  • Move Selection - this command enables you to manually reposition selected objects on the current document. Any nets associated to an object in the selection will remain connected and the connection lines follow the object when it is moved (displayed or not in accordance with the connect mode in force). Any routed track connected to the object will not be moved.

  • Move Selection by X, Y - this command is used to offset the current selection of objects by a precise amount in X and/or Y directions. After launching the command, the Get X/Y Offsets dialog will open. Use this dialog to specify delta X and/or delta Y increment values by which to move the selection.

    The command will only be available when at least one object is selected in the design space.

    The Get X/Y Offsets dialog
    The Get X/Y Offsets dialog

    • X Offset - use this field to specify the distance by which the selection should be moved along the horizontal axis. Positive and negative values can be specifed depending on the direction of movement required. Use the button to the right of this field to quickly toggle the entered value between positive or negative.
    • Y Offset - use this field to specify the distance by which the selection should be moved along the vertical axis. Positive and negative values can be specifed depending on the direction of movement required. Use the button to the right of this field to quickly toggle the entered value between positive or negative.
    • Toggle X/Y Offsets - click this button to quickly swap the offset values. The X Offset value will be used as the Y Offset value and vice versa.
    • Reset X/Y Offsets - click this button to quickly reset both offset values to zero.
    • Define X/Y Offsets Interactively - click this button to have the offsets calculated interactively. You will be taken to the workspace and prompted, in turn, to choose a start and end point. Click at the desired locations; the dX and dY values will be entered into the X Offset and Y Offset fields, respectively.

    To switch the dialog units between imperial and metric, press the Ctrl+Q shortcut. 

  • Rotate Selection - this command is used to rotate selected objects in the design space counterclockwise or clockwise and by a specified angle of rotation. After launching the command, the Rotation Angle (Degrees) dialog will open. Enter the required angle of rotation from 0.001° to 360.00°  (resolution 0.001°). Enter a positive value for counterclockwise rotation or a negative value for clockwise rotation. Click OK to close the dialog then position the cursor and click to define the reference point for rotation. The selected objects will be rotated about the reference point by the entered angle.

    The Rotation Angle dialog
    The Rotation Angle dialog

  • Flip Selection - flip the selected object(s) to the corresponding layer on the opposite side of the board. For example, objects on the Top Layer will be flipped to the Bottom Layer; objects on the Top Overlay will be flipped to the Bottom Overlay, etc.

    • Designator and Comment text becomes mirrored after a flip action.
    • For a pad that exists on the Multi-Layer, flipping will essentially reverse the order of its XY size pairings and shapes. Therefore, if a style of Top-Middle-Bottom has been used and the shapes are initially Round-Rectangle-Octagonal, flipping will reverse the stack and thus the shapes from the top will become Octagonal-Rectangle-Round.

Alignment Commands

Objects can also be moved by changing their alignment. To align objects with other objects, right-click on a selected object, then select Align. Alternatively, use the Edit » Align sub-menu of the main menus or the alignment sub-menu in the Active Bar. The alignment sub-menu contains a number of options for distributing selected objects.

The alignment commands will only move selected objects that are free to move - locked objects will not be moved.

The Align command is used to access the Align Objects dialog, which provides controls for quickly aligning the set of currently selected design objects as required. Use the dialog to set options for both the Vertical and/or Horizontal alignment of the selected objects, as required, then click OK to effect alignment.

The Align Objects dialog
The Align Objects dialog

  • Enabling both Horizontal and Vertical options at the same time may result in a conflict with the selected objects becoming stacked on top of one another.
  • Using the Space equally options can result in the moving objects being off-grid.
  • Horizontal - choose from one of the following options to determine the horizontal alignment of the selected objects:
    • No Change - leave the horizontal alignment of the objects unchanged.
    • Left - align objects so the outer edge of their left-most primitives has the same X location. The object with the left-most primitive is used as the reference.
    • Center - move objects horizontally so their centers are aligned. After clicking OK, you are prompted to click to choose the reference object.
    • Right - align objects so the outer edge of their right-most primitives has the same X location. The object with the right-most primitive is used as the reference.
    • Space equally - objects are equally spaced in the horizontal direction, between the left-most and right-most objects (which do not move).
  • Vertical - choose from one of the following options to determine the vertical alignment of the selected objects:
    • No Change - leave the vertical alignment of the selected objects unchanged.
    • Top - align objects so the outer edge of their upper-most primitives has the same Y location. The object with the upper-most primitive is used as the reference.
    • Center - move objects vertically so their centers are aligned. After clicking OK, you are prompted to click to choose the reference object.
    • Bottom - align objects so the outer edge of their lower-most primitives has the same Y location. The object with the lower-most primitive is used as the reference.
    • Space equally - objects are equally spaced apart in the vertical direction, between the upper-most and lower-most objects (which do not move).

The Position Component Text command is used to run the Component Text Position dialog from where you can change the position of the designator and/or comment text for one or more selected components in the current document.

The Component Text Position dialog
The Component Text Position dialog

The dialog is essentially divided into two regions - the Designator and Comment text. For both designator and comment, a graphical representation of a component is used as an aid to show where the text will appear based on the position selected. The following nine positional styles are available for the text, all of which are classed as 'automatic positions', meaning the text remains in the chosen position as the component is moved and rotated:

  • Left-Above
  • Left-Center
  • Left-Below
  • Center-Above
  • Center
  • Center-Below
  • Right-Above
  • Right-Center
  • Right-Below

To leave text in its current position with no modification, leave the No Change option enabled.

  • The designator and comment text positions can also be changed through the Properties section of the Properties panel. Select the designator/comment or the parent component to have these properties displayed. Click the relevant control that textually summarizes the current layer, position and rotation for the designator/comment then use the Autoposition property available in the pop-up window, as required.
  • To freely position the designator/comment text and have it follow the parent component's movement/orientation, choose the Manual style for the Autoposition property (when configuring properties through the Properties panel). You also can freely click, hold and drag text to the required position directly in the workspace; this will automatically switch the Autoposition property to Manual.

The Align Left / Align RightAlign TopAlign Bottom command enables you to align selected design objects by their left/right/top/bottom edges, respectively. After launching the command, the left/right/top/bottom edge of the left/right/top/bottom-most object is used as a reference, and all other objects in the selection will be moved left/right/top/bottom, so that their left edges are aligned with this reference.

The Align Left (maintain spacing) / Align Right (maintain spacing)Align Top (maintain spacing)Align Bottom (maintain spacing) command enables you to align selected design objects by their left/right/top/bottom edges while maintaining adequate spacing in observance with applicable design rules. After launching the command, the left/right/top/bottom edge of the left/right/top/bottom-most object is used as a reference, and all other objects in the selection will be moved left/right/top/bottom, so that their left edges are aligned with this reference. An object will be moved left/right/top/bottom as close to the reference object as the applicable clearance rule allows:

The Align Horizontal CentersAlign Vertical Centers command enables you to place selected objects in a single column/row, aligned by their horizontal/vertical centers. After launching the command, the cursor will change to a cross-hair and you will be prompted to select one of the objects in the selection; click on it. This becomes the reference object. All other objects in the selection will be moved in relation to this reference object, aligned by their horizontal/vertical centers.

The Distribute HorizontallyDistribute Vertically command allows you to make the horizontal/vertical spacing of a selection of objects equal. After launching the command, the left-most and right-most / top-most and bottom-most objects in the selection will remain fixed in their positions with all other objects spaced equally between them. The vertical/horizontal position of the objects is not changed.

The Increase Horizontal SpacingIncrease Vertical Spacing command allows you to increase the horizontal/vertical spacing of a selection of objects. After launching the command, the left-most/bottom-most object will remain fixed while the other objects in the selection will be moved right/up. Movement is such that the horizontal/vertical distance between the reference points of consecutive objects is increased by the amount specified in the Step X / Step Y field for the default Global Board Snap Grid.

The Decrease Horizontal SpacingDecrease Vertical Spacing command allows you to decrease the horizontal/vertical spacing of a selection of objects. After launching the command, the left-most/bottom-most object will remain fixed while the other objects in the selection will be moved left/down. Movement is such that the horizontal/vertical distance between the reference points of consecutive objects is decreased by the amount specified in the Step X / Step Y field for the default Global Board Snap Grid.

The Align To Grid command is used to move selected components to the nearest point on the applicable and modified snap grid. After launching the command, the reference points for each of the selected components will be moved to the nearest point on the applicable snap grid.

The Move All Components Origin To Grid command is used to move the reference point of all components onto the current Snap Grid. After launching the command, all components in the design space whose pads are on-grid will be moved so that their reference points are aligned to the current snap grid. By default, a report - Move Component(s) Origin To Grid - <PCBDocumentName>.html - will automatically be generated and opened as the active document detailing which components have and have not been moved.

  • Configure which format of report(s) to generate and show from the PCB Editor - Reports page of the Preferences dialog.
  • The applicable snap grid can be set up as required through the Grid Manager section of the Properties panel.
Note that components whose pads are currently off-grid are not moved.

Via the PCB List Panel

Panel Page: PCB List

The PCB List panel allows you to display design objects in tabular format, enabling quick inspection and modification of object attributes. When used in conjunction with the PCB Filter panel, it enables you to display just those objects falling under the scope of the active filter – allowing the targeting and editing of multiple design objects with greater accuracy and efficiency.

Using Cut/Copy and Paste

In the PCB editor, you can cut/copy and paste objects within or between PCB documents, e.g., component(s) from a PCB can be copied into another PCB document. You can cut/copy objects to the Windows clipboard and paste them into other documents.

When using 2D Layout Mode, select the object(s) you want to cut/copy, click Edit » Cut (Ctrl+X) / Edit » Copy (Ctrl+C) from the main menus or choose the Cut/Copy command from the right-click menu. The cursor will change to a crosshair and you will be prompted to select a reference point. This is a coordinate relative to the selected object(s) and is used to accurately position the selection when using the paste command.

When using the Copy command in 3D Layout Mode, the current view in the design space will be copied to the clipboard in bitmap format. You have control over the resolution of the copied image via the 3D Snapshot Resolution dialog that subsequently opens.

To copy the currently selected design object(s) to the clipboard in textual format, the Edit » Copy As Text command from the main menus can be used. This information can then be pasted into any text field or external text document. The details copied to the clipboard include:

  • The type of object it is.
  • The designator and comment (for a component object).
  • The object's location in the design space.
  • The layer upon which the object resides (or start and stop layers for a via).

An example of a component copied as text to the clipboard is:

Component Y1-25MHz (100.6mm,1.5mm) on Top Layer

An example of a track and via copied as text to the clipboard is:

Track (20mm,6mm)(80mm,6mm)  Top Layer
Via (45mm,6mm) Top Layer to Bottom Layer

To place the last content cut/copied to the clipboard, into the active document, choose the Edit » Paste command from the main menus or right-click within the design space and choose the Paste command from the context menu (shortcut: Ctrl+V). The latest clipboard content will appear floating on the cursor. The cursor position relative to the content is determined by the reference point designated when Cut or Copy was used to add the selection to the clipboard.

When using the Paste command, objects are pasted onto the same layer that the source objects were copied from regardless of which layer is currently set as the active layer in the editor.

To place the text that has been copied from a supported OLE application into any open PCB document, the Edit » Paste Text command from the main menus can be used. The text is converted to, and pasted as, PCB string objects rather than a single OLE object. The supported file types include universal formats such as CSV and XLS format spreadsheets and DOC and RTF word documents.

To control what happens to certain object attributes when they are pasted back into the design space, the Edit » Paste Special command from the main menus can be used. After launching the command, the Paste Special dialog will open.

The Paste Special dialog
The Paste Special dialog

Paste Attributes

  • Paste on current layer - enable this option to paste objects onto the current layer.
  • Keep net name - enable this option to keep the original net names for the objects.
  • Duplicate designator - enable this option to paste a component with the same designator without auto-incrementing.
  • Add to component class - enable this option to have the pasted component added to the same component class as the source component.
The Duplicate designator and Add to component class options become available for use when the copied source component is available on the clipboard.

Buttons

  • Paste - click to paste the object with all specified attributes.
  • Paste Array - click to open the Setup Paste Array dialog in which you can set up options for array paste.

Depending on the specific content being pasted, the following attributes can be controlled:

  • The objects can be pasted onto the current layer rather than the default paste behavior of pasting to the same layer from which the source objects were copied.

    You can also paste content onto the current layer directly in the design space using the Alt+Insert keyboard shortcut.
  • Ability to keep any assigned net naming.
  • Ability to duplicate the designator (for a pasted component).
  • Ability to add a pasted component to the same Component Class as the original source component.

Setup the options as required then click the Paste button to start the paste operation.

Clicking the Paste Array button in the Paste Special dialog will open the Setup Paste Array dialog, which allows you to paste multiple copies of the clipboard objects into the current document.

The Setup Paste Array dialog
The Setup Paste Array dialog

Placement Variables

  • Item Count - the number of repeat placements to be performed. For example, typing 4 will place 4 copies of the current clipboard contents.
  • Text Increment - enter the automatic increment for the display text (e.g., component or pad designator). Both alpha and numeric increments other than 1 are supported. For example, by setting the designator of a pad prior to copying it to the clipboard and setting the Text Increment field, the following types of pad designator sequences can be placed:
    • Numeric (1, 3, 5)
    • Alphabetic (A, B, C)
    • Combination of alpha and numeric (A1, A2, or 1A, 1B, or A1, B1 or 1A, 2A, etc)
  • To increment numerically, set the Text Increment field to the amount you wish to increment by.
  • To increment alphabetically, set the Text Increment field to the letter in the alphabet that represents the number of letters you wish to skip. For example, if the initial pad had a designator of 1A and the Text Increment field was set to C (the third letter of the alphabet), the pads would have the designators 1A, 1D (three letters after A), 1G (three letters after D), and so on.
  • Note that the last-used incremental value is remembered after pasting an array, the next value in that sequence will be used as the base value of the next array that you paste, unless you perform a new Copy action.

Array Type

  • Circular- enable this option to paste a circular array, using the current Circular Array settings.
  • Linear - enable this option to paste the array in a straight line, using the current Linear Array settings.

Circular Array

  • Rotate Item to Match - if enabled, array items will be rotated by the same angular amount as their Spacing.
  • Spacing (degrees) - the angular space between two adjacent pasted items.

Linear Array

  • X-Spacing - enter the desired X space between two adjacent items.
  • Y- Spacing - enter the desired Y space between two adjacent items.

When you paste the array, it will be held by the same reference location that was used when the Copy action was performed.

Enter the appropriate values in this dialog then click OK to place the array.

  • If placing a linear array, you will be prompted to select the starting point for the array. Position the cursor then click or press Enter to place the array.
  • If placing a circular array, you will be prompted to select the center point for the array, followed by the starting point for the array. Position the cursor in each case then click or press Enter to place the array. The objects will be placed in counterclockwise fashion around the nominated center point.
The starting point for the array will be where the reference point - designated when Cut or Copy was used to add the selection to the clipboard - will be located. It is therefore advisable to ensure the reference point is properly designated at the time of cut/copy, otherwise unexpected results may occur when pasting the array.

To copy one or more selected objects and then paste multiple instances of the selection wherever required in the current document, you can also use the Edit » Duplicate command from the main menus (shortcut: Ctrl+R). After launching the command, the cursor will change to a cross-hair and you will enter duplicate mode. The process involves the following sequence of steps:

  1. You will first be prompted to select a reference point. This is the point by which the selection will be pasted. Move the cursor to the required position near to the selection then click or press Enter. A copy of the selection will appear floating on the cursor.
  2. Move the cursor to the desired location in the design space then click or press Enter to place the copy.
  3. Another copy of the selection will appear floating on the cursor ready for placement.
  4. Continue placing further instances of the copied selection (rather like using a rubber stamp) or right-click or press Esc to exit.

Note that this command is used to copy and paste objects. As such, you cannot use the command for duplicating the children of group objects.

When an object is being pasted on a copper layer, and it overlaps a set of objects of different types when pasted, a net of the highest priority object will be assigned to the pasted object. The priorities are as follows (1 is the highest priority):

  1. Pad
  2. Fill
  3. Region
  4. Track
  5. Arc
  6. Via
  7. Polygon Pour

A net of the highest priority object is assigned to a pasted object. Here is shown an object (track) pasted over a set of objects of different types with different nets assigned. Since the pad is the object of highest priority in this set, its net (Pad_Net) will be assigned to the pasted object. Hover the cursor over the image to see the result.
A net of the highest priority object is assigned to a pasted object. Here is shown an object (track) pasted over a set of objects of different types with different nets assigned. Since the pad is the object of highest priority in this set, its net (Pad_Net) will be assigned to the pasted object. Hover the cursor over the image to see the result.

When an object is being pasted on a copper layer, and it overlaps a set of objects of the same type when pasted, a net of the object that is under the cursor when clicking to paste the object will be assigned.

A net of the object under the cursor is assigned to a pasted object. Here is shown an object (track) pasted over a set of objects of the same type (pads). Since pad 2 is the object that is under the cursor when clicking to paste the object, the net of this pad (Pad2_Net) will be assigned to the pasted object. Hover the cursor over the image to see the result.
A net of the object under the cursor is assigned to a pasted object. Here is shown an object (track) pasted over a set of objects of the same type (pads). Since pad 2 is the object that is under the cursor when clicking to paste the object, the net of this pad (Pad2_Net) will be assigned to the pasted object. Hover the cursor over the image to see the result.

When a set of physically connected objects is being pasted on a copper layer, and objects of different types in this set overlap existing objects with different nets, a net of the highest priority object in this set will be assigned to all pasted objects. The above priorities are applied in this case.

The net assigned to the highest priority object is assigned to the set of physically connected objects. Here is shown a set of connected objects (from left to right: Fill, Region, Track, Arc, Via, Polygon Pour) pasted over objects (vias) with different nets assigned. Since the fill is the object of highest priority in this pasted set, the net assigned to it (Via1_Net) will be assigned to each object in this set. Hover the cursor over the image to see the result.
The net assigned to the highest priority object is assigned to the set of physically connected objects. Here is shown a set of connected objects (from left to right: Fill, Region, Track, Arc, Via, Polygon Pour) pasted over objects (vias) with different nets assigned. Since the fill is the object of highest priority in this pasted set, the net assigned to it (Via1_Net) will be assigned to each object in this set. Hover the cursor over the image to see the result.

Locking Design Objects

Design objects can be locked from being moved or being edited on the PCB document by enabling their Locked attributes. For instance, if the position or size of specific objects is critical, lock them. Locking can be done in the Properties panel by clicking on the padlock icon () for the desired object(s) as shown in the following examples. 

Examples of the Lock icon in the Properties panel in Component mode and Pad mode. Examples of the Lock icon in the Properties panel in Component mode and Pad mode.
Examples of the Lock icon in the Properties panel in Component mode and Pad mode.

To toggle the state of the Locked property for a placed object that has the Locked property, you can also right-click over the object in the design space and choose the <ObjectType> Locked command from the context menu. When the object is already locked, the command entry on the menu will display a tick icon to the left.

If you attempt to move or rotate a design object that has its Locked property enabled, a dialog appears asking for confirmation to proceed with the edit.

If the Protect Locked Objects option is enabled in the PCB Editor – General page of the Preferences dialog and the design object is locked, the object cannot be selected or graphically edited. Use the Lock icon on the Properties panel to unlock the object or disable the Protect Locked Objects option to graphically edit this object.

If you attempt to select locked objects along with other objects, only those objects that are unlocked can be selected and moved as a group when the Protect Locked Objects option is enabled.

Component Primitive Locking

If a PCB component has its primitives locked (the Primitives option in the Component mode of the Properties panel is in its  state), all or the most properties of these primitives cannot be modified using graphical (e.g., using drag-and-drop) and non-graphical (e.g., using the Properties or List panel) editing methods. This will help to prevent occasional changes of component primitives that can result in incorrect assembly and fabrication outputs.

To enable/disable the preventing modification of PCB component primitives functionality, use the Protect Locked Primitives In Component option on the PCB Editor – General page of the Preferences dialog.

By way of an example, the Pad mode of the Properties panel is shown in the image below for a pad that is a constituent part of a PCB component that has its primitives locked. Note that all properties of the pad (except for Net and Testpoint properties) are dimmed and not available for editing. Note also that the  icon is shown at the far right of the pad's Component field, which denotes that the parent component has its primitives locked, and pad properties cannot be modified.

The Pad mode of the Properties panel (on the left) for a pad of a PCB component that has its primitives locked (on the right).
The Pad mode of the Properties panel (on the left) for a pad of a PCB component that has its primitives locked (on the right).

Re-Entrant Editing

The PCB Editor includes a powerful feature called re-entrant editing. This allows a second operation to be executed using keyboard shortcuts without the current operation being terminated. Re-entrant editing allows you to work more flexibly and intuitively. For example, consider starting to place a track and then realizing that another track segment must be deleted. There is no need to drop out of Interactive Routing mode. Press the E, D shortcut keys, delete the required track segment then press the Esc key to return to interactively routing the design.

Setting the PCB Cursor Appearance

By default, the PCB cursor is set as a small green 90 degree cross. This can be configured using the Cursor Type and Cursor Color settings, on the PCB Editor – General page of the Preferences dialog. For example, a large 90 degree cross that extends to the edges of the design window (Large 90 option) can be useful when placing and aligning design objects. Alternatively, a cross at 45 degrees (Small 45 option) might be useful if the 90 degree options are hard to see against grid lines.

Measuring the Distance in a PCB Document

Measure Distance between Two Points

To measure and display the distance between any two points in the current document, the Reports » Measure Distance command from the main menus (shortcut: Ctrl+M) is used.

After launching the command, the cursor will change to a cross-hair and you will enter measurement mode. Measurement is performed as follows:

  1. Position the cursor where you want to start measuring then click or press Enter.
  2. Move the cursor to the required end point then click or press Enter again. As you move the cursor, a measuring line is displayed as an aid.
  3. The Measure Distance dialog will appear, reporting the point-to-point distance measured, the X (horizontal) distance, and the Y (vertical) distance in both metric (mm) and imperial (mil) units. The measurement is also displayed visually within the design space, showing the measurement's X, Y, and direct distances. The direct (shortest) distance is shown in yellow, with the X and Y distances in light blue. The measurement is also entered as an entry in the Messages panel.
  4. Continue measuring the distance between other points or right-click or press Esc to exit measurement mode.
  5. To clear previous measurements from the design space, press Shift+C.
  • Change the snap grid if you cannot accurately position the cursor at the required points.
  • You may need to temporarily disable the Electrical Grid if you find that the cursor snaps to the center of electrical objects.
  • The visual results (measurement lines) for each measurement remain displayed in the design space until cleared by using the Shift+C keyboard shortcut.
  • Double-click on a measurement result in the Messages panel to cross-probe to that measurement and have its measurement lines displayed again in the design space.
  • Measurement information is also presented, dynamically, in the Heads-Up Display.
  • To copy the contents of the Measure Distance dialog to Windows Clipboard, press Ctrl+C when the dialog is open.
  • After selecting a start point, hold the Alt key to constrain movement to the horizontal, vertical, or diagonal direction depending on the initial direction of movement.

Measure Distance between Two Primitive Objects

To measure and display the distance between any two primitives in the current document, the Reports » Measure Primitives command from the main menus is used.

After launching the command, the cursor will change to a cross-hair, and you will enter measurement mode. Measurement is performed as follows:

  1. Position the cursor over the first primitive then click or press Enter.
  2. Move the cursor to the required second primitive then click or press Enter again.
  3. The Clearance dialog will open, reporting the clearance between the two primitives in both metric (mm) and imperial (mil) units. The dialog also contains information on the layer and location for each of the primitives. The measurement is also displayed visually within the design space, showing the measurement's X, Y, and direct distances. The direct (shortest) distance is shown in yellow, with the X and Y distances in light blue. The measurement is also entered as an entry in the Messages panel.
  4. Continue measuring the distance between other primitives or right-click or press Esc to exit measurement mode.
  5. To delete measurements from the design space, click Shift+C.
  • To be able to select a primitive using this command, that primitive type must be enabled in the Selection Filter.
  • This command only measures the distance between primitive design objects and, as such, you will not be able to include group objects in your measurements (e.g., components, dimensions, etc.).
  • The visual results (measurement lines) for each measurement remain displayed in the design space until cleared by using the Shift+C keyboard shortcut.
  • Double-click on a measurement result in the Messages panel to cross-probe to that measurement and have its measurement lines displayed again in the design space.
  • To copy the contents of the Clearance dialog to Windows Clipboard, press Ctrl+C when the dialog is open.

Measure Selected Objects

To measure the length of selected track in the current design, the Reports » Measure Selected Objects command from the main menus is used.

After launching the command, an information dialog will appear, detailing the total measured length of the track. The measurement is also entered as an entry in the Messages panel.

  • Measurable primitives can be either routed track (net-aware) or lines (track that is not net-aware). Arc objects can also be included in the measurement.
  • Measurements are returned in both metric and imperial units.
  • To copy the contents of the information dialog to Windows Clipboard, press Ctrl+C when the dialog is open.

Measure 3D Objects

To measure distances between objects when viewing the PCB in 3D, the Reports » Measure 3D Objects command from the main menus is used. Object-to-object and distance by board surfaces are calculated. Using this tool, you can quickly verify that clearances between objects are indeed correct in conjunction with 3D clearance checking.

After launching the command, the cursor will change to a cross-hair and you will enter measurement mode. Measurement is performed as follows:

  1. Choose the first 3D object or specific face of that object. As you move the cursor over a potential 3D object, the color of that object will change to green. If you want to select a specific face of the object, hold the Ctrl key as you move the cursor - the face currently under the cursor will be highlighted. With the cursor in place click or press Enter to confirm object/face selection.
  2. The tool will present visual measurements in the workspace for the shortest distance from the underside of this first object (face) to the board surface, and the shortest distance from this first object (face) to the board edge.
  3. Choose the second 3D object or specific face of that object.
  4. The tool will present visual measurements in the workspace for the shortest distance from the underside of this second object (face) to the board surface, and the shortest distance from this second object (face) to the board edge. In addition, the tool also visually presents the shortest distance between the two chosen objects (faces).
  5. The 3D Distance dialog will open, displaying the measurement results. When you have finished examining the results in the dialog, click the OK button to close it.
  6. Continue measuring the distance between other objects/faces or right-click or press Esc to exit measurement mode.
  • During the measurement process, you can press Shift+C to clear the display of measurements.
  • All measurement results are logged in the Messages panel. You can double-click on a previous entry to cross probe to that measurement.
  • The information about the chosen 3D object includes the Identifier of the chosen 3D Body objects (in parentheses). Having a value for the Identifier will help you know that you have clicked on the right object.
  • The tool calculates the distance between the two closest points on the chosen objects (or faces) - this distance is displayed in yellow. All other measurements are shown in light blue.
  • To calculate the object-to-object distance, the tool must first calculate the location of each of the selected objects. The results of these object-location measurements are also displayed. For the object-to-board measurements, the software calculates the distance from:
    1. the reference point on the object, to the board surface (Z measurement), and
    2. the reference point on the object, to the board edge (X or Y measurement).
    As with the object-to-object measurement, it also triangulates from the reference point on the object to the reference point on the board and displays this direct distance in yellow.
  • To copy the contents of the 3D Distance dialog to Windows Clipboard, press Ctrl+C when the dialog is open.

Measure Distances between Points of 3D Bodies

To measure distances between two points on the same chosen 3D Body, or between points between two different 3D bodies, the Measure Distances command is used.

The process is the following:

  1. Switch to 3D Layout Mode (shortcut: 3).
  2. Choose the Tools » 3D Body Placement » Measure Distances command from the main menus. The cursor will change to a cross-hair and you will be prompted to select the 3D model that you wish to start measuring from.
  3. Position the cursor over the 3D model that you wish to measure from and click, or press Enter. The cursor will change to the 3D positional cursor (blue, six-pointed), and you will be prompted to select a point on the 3D model.
  4. Move the 3D cursor over a vertex, or snap point, and click, or press Enter, to define the starting point for the measurement.
  5. Move the 3D cursor over a second vertex, or snap point, on the same 3D model and click, or press Enter, to define the end point for the measurement. Alternatively, click on a second, different 3D model, and choose a vertex, or snap point on that second model to use as the end point for the measurement. In either case, as you move the cursor to choose the end point, a measurement line extends from the chosen start point.
  6. An information dialog appears showing the point-to-point distance, as well as component distances for X-plane, Y-plane, and Z-plane, in both metric and imperial units.
  7. Continue to measure further distances, or right-click, or press Esc, to exit.
The color of the measurement line is based on the Selections system color, part of the System Colors section on the Layers & Colors tab of the View Configuration panel.

True Type Font Support

The PCB Editor offers the ability to use Stroke-based or TrueType fonts for text-related objects in a design (string, coordinate, and dimension text). Choice of font is made from within the associated Properties panel. Three Stroke-based font options are available - Stroke, Sans Serif, and Serif. The Default style is a simple vector font that supports pen plotting and vector photoplotting. The Sans Serif and Serif fonts are more complex and will slow down vector output generation, such as Gerber. The Stroke-based fonts are built into the software and cannot be changed. All three fonts have the full IBM extended ASCII character set that supports English and other European languages. When using TrueType fonts, TrueType and OpenType (a superset of TrueType) fonts found in the \Windows\Fonts folder are available for use. The feature also offers full Unicode support.

Note that only detected (and uniquely named) root fonts will be available for use. For example, Arial and Arial Black will be available but Arial Bold, Arial Bold Italic, will not.

The PCB Editor – TrueType Fonts page of the Preferences dialog provides options for embedding TrueType fonts when saving a design and for applying font substitution when loading a design.

Embedding fonts is useful when text is required to be displayed in a font that may or may not be available on a target computer upon which the design is loaded. Font substitution enables specification of a TrueType font to be used as a replacement when loading a design where fonts have not been embedded and where fonts may not be available on the computer upon which the design is currently loaded.

Net Information

For copper objects on a PCB (track, via, polygon, etc.), the following information is presented in the Net Information region of the Properties panel when the object is selected:

  • the parent Net, Diff Pair and/or xSignal and associated class in each case. Note that the Diff Pair and xSignal entries are shown only if the object is a part of a differential pair or xSignal, respectively.
  • Delay – the delay of the selected object(s) and the delay of the routed segments of the entire net. Include the Propagation Delay values of pads and vias, if they have been defined for the pads and vias.
  • Length – the total length sum of the selected object(s) and the total Signal Length. The Signal Length is the accurate calculation of the total node-to-node distance. Placed objects are analyzed to: resolve stacked or overlapping objects and wandering paths within pads; and via lengths are included. The Pin Package Length is also included if it has been defined for the pad(s). If the net is not completely routed, the Manhattan (X + Y) length of the connection line is also included. For more information regarding Signal Length and its applications, see the information about the PCB - Nets panel.

    The total length includes an estimate for the unrouted part of the net (the Manhattan (X + Y) length of the connection line), but for the total delay, it does not.
  • Max Current - the maximum current that the selected Track, Arc or Via object(s) can carry, determined from the IPC-2221A formula (Section 6.2):  

    I = k * ΔT0.44 * A0.725

    where:

    I = current [amps]
    A = cross-sectional area [sq mils] (trace width * layer stack copper thickness, or Abarrel, as shown below)
    ΔT = allowable temperature rise above ambient [°C]
    k = constant, such that:

    k = 0.048 for outer layers
    k = 0.024 for inner layers

    When multiple objects are selected, for example an entire net, the Max Current for that net is the smallest individual Max Current value of the selected objects.

  • Resistance - the sum of the resistance of the selected Track, Arc and Via objects, determined from the derived formula:

    R = (ρ * L / A

    where:

    R = resistance [Ω]
    ρ = resistivity of copper [Ω*mm2/m]
    L = trace length [m] (or Via Length, as described below)
    A = cross-sectional area = T * W [mm2] (or Abarrel, as shown below)
    T = trace thickness (from layerstack) [mm]
    W = Trace width [mm]

    Assumptions:

    • Ambient temperature = 22 °C
    • Allowable temperature rise = 20 °C
    • Thruhole copper wall thickness = 0.018mm 
    • Resistivity of copper = 0.017 Ω*mm2/m

    The total Resistance of the selected objects is the sum of the resistance of the individual objects.

Via Barrel Cross-Sectional Area - determined as follows:

 

Abarrel = AViaHoleSize - AFinishedHoleSize

Abarrel = [ π * (ViaHoleSize/2)] - [ π * ((ViaHoleSize - 2 * ViaWallThickness)/2)2 ]

Abarrel = π (ViaHoleSize ViaWallThickness ViaWallThickness2)

Via Length = distance from the center of entrance layer to the center of exit layer, as shown above

Notes - via length in these calculations is dependent on the via belonging to a net and the layers used by the connected tracks. A selected via with no net assigned will display the layer-edge to layer-edge length instead of the layer-center to layer-center length. Also, a via with a net assigned but no connected tracks will display a length of zero.

The Net Information region of the Properties panel. Shown here is an example for a selected track.
The Net Information region of the Properties panel. Shown here is an example for a selected track.

Click a link in the Net Information region to open the associated net/differential pair/xSignal in the PCB panel.

Assigning Nets to Objects

The PCB editor provides a number of ways to assign nets to primitive objects:

  • When one or more objects are selected, use the drop-down of the Nets field in the Properties panel. All nets for the active board design will be listed in the drop-down list. Select No Net to specify that the track is not connected to any net. Alternatively, you can click on the Assign Net icon () to choose an object in the design space - the net of that object will be assigned to selected objects.
  • Right-click over one or more selected objects, then choose Net Actions  » Assign Net. After launching the command, a crosshair appears. Hover the cross-hair to the net to which you want to assign the object(s), then click to select that net.
  • To resynchronize the net name of the routing primitives to the net name on the pads to which they connect, select the Design » Netlist » Update Free Primitives From Component Pads command from the main menus. After launching the command, a confirmation dialog opens asking whether you want to update free primitive nets with the component-pad nets. After clicking Yes and starting from each pad, the connected copper is selected and the net name of each primitive is set to match that of the pad. This operation does not affect the internal PCB netlist.

To examine and confirm that the objects that are physically connected, have the correct net assigned to belong in that physical net (a physical net means connected copper in this instance), you can use the Configure Physical Nets dialog accessed by choosing the Design » Netlist » Configure Physical Nets command from the main menus. The software analyzes the design, checking that all pads and the objects that physically connect them together (tracks, arcs, fills, etc.,) have the same net name assigned. When all net objects are correct, the net is shown in green. If any objects are detected as touching but have a different net assigned, they are flagged in red. A common example of when this can occur is if a component footprint has extra copper objects within the footprint. When this footprint is loaded during synchronization, the pads have the assigned net name applied to each pad but not the extra copper. The dialog is interactive; click on a net or primitive to cross probe to that object. Right-click or click the Menu button to access the available commands. The Action region of the dialog provides controls for specifying the action needed to be taken to resolve issues with the connected copper. By default, actions will be set automatically but can be adjusted as required. Once the actions are set, click the Execute button to update the net assignments.

Note that the default state for this dialog is to Only Show Errors, which means that objects that are correctly assigned are not listed. Disable this option by disabling the Only Show Errors option (using the Menu button) in order to display all objects using the Menu button.

The Configure Physical Nets dialog (displaying Only Show Errors option enable (back) and Only Show Errors option disabled (front)).
The Configure Physical Nets dialog (displaying Only Show Errors option enable (back) and Only Show Errors option disabled (front)).

  • Electrically Connected Copper - this region lists distinct groupings of copper primitives that are electrically connected as detected in the wiring of the design. For each grouping, the following information is presented:
    • Primitive - at the top-level, this entry reflects how many primitives are in the connected copper. Primitives can be displayed in a flat listing or grouped by type of primitive. The latter is configured by enabling the Show Primitive Groups option of the Menu button options. If this is done, the primitives will be split into the following groupings:
      • Connected Component Primitives - lists all component pad primitives as its children. These can be further grouped by parent component by enabling the Menu button option Show Components.
      • Connected Free Primitives - lists all non-component copper primitives as its children, further grouped by primitive type (Fills, Polygons, Tracks, Vias).
Connected Component Primitives are only presented when the Show Component Pads option is enabled on the Menu button options. Similarly, Connected Free Primitives are only presented when the Show Non Component Pads option is enabled. If one of these options is disabled, the top-level entry will reflect how many primitives are currently hidden. If both of these options are disabled, the dialog will be empty! The Show All Primitives button will become available at the bottom of the dialog, which quickly reveals all primitives (essentially enabling one or both of these disabled options).
Clicking on a primitive entry will highlight that primitive in the design workspace. Selecting multiple primitive entries will select all primitives in that selection. Selecting a higher-level entry in the list will cause all descendent child primitives to be highlighted in the workspace.
  • Original Net Names - this field reflects the net name currently assigned to the primitive, i.e., the net to which the primitive currently connects. The entry will be one of the defined nets for the board. However, if a primitive is not connected to a net, it will have the entry <Unassigned>.
  • Status - this field provides a top-level status entry for the grouping, which can be one of four states:
    • Blank - net assignment for the connected copper grouping is all correct and no update is required. The top-level entry for the grouping is colored green.
    • 1. Update Required - Unassigned Nets - in this state, none of the primitives in the grouping have been assigned to a net. The top-level entry for the grouping is colored yellow.
    • 2. Update Required - Some Unassigned Nets - in this state, some of the primitives have been assigned to the same net, but others have not been assigned at all. The top-level entry for the grouping is colored orange.
    • 3. Ambiguous - Multiple Net Names - in this state, there are primitives in the grouping that have been assigned to different nets. There may also be primitives not yet assigned. The top-level entry for the grouping is colored red.
  • Action - this region provides controls for specifying the action needed to be taken to resolve issues with the connected copper along with the result of executing the configured changes. For each grouping, the following is presented:
    • Proposed Action - this field is used to determine what action, if any, is to be taken. At the highest level for a grouping, this entry can be set to Update Net To, or Don't Update Net To. When updating, choose the new target net in the New Net Name field. Based on these two settings, the software calculates the actions that are to be performed at the child primitive level, arriving at one of the following proposals:
      • No Action Required - the primitive is already assigned/connected to the target net.
      • Update - include the primitive in the update so that it is assigned/connected to the new target net.
      • Don't Update - do not include the primitive in the update. It will remain connected to its current net.
    • New Net Name - use this field to set a new target net to which the primitives should be connected. The field's drop-down lists all nets detected among the primitives in the connected copper grouping. If you need to use a different net, right-click on the field and use the Change Copper Net To Board Net command from the context menu. This opens the Choose Net dialog which lists all nets currently defined for the board. Choose the net you require then click OK. That net will be entered into the field.
    • Done - this field reflects the success () or failure () of the update action once the Execute button is pressed and the changes applied.
Toggling the proposed action at a parent level quickly toggles the proposed action at the child level and for all children under that parent. Where individual children differ in their proposed actions - some included for update, some excluded - the parent level above in the hierarchy of grouped primitives will reflect this with the entry Some Updates.
  • Execute - once you are satisfied with the actions assigned to the netlist, click this button to update the net assignments.
  • Menu - click to access the following menu of commands that relate to the main list in general or to the currently selected primitive(s). The commands are identical to those available on the right-click menu for the main list region.
    • Update/Don't Update/No Action - use to quickly toggle the proposed action for the selected primitive(s). At a higher, parent level in the primitive hierarchy, use it to toggle the proposed action for all descendent children.
    • Select All - use to quickly select all connected copper groupings (the highest level entries in the list).
    • Select All With Same Status - with a top-level connected copper grouping entry selected, use this command to quickly select all other top level groupings with the same status.
    • Clear All Selected - use to deselect all entries in the list.
    • Expand All In Connected Copper - use to quickly expand all child groupings within the currently focused connected copper grouping.
    • Expand All - use to quickly expand all groupings for all connected copper groupings in the list.
    • Expand Children - use to quickly expand all descendent child groups below the currently selected grouping.
    • Collapse All In Connected Copper - use to quickly collapse all child groupings within the currently focused connected copper grouping.
    • Collapse All - use to quickly collapse all groupings for all connected copper groupings in the list.
    • Collapse Children - use to quickly collapse all descendent child groups below the currently selected grouping.
    • Only Show Errors - enable to only show errors in the dialog. The list will only present connected copper groupings whose Status is level 1, 2, or 3. Disable to also show connected copper that is correctly assigned.
    • Show Components - enable to have component pad primitives grouped by their parent components.
    • Show Primitive Groups - enable to have primitives grouped by their primitive type.
    • Animate Action Execution - enable to have the dialog scroll through the list as the execution proceeds, giving you an animated real-time progress of the execution of net changes. Disabling this option means execution of changes will be performed without such animation.
    • Warn On Netlist Change - enable to be warned when changes will affect the netlist for the board. The Netlist Change dialog will open, alerting you to how many primitives will have their nets changed and that this will affect the netlist. You can either click to Continue or click Filter Affected to more closely inspect the proposed changes.

      The Netlist Change dialog
      The Netlist Change dialog

    • Show Component Pads - enable to show connected component primitives in the list.
    • Show Non Component Pads - enable to show connected free primitives in the list.
    • Show Changes That Affect Netlist - enable to only present a list of the proposed actions (changes) that will affect the netlist for the board.
    • Change Copper Net To - one or more menu entries of this type appear when there are not many nets currently assigned to primitives within the focused connected copper grouping. Use such an entry to quickly choose the target net for the New Net Name field.
    • Change Copper Net To Net - this menu entry appears when there are too many nets currently assigned to primitives within a connected copper grouping to display as individual menu entries. Using this command gives access to the Choose Net dialog, listing all nets currently assigned to primitives within the grouping. Choose the net you require then click OK; that net will be entered into the New Net Name field for the focused connected copper grouping.
    • Change Copper Net To Board Net - use this command if you need to use a different net to those currently assigned to primitives of the focused connected copper grouping. This opens the Choose Net dialog, listing all nets currently defined for the board. Choose the net you require then click OK; that net will be entered into the New Net Name field.
  • Show All Primitives - click this button to quickly reveal all primitives. This button becomes available if the Show Component Pads and/or Show Non Component Pads options are disabled on the menu.

You can also clear all nets from the current design document, essentially flushing the internal PCB netlist. This may be desirable if you have changed net information in the source schematic documents and you want to fully resynchronize your PCB with the source schematic netlist information. To do this, choose the Design » Netlist » Clear All Nets command from the main menus. After launching the command, a confirmation dialog will open alerting you to the fact that this operation will clear all net information from the PCB. After clicking Yes, all net information will be removed. Any routed track will remain routed but will have a No Net assignment. Any unrouted logical connections will be removed.

To learn more about connectivity in your PCB design, refer to the Understanding Connectivity on Your PCB page.

To create a netlist file based on the connectivity created by the routing in the current design, choose the Design » Netlist » Create Netlist From Connected Copper command from the main menus. After clicking Yes in the confirmation dialog that opens, a netlist (Generated <PCBDocumentName>.Net, added to the Projects panel as a free document under the Source Documents sub-folder) is created in the same folder as the PCB design document and automatically opened as the active document. Each net in the netlist gets its name from one of the pads to which the routed copper connects.

Primitive Objects

Primitive objects in the PCB Editor are fundamental elements of design. They are called 'primitive' due to their raw or most basic nature. Certain primitive objects are used as building blocks to create more advanced design objects, such as arcs, fills, and tracks, to create PCB 2D component models.

Primitive objects are available for placement in the PCB Editor, with many object types also supported for placement in the PCB Library Editor. Commands for placement can be found in the main Place menu, as well as the Active bar, the Utilities toolbar, and various drop-downs of the Wiring toolbar. Depending on the object, placement may require several mouse clicks to define the object's appearance.

PCB primitive objects can be placed from the Active, Utilities, and Wiring toolbars.PCB primitive objects can be placed from the ActiveUtilities, and Wiring toolbars.

Objects are placed on the current layer. Ensure the correct layer has been made the current layer before effecting placement. The layer on which an object resides can be changed after placement.

Track objects are used for routing and for general-purpose drawing lines. There are four placed track segments in the image above, and another in the process of being placed.
Track objects are used for routing and for general-purpose drawing lines. There are four placed track segments in the image above, and another in the process of being placed.

A Track segment is a straight line of a defined width. Use tracks to define a straight line in the PCB design space. Tracks are placed on a signal layer to form the electrical interconnections, or routing, between component pads. Tracks placed on a non-electrical layer are called Lines, where they are used as general-purpose drawing elements to create component outlines, instructional information, keepout boundaries, etc. Tracks also are used in group design objects, such as dimensions and coordinates.

Although tracks and lines are actually the same object, the difference is how the software behaves during their placement, which is why there are different commands. When a track placement command is run, such as Interactive Routing, the software monitors the click location and automatically adopts the net name of an existing object (such as a pad) under the click location. It also monitors and obeys any applicable design rules. When a line placement command is run (Place » Line), these monitoring behaviors do not occur.

Tracks are available for placement in both PCB editor and the PCB Library editor. Regardless of which command is used (routing/track or line placement), the basic placement behavior is the same. After launching the command, the cursor will change to a crosshair and you will enter track placement mode. Placement is made by performing the following sequence of actions:

  1. Click or press Enter to anchor the starting point for the first track segment. If a routing-type placement command is being run and you click to start placement on an existing object, the track will adopt the net name of that object. For routing, the width will be determined by the applicable Routing Width design rule; this can be overridden by certain interactive routing options, which are described in more detail below.
  2. Move the cursor to define the track segment then click or press Enter to anchor the end point for this first segment, which is also the starting point for the next connected segment.
  3. Continue to position the cursor then click or press Enter to anchor a series of vertex points that define the series of connected track segments.
  4. Right-click or press Esc to end the current series of connected track segments.

Additional actions that can be performed during placement include:

  • Press the * key on the numeric keypad to cycle through the available signal layers. Alternatively, use the Shift+Ctrl+Wheel Roll combination to move through the routing layers; each notch of the mouse wheel will move to the next (or previous) available signal layer.
  • Press the + and - keys on the numeric keypad to cycle forward and backward through all layers currently visible in the design.

While placing track segments there are five available corner modes, four of which also have corner direction sub-modes. During placement:

  • Press Shift+Spacebar to cycle through the available corner modes.
  • Press Spacebar to toggle between the two corner direction sub-modes.
  • When in either of the arc corner modes, hold the , or . key to shrink or grow the arc. Hold the Shift key as you press to accelerate arc resizing.
  • Press the 1 shortcut key to toggle between placing one segment per click (shown in the first five images below), or two segments per click (shown in the last image below). In the first mode, the hollow track segment is referred to as the look-ahead segment.
  • Press the Backspace key to remove the last vertex.

Press Shift+Spacebar to cycle through the five available corner modes, press Spacebar to toggle the corner direction, press the 1 shortcut to toggle placement between one segment or two segments. Press Shift+Spacebar to cycle through the five available corner modes, press Spacebar to toggle the corner direction, press the 1 shortcut to toggle placement between one segment or two segments.
Press Shift+Spacebar to cycle through the five available corner modes, press Spacebar to toggle the corner direction, press the 1 shortcut to toggle placement between one segment or two segments. Press Shift+Spacebar to cycle through the five available corner modes, press Spacebar to toggle the corner direction, press the 1 shortcut to toggle placement between one segment or two segments.
Press Shift+Spacebar to cycle through the five available corner modes, press Spacebar to toggle the corner direction, press the 1 shortcut to toggle placement between one segment or two segments. Press Shift+Spacebar to cycle through the five available corner modes, press Spacebar to toggle the corner direction, press the 1 shortcut to toggle placement between one segment or two segments.
Press Shift+Spacebar to cycle through the five available corner modes, press Spacebar to toggle the corner direction, press the 1 shortcut to toggle placement between one segment or two segments.

The graphical method of editing allows you to select a placed track object directly in the design space and change its size, shape or location graphically.

When a track object is selected, the following editing handles are available:

A selected Track
A selected Track

  • Click and drag A to reposition the end points of the track.
  • Click and drag B to change the shape of the track.

The PCB editor includes sophisticated algorithms for moving track segments on the board so that the arrangement of the routing can be maintained. This sliding of track segments can be invoked interactively either by clicking to first select the track segment and then clicking and holding when the special cursor appears to slide the segment or by clicking and holding on a track segment and sliding it. Sliding behavior can be configured using the Dragging options on the PCB Editor - Interactive Routing page of the Preferences dialog. These options allow you to assign the Move action to a track, which is useful if you want to be able to freely move an individual track segment.

Control track sliding behavior with dragging options set at the Preferences level.
Control track sliding behavior with dragging options set at the Preferences level.

If the Move action is assigned through these options, the track segment can be rotated or mirrored during the move.

Interactive Routing and the Applicable Design Rules

During Interactive Routing, the default behavior is for the software to ensure the track segments are placed in accordance with the applicable Electrical and Routing design rules. That means the software will not allow a new track segment to be placed that violates an existing track segment that belongs to a different net; instead, it will clip the track segment to meet the design rules. This interactive routing behavior is known as the Routing Conflict Resolution mode. The default mode is Stop at First Obstacle (the current mode is displayed on the Status bar). Press Shift+R to cycle through the available modes.

The term applicable design rules means all the rules that apply to the object being placed. The design rules engine works on a system where you scope exactly to which objects you want each rule to apply. During placement, the design rules engine is queried to determine the highest priority rule that applies in the current placement situation. Rules that apply during Interactive Routing include:

  • Electrical Clearance
  • Routing Width
  • Routing Via Style

The animation below demonstrates routing in action. The net GND is being routed in accordance with a defined and applicable Routing Width design rule. Note that when the cursor is moved over the via associated to the +12V net, the route is automatically being clipped to ensure the applicable Electrical Clearance Constraint design rule is being met.

The applicable routing width and clearance design rules are automatically obeyed during interactive routing.
The applicable routing width and clearance design rules are automatically obeyed during interactive routing.

How the Routing Width is Determined

Unless the rules engine is disabled, the overriding behavior of the software is to always ensure that the routing width is within the range allowed by the applicable Routing Width design rule. A common approach is to allow a range of widths to be used for a net to give you flexibility in fitting in the route while satisfying the current carrying requirements of that net. Supporting this, the Routing Width design rule has Min, Preferred and Max settings in the PCB Rules and Constraints Editor that can be configured to allow a range of widths or can be set the same to require a specific width. The width can also be configured as an Impedance and can also have a different range specified for each signal layer.

The default Routing Width design rule is applied to all nets for a new PCB.
The default Routing Width design rule is applied to all nets for a new PCB.

As the designer, you have a number of options that can help select the most appropriate routing width when you begin routing. These are configured on the PCB Editor — Interactive Routing page of the Preferences dialog, as shown below.

The Interactive Routing Width Sources options determine what size is used when you start a route.
The Interactive Routing Width Sources options determine what size is used when you start a route.

Note the Track Width Mode is set to Rule Preferred in the image. This denotes that when the route commences on an existing net object, such as a pad, this is the width that will be used. However, if the route commences on an existing track, then the Pickup Track Width From Existing Routes option will override the Track Width Mode and set the new width to match the existing width.

As the designer, you can also press the Shift+W shortcut while routing to access a dialog where a different width can be selected, or you can press Tab to open the Properties panel and type in a new Width value. The value chosen or entered must lie between the Min and Max settings defined in the applicable rule. If not, it is automatically clipped back to the nearest of these. 

Interactive Routing Shortcuts

While you are routing, there are a number of shortcuts that are available. For example, you can press Shift+R to cycle through the available conflict resolution modes, or press Backspace to delete the last placed vertex (corner). To display a list of shortcuts while you are routing, press Shift+F1. A menu of available interactive shortcuts is displayed; select the required shortcut or press Esc to close the menu and use the shortcut key sequence.

During interactive routing, press Shift+F1 to display a menu of available interactive shortcuts
During interactive routing, press Shift+F1 to display a menu of available interactive shortcuts

Moving a Track

The Edit » Move sub-menu and the movement command menu in the Active Bar includes a number of commands that can be used to change the position or the shape of a track.

Re-Route

This command enables you to manually reroute existing track on the board. After launching the command, the cursor will change to a cross-hair and you will be prompted to choose a track. Position the cursor over the required track then click or press Enter. The functionality of this feature depends on whether or not the Preserve Angle When Dragging option is enabled on the PCB Editor - Interactive Routing page of the Preferences dialog:

  • Preserve Angle Dragging enabled - the track will be broken with a new segment added to maintain the orthogonal/diagonal connections. Move the cursor to slide this segment as required then click to effect placement. Right-click or press Esc at this point otherwise that new segment will be broken with a further segment. Use the Shift+R keyboard shortcut to cycle through options that control how obstacles should be handled during dragging (Ignore Obstacles, Avoid Obstacles, or Avoid Obstacles (Snap Grid)). If one of the Avoid Obstacles modes is enabled, the rules will be obeyed during dragging preventing you from dragging a segment into violation.
  • Preserve Angle Dragging disabled - both ends of the track segment will be anchored and you can now lay new segments of track between the two. Click or press Enter to place a new segment of track. Continue placing new track segments for the reroute or right-click or press Esc to stop.

Continue rerouting further tracks or right-click or press Esc to exit.

  • If Preserve Angle Dragging is enabled, you can effectively disable it temporarily by holding the Alt key before clicking on the target track segment. Continue to hold the Alt key while progressively clicking to reroute.
  • When rerouting track using this command and with Preserve Angle Dragging disabled, it is advisable to start the reroute from the left end of the chosen track segment and work towards the right end.
  • Similar re-routing functionality can be achieved by selecting a track segment then clicking-and-dragging its center vertex. Then subsequent clicking-and-dragging on resulting segment's center vertices along the original track from one end to the other.

Break Track

This command enables you to create a vertex (or break) in a track segment. After launching the command, the cursor will change to a crosshair and you will be prompted to select a track. Position the cursor over the required track segment at the specific point along the segment where you want to insert a break then click or press Enter. A vertex is inserted, effectively breaking the original segment into two.

Move the vertex to the required position then click or press Enter to place. The attached track segments behave according to the setting of the Preserve Angle When Dragging option on the PCB Editor - Interactive Routing page of the Preferences dialog:

  • Preserve Angle When Dragging enabled - the angles to adjacent track segments are preserved, maintaining the routing style.
  • Preserve Angle When Dragging disabled - the two individual track segments will rubber band to accommodate the move without maintaining the existing routing style.

Continue breaking more track segment or right-click or press Esc to exit.

You also can break a track segment at the current cursor position by using the Shift+Ctrl+Click&Hold keyboard shortcut.

Drag Track End

This command enables you to manually reposition or drag the end of a routed track segment. After launching the command, the cursor will change to a cross-hair and you will be prompted to select an object. Position the cursor over a track then click or press Enter. The cursor will jump to the end of the track segment that it is nearest to and the track end will be attached to the cursor. Move the end of the track to the desired position then click or press Enter to effect placement.

  • If the end of the chosen track segment is a vertex point to which no other track segments are connected, move the vertex to the required position.
  • If the end of the chosen track segment is a vertex point to which two track segments are connected, the attached track segments will rubber-band as the vertex is moved.
  • If the end of the track segment is connected to a component pad, moving the end will disassociate it from the pad. After the end is repositioned, a logical connection line will be shown from the track end to the pad provided the Smart Track Ends option is enabled on the PCB Editor – General page of the Preferences dialog.
  • If the end of the track segment is connected to a free pad, the pad will become attached to the cursor ready for repositioning. All track connected to the pad will rubber-band accordingly.
  • If the end of the track segment is connected to a via, the via will become attached to the cursor ready for repositioning. All track connected to the via will rubber-band accordingly.

Continue dragging further track ends or right-click or press Esc to exit.

  • This command is overridden if the Preserve Angle When Dragging option is enabled on the PCB Editor - Interactive Routing page of the Preferences dialog.
  • This feature also can be invoked by selecting the required track first then clicking and dragging the required end vertex.

Move / Resize Tracks

This command is used to move the end-points of multiple selected track segments, effectively resizing the segments. After launching the command, the cursor will change to a cross-hair and you will be prompted to choose a track end-point. To move/resize the tracks:

  1. Position the cursor on the end-point of one of the segments in the selection then click or press Enter.
  2. Move the cursor; all of the track segments in the selection will resize dynamically while maintaining original distances and angles between each other. The other end of each segment will rubber-band to maintain its existing connection/location.
  3. Once the segments are in the desired location, click or press Enter to effect placement and exit movement mode.
  4. To cancel out of the operation, right-click or press Esc.

While moving the segments around, the following additional controls are available:

  • Press the Tab key to cycle the cursor between the end-point of each track segment in the selection.
  • Hold the Alt key while moving to constrain movement in a particular direction dependent on initial direction moved. Horizontal, vertical and 45 degree angle directions are possible.
  • Press the Spacebar twice to quickly make all end-points of the track segments in-line with each other in either the horizontal or vertical planes. Press the Spacebar twice quickly again to return to the previous sizing.
This command also can be used to move the end-point of a single, un-selected track segment. Note that only the Alt key additional control can be used in this case.

Slicing Tracks

The Track Slicer tool provides an easy mechanism for cutting one or more track segments into two and can slice tracks on the current signal layer or all visible signal layers. To access the tool, choose the Edit » Slice Tracks command from the main menus.

After launching the command, the cursor will change to a cross-hair and you will be prompted to choose a starting location for the slice. In addition, filtering is applied to only show track objects within the workspace. This will either be all track across all visible signals layers or only track on the current signal layer, depending on the active setup of the Track Slicer. To slice one or more tracks:

  1. Position the cursor then click or press Enter to anchor the starting point for the slice.
  2. Move the cursor across the point of the track, or tracks, where you want to slice - the path of the slicer is shown by a line with the prospective cut(s) visually depicted.
  3. Click or press Enter to anchor the end point of the slicer's track.
  4. Continue slicing further track segments, or right-click or press Esc to exit slice mode.

Additional actions that can be performed - after the initial anchor point for the slice has been chosen, and while moving the 'slicing line' - are:

  • Press the B key to cycle between cutting track on the current signal layer only, or track on all visible signal layers.
  • Press the Spacebar to switch the cutting angle between 45 Degree increments or Any Angle.
  • Press the N key to cycle the slicer blade side between Left, Right and Middle.
  • Press the / key to select all sliced tracks.
  • Press the "," key to select sliced tracks to the left of the slicer.
  • Press the "." key to select sliced tracks to the right of the slicer.
  • Press the M key to not have any sliced tracks selected.
  • Press the Tab key to access the Slicer Properties dialog, from where properties for the Track Slicer can be changed on-the-fly.

    The Slicer Properties dialog
    The Slicer Properties dialog

  • A track segment is sliced such that the extents of the blade pass through what will become the centers of the hotspots of the resulting two segment ends.
  • You can freely define the width of the slicing blade through the Slicer Properties dialog. Alternatively, you can constrain the width of the blade based on the current Snap grid. If the value for the Blade Width is not a multiple of the Snap grid, it will be clipped so that it is on-grid. The resulting width is known as the Gridded Width. If this option is disabled AND the Blade Width is not a multiple of the current Snap grid, one or both of the resulting track segment ends may reside off-grid. If the Blade Side is set to Left or Right, the track end at the extent of the blade will be located off-grid (the track end along the starting location axis will remain on-grid). If the Blade Side is set to Both, then both track ends will reside off-grid.
  • The Blade Side option controls how the slice is made, in relation to the axis determined from the chosen starting location for the slice. In the design space, the axis determined by the chosen starting location appears as a solid line, while the extent of the blade appears as a dashed line. The following options are available:
    • Left - the slice will be made to the left of the starting location axis. The slice distance will be equal to the full Blade Width, or Gridded Width, as applicable.
    • Right - the slice will be made to the right of the starting location axis. The slice distance will be equal to the full Blade Width, or Gridded Width, as applicable.
    • Both - the slice will be made equally to the left and right of the starting location axis. The slice distance on each side will be equal to half the full Blade Width, or half the Gridded Width, as applicable.
  • Enable the Cut Current Layer Only option to only slice through track segments on the current layer only. Disable this option to slice through track segments on all visible layers, where those segments fall within the 'path' of the Track Slicer.
  • The extent of masking when filtering is applied to the workspace can be manually adjusted using the Dimmed Objects slider bar located in the Mask and Dim Settings section on the View Options tab of the View Configuration panel. Clear filtering by using the Shift+C keyboard shortcut.

Converting Tracks to Chamfered Path

The chamfering of 90 degree routing corners is a technique used to reduce reflections caused by the corner in a microwave frequency route. Arcs can be used but should have a radius of at least 3x the route width. Chamfering (also called mitering) is an alternative where the outer point of the corner is sliced off. Because Altium Designer's track objects have rounded ends, they cannot be used to create a chamfered corner. To create the chamfered corner, the selected track segments are replaced with region objects.

Select all the track segments to be chamfered and then select the Tools » Convert » Convert Selected Tracks to Chamfered Path command from the main menus. The Convert Tracks to Chamfered Path dialog will open. Use this dialog to configure the chamfer then click OK. Each selected track segment pair (with offending 90 degree angles) will be replaced with chamfered cornering and the original track segments in each pairing will be converted to a single solid (copper) region object.

Selected tracks will be chamfered by the specified amount at each right-angle corner.
Selected tracks will be chamfered by the specified amount at each right-angle corner.

Use the following options in the dialog to configure the chamfer:

  • Chamfer - amount of the outside corner that is to be sliced off, or chamfered, as a percentage of the existing diagonal corner distance.
  • Inside Chamfer - amount of material to be added to the inside corner as a percentage of the existing diagonal corner distance.

How big should the Chamfer be?

The percentage mitre is the cut-away fraction of the diagonal between the inner and outer corners of the un-mitred bend. 

The optimum mitre for a wide range of microstrip geometries has been determined experimentally by Douville and James. They find that a good fit for the optimum percentage mitre is given by

Subject to  and with the substrate dielectric constant .

This formula is entirely independent of . The actual range of parameters for which Douville and James present evidence is  and . They report a VSWR of better than 1.1 (i.e. a return better than −26 dB) for any percentage mitre within 4% (of the original ) of that given by the formula. At the minimum  of 0.25, the percentage mitre is 98.4%, so that the strip is very nearly cut through.

The process of chamfering converts multiple track segments into a single region object. This is a one-way process; once the tracks have been converted to a region, they cannot be converted back. For this reason chamfering should only be performed once all routing is complete. If you are unsure, save off a copy of the board before chamfering.

Outlining Selected Objects with Tracks and Arcs

The Tools » Outline Selected Objects command from the main menus can be used to place an outline of tracks and arcs around selected free primitives in the design. This feature can be particularly useful if you want to electrically isolate critical nets by tying the outline to a ground source. After launching the command, the objects will be outlined with tracks and/or arcs. The outline tracks/arcs are placed with a width of 8mil and the Net property set to No Net.

Clearance, Width and Short-Circuit design rules for the design are observed, so clearance violations will be flagged by the Design Rule Checker.

The Track mode of the Properties panel.
The Track mode of the Properties panel.

Location

The icon to the right of this region must be displayed as (unlocked) in order to access the below fields. Toggle the lock/unlock icon to change its lock status.
  • (X/Y)
    • X (first field) – the current X (horizontal) coordinate of the reference point of the track relative to the current design space origin. Edit to change the X position of the track. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default.
    • Y (second field) – the current Y (vertical) coordinate of the reference point of the track relative to the current origin. Edit to change the Y position of the track. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default.

Properties

  • Component – this field is shown in the PCB editor only when the selected Track is a constituent part of a PCB Component and displays the designator of the parent PCB component. Select the clickable Component link to open the Component mode of the Properties panel for the parent component.
  • Net – use to choose a net for the track. All nets for the active board design will be listed in the drop-down list. Note that if object placement commences at the same location as an existing object that is already connected to a net, then the Net property of the new object is automatically assigned to that net. Select No Net to specify that the track is not connected to any net. The Net property of a primitive is used by the Design Rule Checker to determine if a PCB object is legally placed. Alternatively, you can click on the Assign Net icon () to choose an object in the design space - the net of that object will be assigned to selected track(s).
  • Layer – use the drop-down to select the layer on which the track is located.
  • Width – displays the current width of the track. Edit this field to change the track width within the range 0.001mil to 10000mil.
  • Start (X/Y) – displays the current X/Y coordinate of the track start point relative to the current origin.
  • End (X/Y) – displays the current X/Y coordinate of the track end point relative to the current origin.
  • Length – displays the current length of the track. Edit this field to change the track length within the range 0.001mil to 10000mil.

    Values can be defined in either mm or mil units. When entering a value in units other than the current units, add the mm or mil suffix to the value.

Paste Mask Expansion

  • Rule/Manual – select the desired paste mask expansion configuration. Select Rule to have the paste mask expansion for the track follow the defined value in the applicable Paste Mask Expansion design rule. Select Manual to override the applicable design rule and specify the paste mask expansion value for the track. You can then enable and enter the desired measurement.
To define or alter the value in the applicable Paste Mask Expansion design rule, visit the PCB Rules and Constraints Editor page.

Solder Mask Expansion

  • Rule/Manual – select the desired solder mask expansion configuration. Select Rule to have the solder mask expansion for the track follow the defined value in the applicable Solder Mask Expansion design rule. Select Manual to override the applicable design rule and specify the solder mask expansion value for the track. You can then enable and enter the desired measurement.
To define or alter the value in the applicable Solder Mask Expansion design rule, visit the PCB Rules and Constraints Editor page.

Two placed Arcs; on the left is a Full Circle Arc, on the right is an Arc selected for editing.
Two placed Arcs; on the left is a Full Circle Arc, on the right is an Arc selected for editing.

An arc is a primitive design object. It is essentially a circular track segment that can be placed on any layer. Arcs can have a variety of uses in PCB layout. For example, they can be used when defining component outlines on the overlay layers, or on a mechanical layer to indicate the board outline, edges of cutouts, and so on. They also can be used to produce curved paths while interactively routing. Arcs can be open or closed to create a circle (often referred to as a full circle arc).

Arcs are available for placement in both PCB and PCB Library Editors. There are four arc placement modes available (Center, Edge, Any Angle, and Full Circle). The way in which an arc is placed depends on the particular method of placement that you have chosen to invoke:

  • Place arc by center – this method enables you to place an arc object using the arc center as the starting point.

    After launching the command, the cursor will change to a cross-hair and you will enter arc placement mode. Placement is made by performing the following sequence of actions:

    1. Click or press Enter to anchor the center point of the arc.
    2. Move the cursor to adjust the radius of the arc then click or press Enter to set it.
    3. Move the cursor to adjust the start point for the arc then click or press Enter to anchor it.
    4. Move the cursor to change the position of the arc's end point then click or press Enter to anchor it and complete placement of the arc.
    5. Continue placing further arcs or right-click or press Esc to exit placement mode.
  • Place arc by edge – this method enables you to place an arc object using the edge of the arc as the starting point. The arc angle is fixed at 90°.

    After launching the command, the cursor will change to a cross-hair and you will enter arc placement mode. Placement is made by performing the following sequence of actions:

    1. Click or press Enter to anchor the start point for the arc.
    2. Move the cursor to change the position of the arc's end point then click or press Enter to anchor it and complete placement of the arc.
    3. Continue placing further arcs or right-click or press Esc to exit placement mode.
  • Place arc by edge (any angle) – this method enables you to place an arc object using the edge of the arc as the starting point. The angle of the arc can be any value.

    After launching the command, the cursor will change to a cross-hair and you will enter arc placement mode. Placement is made by performing the following sequence of actions:

    1. Click or press Enter to anchor the start point for the arc.
    2. Move the cursor to adjust the radius of the arc then click or press Enter to anchor the center point.
    3. Move the cursor to change the position of the arc's end point then click or press Enter to anchor it and complete placement of the arc.
    4. Continue placing further arcs or right-click or press Esc to exit placement mode.
  • Place full circle arc – this method enables you to place a 360° (full circle) arc.

    After launching the command, the cursor will change to a crosshair and you will enter arc placement mode. Placement is made by performing the following sequence of actions:

    1. Click or press Enter to anchor the center point of the arc.
    2. Move the cursor to adjust the radius of the arc then click or press Enter to set it and complete placement of the arc.
    3. Continue placing further arcs or right-click or press Esc to exit placement mode.

Additional actions that can be performed during placement are:

  • For all methods (excluding full circle arcs), press the Spacebar before defining the arc's end point to render the arc in the opposite direction.
  • Press the L key to flip the arc to the other side of the board – note that this is only possible prior to anchoring the arc's start/center point.
  • Press the + and - keys (on the numeric keypad) or use the Shift+Ctrl+Wheelroll shortcuts to cycle forward and backward through all visible layers in the design to change placement layer quickly.

This method of editing allows you to select a placed arc object directly in the design space and graphically change its size, shape or location.

When an arc object is selected, the following editing handles are available:

A selected Arc
A selected Arc

  • Click and drag A to adjust the radius.
  • Click and drag B to adjust the end points (start and end angles).
  • Click anywhere on the arc away from editing handles then drag to reposition it. Alternatively, click and drag on the arc center-point. While dragging, the arc can be rotated or mirrored:
    • Press the Spacebar to rotate the arc counterclockwise or Shift+Spacebar for clockwise rotation. Rotation is in accordance with the value for the Rotation Step, defined on the PCB Editor – General page of the Preferences dialog.
    • Press the X or Y keys to mirror the arc along the X-axis or Y-axis.

The Arc mode of the Properties.
The Arc mode of the Properties.

Location

The  icon to the right of this region must be displayed as  (unlocked) in order to access the below fields. Toggle the lock/unlock icon to change its lock status.
  • (X/Y)
    • X (first field) - this field shows the current X position of the center of the arc relative to the current origin. Edit the value in the field to change the position of the arc relative to the current origin. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the design space) and are used if the unit is not specified. 
    • Y (second field) - this field shows the current Y position of the center of the arc relative to the current origin. Edit the value in the field to change the position of the arc relative to the current origin. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. Default units (metric or imperial) are determined by the Units setting in the Other region of the Properties panel in Board mode (accessed when no objects are selected in the design space) and are used if the unit is not specified. 

Properties

  • Component – this field is shown in the PCB editor only when the selected Arc is a constituent part of a PCB Component and displays the designator of the parent PCB component. Select the clickable Component link to open the Component mode of the Properties panel for the parent component.
  • Net – use to choose a net for the arc. All nets for the active board design will be listed in the drop-down list. Note that if object placement commences at the same location as an existing object that is already connected to a net, then the Net property of the new object is automatically assigned to that net. Select No Net to specify that the arc is not connected to any net. The Net property of a primitive is used by the Design Rule Checker to determine if a PCB object is legally placed. Alternatively, you can click on the Assign Net icon () to choose an object in the design space - the net of that object will be assigned to selected arc(s).
  • Layer - this field displays the layer to which the arc is currently assigned. Arcs can be assigned to any available layer. To change the assigned layer, click the field and select a layer from the drop-down list. 
  • Width - this field displays the width of the arc line. Enter a different value for the width if required.
  • Radius - this field displays the radius of the arc measured from the center point to the center of the arc line. Enter a different value for the radius if required.
  • Start Angle - this field displays the start angle of the arc measured from the X-axis in the first quadrant (plane geometry). Enter a different value for the start angle if required.
  • End Angle - this field displays the end angle of the arc. Enter a different value for the end angle if required.
  • Propagation Delay - this field displays the time it takes for a signal to propagate along that route. 

Paste Mask Expansion

  • Rule - select to have the paste mask expansion for the arc follow the defined value in the applicable Paste Mask Expansion design rule. The associated expansion value will be disabled if this option is chosen.
  • Manual - select to override the applicable design rule and specify the paste mask expansion value for the arc in the field below. 

Solder Mask Expansion

  • Rule - select the checkbox to have the solder mask expansion for the arc follow the defined value in the applicable Solder Mask Expansion design rule. The associated expansion value will be disabled if this option is chosen.
  • Manual - select the checkbox to override the applicable design rule and specify the solder mask expansion value for the arc in the field below.

Placed Text objects
Placed Text objects

A Text object places a single-line string or multi-line text frame on the selected layer in a variety of display styles and formats including popular barcoding standards. It can be user-defined text or a special type of string, referred to as a special string that can be used to display board or system information or the value of user parameters on the board. The text frame is a re-sizeable rectangular area that can contain multiple lines of text and can automatically wrap and clip text to keep it within the bounds of the frame.

Text objects are available for placement in both PCB and PCB footprint editors by choosing the Place » String or Place » Text Frame command from the main menus. After launching the string placement command, the cursor will change to a cross-hair and you will enter text placement mode. A text object will appear floating on the cursor:

  1. Position the cursor then click or press Enter to place a text object.
  2. Continue placing further text objects or right-click or press Esc to exit placement mode.
Depending on the selected placement command (Place » String or Place » Text Frame), the Text object being placed will be in String or Frame mode that can be changed in the Properties panel during or after placement.

Additional actions that can be performed during placement are:

  • Press the Spacebar to rotate the text object counterclockwise or Shift+Spacebar for clockwise rotation. Rotation is in accordance with the value for the Rotation Step defined on the  PCB Editor – General page of the Preferences dialog.
  • Press the X or Y keys to mirror the text object along the X-axis or Y-axis.
  • Press the L key to flip the text object to the other side of the board.
  • Press the + and - keys (on the numeric keypad) to cycle forward and backward through all visible layers in the design to change placement layer quickly.

The graphical method of editing allows you to select a placed text object directly in the design space and change its location, rotation, orientation, and size.

When a text object is selected, the following editing handles are available:

A selected Text
A selected Text

  • Click and drag B to rotate the text object about its reference point A (denoted by the small x).
  • Click and drag C to resize the text object's bounding box in the vertical and horizontal directions simultaneously.
  • Click and drag D to resize the text object's bounding box in the vertical and horizontal directions separately.
  • Click anywhere on the text object away from editing handles and drag to reposition it. While dragging, the comment can be rotated or mirrored:
    • Press the Spacebar to rotate the text object counterclockwise or Shift+Spacebar for clockwise rotation. Rotation is in accordance with the value for the Rotation Step defined on the PCB Editor – General page of the Preferences dialog.
    • Press the X or Y keys to mirror the text object along the X-axis or Y-axis.
The default text for a newly-placed string object is String. Once placed (unless changed before or during placement), change this text as required using the text entry window when viewing the properties for the string through the Properties panel.

Special Strings

While text objects can be used to place user-defined text on the current PCB layer, it is not only user-defined text that can be placed. To assist in producing documentation, the concept of special strings is used. These act as placeholders for design, system or project information that is to be displayed on the PCB at the time of output generation.

Examples of design, system, and design parameter special strings shown as source strings (the first image) and converted (the second image). Examples of design, system, and design parameter special strings shown as source strings (the first image) and converted (the second image).
Examples of design, system, and design parameter special strings shown as source strings (the first image) and converted (the second image).

The special strings that are available in a PCB document come from a number of sources:

  • A default set of predefined special strings are provided for use with new PCB documents.
  • Custom special strings can be added by defining additional parameters at the project-level (these parameters are defined on the Parameters tab of the Project Options dialog) and at the variant-level (these parameters are defined in the Edit Project Variant dialog or in the Properties panel in its Variant mode in the Variant Manager).
  • User Parameters added to components in the schematic domain are transferred via an ECO to become available to PCB components. If a special string that refers to a component parameter is added to a PCB footprint at the source library level, that string will be interpreted on the target mechanical layer or overlay when the PCB component is placed.

Notes about Using Special Strings

  • A special string is denoted by the string starting with a . (dot) character (e.g. .Layer_Name.Net_Count, etc).  If a string starts with ".", the entire string is treated as a 'special' string. This syntax is also used when referencing a user-parameter, the parameter name is preceeded by the "." (dot) character.
  • To include more than one special string within a PCB text, enclose each special string within apostrophe ( ' ) characters; for example: '.Pcb_File_Name_No_Path' '.Print_Date'.
  • You can also use text, spaces and special characters between concatenated special strings, for example: FileName= '.Pcb_File_Name_No_Path' : PrintDate = '.Print_Date'.
  • Spaces and special characters can also be used within Project and Variant parameter names.
  • The values of some special strings can only be viewed when the relevant output is generated, including the .Legend, .Plot_File_Name, and .Printout_Name. Most special strings can be viewed on screen.

    When generating documentation for a PCB project and releasing into a Workspace, there needs to be some way of indicating which Item and Revision the documentation relates to, as well as the configuration of the design project used in the release and any applicable driving variant. A set of special strings are available to manage this, including .PCBConfigurationName, .ItemAndRevision, and .VariantName. These special strings are not interpreted until the time the output is generated (unless viewing the PCB in 3D, which itself is considered an output). The information supplied by using these strings can be seen on generated output including Gerber/ODB++ files, Final Artwork prints, PCB prints, PCB 3D prints, PCB 3D Video, and Assembly drawings.
  • Special strings are automatically converted for on-screen display. If the string cannot be converted either the value of the typed string, or a message will be displayed. For example, if the project is not under version control and the special string .VersionControl_RevNumber is placed on the PCB, the message Not in Version Control will be displayed.
  • To assist in identifying special strings, the View Configuration panel includes a Special Strings option. When the option is enabled, any placed text objects that are formed from converted special strings will be superimposed (labeled) with the unconverted special string name.

Placing a Special String

To use a special string on a PCB, place a text object then select one of the special string names from the Text field's drop-down (String mode) or the  drop-down (Frame mode) in the Properties panel.

Accessing special strings for a placed string object. Accessing special strings for a placed string object.
Accessing special strings for a placed string object.

The following are the predefined, system-based special strings available for use on a PCB document:

  • .Application_BuildNumber – the version of the software in which the PCB is currently loaded. When generating Gerber output, use this string to record the software build on which the design was created.
  • .Arc_Count – the number of arcs on the PCB.
  • .Comment – the comment string for a component (placed on any layer in the library editor as part of the component footprint).
  • .Component_Count – the number of components on the PCB.
  • .ComputerName – the name of the computer on which the software is installed and running.
  • .Designator – the designator string for a component (placed on any layer in the library editor as part of the component footprint).
  • .Fill_Count – the number of fills on the PCB.
  • .Hole_Count – the number of drill holes on the PCB.
  • .Item – the Item that the generated data relates to (e.g., D-810-2000). The data will be used to build that item.
  • .ItemAndRevision – the item and specific revision of that Item that the generated data relates to in the format <Item ID>-<Revision ID> (e.g., D-810-2000-01.A.1). The data will be used to build that specific revision of that particular item.
  • .ItemRevision – the specific revision of the Item that the generated data relates to (e.g., 01.A.1). The data is stored in that Item Revision within the target server.
  • .ItemRevisionBase – the Base Level portion of an Item Revision's naming scheme (e.g., 1).
  • .ItemRevisionLevel1 – the Level 1 portion of an Item Revision's naming scheme (e.g., A).
  • .ItemRevisionLevel1AndBase – the Level 1 and Base Level portions of an Item Revision's naming scheme (e.g., A.1).
  • .ItemRevisionLevel2 – the Level 2 portion of an Item Revision's naming scheme (e.g., 01).
  • .ItemRevisionLevel2AndLevel1 – the Level 2 and Level 1 portions of an Item Revision's naming scheme (e.g., 01.A).
  • .Layer_Name – the name of the layer on which the string is placed.
  • .Legend – a symbol legend for mechanical drill plots. This string is only valid when placed on the Drill Drawing layer. Note: this is a legacy feature; place a Drill Table object for more detailed drill information.
  • .ModifiedDate – the modified date stamp of the PCB; it is automatically populated. Example: 23/09/2015.
  • .ModifiedTime – the modified time stamp of the PCB; it is automatically populated.
  • .Net_Count – the total number of different nets on the PCB.
  • .Net_Names_On_Layer – the names of all nets on the specific layer. This string is only valid when placed on an internal plane layer.
  • .Pad_Count – the number of pads on the PCB.
  • .Pattern – the names of the component footprints used on the PCB.
  • .Pcb_File_Name – the path and file name of the PCB document.
  • .Pcb_File_Name_No_Path – the file name of the PCB document.
  • .PCBConfigurationName – the name of the data set from which the output has been generated as defined in the Release view (Project Releaser).
  • .Plot_File_Name – for generated Gerber output, this string identifies the file name of the Gerber plot file. For printed output, it identifies the layer depicted within the output. For ODB++ output, it identifies the name of the parent folder in which the files are stored.
  • .Poly_Count – the number of polygons on the PCB (consisting of polygon pours, internal planes and split planes).
  • .Print_Date – the date of printing/plotting.
  • .Print_Scale – the printing/plot scale factor.
  • .Print_Time – the time of printing/plotting.
  • .Printout_Name – the name of the printout.
  • .Project - project name.
  • .ProjectRev - project revision.
  • .SlotHole_Count – the number of slotted holes on the PCB.
  • .SquareHole_Count – the number of square holes on the PCB.
  • .String_Count – the number of strings on the PCB.
  • .Total_Thickness – the thickness of the board.
  • .Total_Thickness(Board Layer Stack) – the thickness of the board layer stack.
  • .Track_Count – the number of tracks on the PCB.
  • .VariantName - the variant of the design from which the output has been created.
  • .VersionControl_PrjFolderRevNumber – the current revision number of the project, which is incremented whenever a full commit of the project (i.e., including the project file) is performed. Version control must be used for this string to contain any information.
  • .VersionControl_ProjFolderRevNumber – the current revision number of the project, which is incremented whenever a full commit of the project (i.e., including the project file) is performed. Version control must be used for this string to contain any information.
  • .VersionControl_ProjFolderRevNumberShort – a short Git hash format (the first eight characters) of the Project. Version control must be used for this string to contain any information.
  • .VersionControl_RevNumber – the current revision number of the document. Version control must be used for this string to contain any information.
  • .VersionControl_RevNumberShort – a short Git hash format (the first eight characters) of the current revision number of the document. Version control must be used for this string to contain any information.
  • .Via_Count – the number of vias on the PCB.
The full list of special strings available will also include any derived from user-defined project-level parameters.
The software provides the ability to place Text objects as barcode symbols directly onto a PCB on any layer, allowing barcodes to be easily imprinted on a PCB as part of the manufacturing process. To learn more about using a Text object as a barcode, see the Adding a Barcode section of the Including Barcodes & Logos page.

The Text mode of the Properties
The Text mode of the Properties

Location

The  icon to the right of this region must be displayed as  (unlocked) in order to access the below fields. Toggle the lock/unlock icon to change its lock status.
  • (X/Y)
    • X (first field) - the current X (horizontal) coordinate of the reference point of the text object, relative to the current design space origin. Edit to change the X position of the text object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default.
    • Y (second field) - The current Y (vertical) coordinate of the reference point of the text object, relative to the current origin. Edit to change the Y position of the text object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default.
  • Rotation - specify the rotation of the text object. The minimum angular resolution is 0.001 degrees.

Properties

  • Use the String and Frame buttons to switch between single- and multi-line text editing modes:

    • String

      • Text - enter the desired text. Use the field's drop-down to access the list of available special strings. Refer to the list of predefined special strings above for a list of special strings and descriptions of each.

    • Frame

      • Text - enter the desired text. Click  to access a drop-down from which you can select the type of special string(s) to add if desired. Refer to the list of predefined special strings above for a list of special strings and descriptions of each.

        Use Shift+Enter to add a new line.
  • Layer - use the drop-down to select the desired layer. Enable Mirror if desired.
  • Text Height - specify the height of the string.

Font Type

  • TrueType - select to use fonts available on your PC (in the \Windows\Fonts folder). TrueType fonts offer full Unicode support. By default, the software links to a used TrueType font (they are not stored in the PCB file), which means the same font must be present on each PC to which the design is moved. Alternatively, embed used TrueType fonts in the PCB file using the options in the PCB Editor - True Type Fonts page of the Preferences dialog, where you can also select a Substitution Font to be used if a non-embedded Font is not available.
    • Justification - use these controls to set the horizontal and vertical alignment of the text.
    • Font - use the drop-down to select the desired TrueType font. Use the B (bold) and/or I (italic) options to add emphasis to the text as required.
    • Inverted - enable to have the text displayed as inverted with control over the size of the border around the text (using the associated Width and Height fields that become available).
  • Stroke
    • Justification - use these controls to set the horizontal and vertical alignment of the text.
    • Font - use the drop-down to select the desired Stroke font. Choices are:
      • Default - a simple vector font designed for pen plotting and vector photo plotting.
      • Sans Serif - a complex font that will slow down vector output generation, such as Gerber.
      • Serif - a complex font that will slow down vector output generation, such as Gerber.
    • Stroke Width - displays the width of the stroke.
  • BarCode - used to tag and identify PCBs, streamlining inventory tracking, for example, through the use of automated scan machines.
    • Type - select one of the following bar code types:
      • Code 39 - the US Department of Defense standard; often referred to as Code 3 of 9. It is also used in the automotive industry.
      • Code 128 - the global trade identification standard; supports any of the ASCII 128 character set (all digits, character, and punctuation marks).
    • Render Mode - choose a render mode for barcode display: Min Single Bar Width or Full BarCode Width.
      • Full Width - specify the overall width of the bar code. This option is not available if Min Single Bar Width is selected.
      • Full Height - specify the overall height of the bar code.
      • Min Width - specify the minimum width of the bar code. This field is not available if Full BarCode Width is selected.
      • Horizontal Margin - this field defines the size of the margin on the left and right edges.
      • Vertical Margin - this field defines the size of the margin on the top and bottom edges.
      • Font Name - use the drop-down to select the font.
        • Show Text - enable to display the actual text string from which the barcode is derived (i.e. the string entered in the Text field).
        • Inverted - when enabled, the bars are inverted and a border is added on all four sides.
    Learn more about Adding a Barcode.
  • Border Mode
    • Margin - click this button to enable the editing of the Margin Border option.
      • Text Offset - the amount the designator is offset back from the edge/corner that it is justified against. This option has no effect when the Center justification mode is chosen. This option is not available for Margin.
    • Offset - click this button to enable the editing of the Text Offset option.
      • Margin Border - use to specify the size of the margin border surrounding the designator. This option is not available for Offset.
When the string is selecting, a bounding box will appear, containing a small (x) on the bounding handle.

Group Objects

A group object is any set of primitives that has been defined to behave as an object. These may be user-defined, such as components and polygon pours, or system-defined, such as coordinates and dimensions. A group object can be manipulated as a single object within the design space. For example, it can be placed, selected, copied, changed, moved, and deleted.

Group objects are available for placement in the PCB Editor with the coordinate object also supported for placement in the PCB Library Editor. Commands for placement can be found in the main Place menu, as well as the Wiring toolbar, and various drop-downs of the Utilities toolbar. Depending on the object, placement may require several mouse clicks to define the object's appearance.

Objects are placed on the current layer. Ensure the correct layer has been made the current layer before effecting placement. An object can be changed with respect to the layer on which it resides after placement.

The component footprint defines the component mounting and connections on the PCB and can also include 3D body objects to define the actual component. The component footprint defines the component mounting and connections on the PCB and can also include 3D body objects to define the actual component.
The component footprint defines the component mounting and connections on the PCB and can also include 3D body objects to define the actual component.

The component footprint defines the space and connection points needed to mount the physical component on the printed circuit board. It is a group object made up of a collection of simple primitive objects, which could include pads, lines and arcs, as well as other design objects. The pads provide the mounting and connection points for the component pins. Additional design primitives, such as lines and arcs, are often included to define the outline of the component shape on the component overlay (silkscreen) layer.

The component footprint can also include optional 3D body objects, which define the physical space or envelope of the actual component that is mounted on the board. If the physical component has been defined using 3D body objects or imported STEP models, three-dimensional component clearance checking can be performed.

Component footprints are created in the PCB Library Editor by placing suitable design objects to create the shape required to mount and connect the component. The component reference point is the origin of the Library Editor design space, which can be set in the Library editor to: pin 1, the geometric center, or a user-defined location on the component.

To learn more about footprint creation, refer to Creating a PCB Footprint.

Availability

Component footprints are created in the PCB Library editor and placed in the PCB editor. PCB component footprints are automatically placed from the available libraries when the design is transferred from the schematic editor to the PCB editor. This is called Design Synchronization, which is a process to detect and resolve the differences between the schematic and the PCB.

Alternatively, a component can be placed directly in the PCB editor. To do this:

  1. Click Place » Component. If it is not active, the Components panel will open ready to locate the component required for placement.
  2. Select the component in the Components panel (View » Panels » Components), right-click then select Place <ComponentName>.
PCB component footprints (and schematic components) can only be placed from the connected Workspace or available libraries. The term 'available libraries'  includes libraries that are part of the current project being worked on, or libraries currently installed in Altium Designer. Libraries can be installed and removed via the Data Management - File-based Libraries page of the Preferences dialog or the Available File-based Libraries dialog (click the  button in the Components panel then select File-based Libraries Preferences from the drop-down).

Placement

The process used to locate the required component footprint will depend on the method chosen to perform placement. Once the required footprint has been chosen for placement and is floating on the cursor:

  1. Press Tab to edit the properties of the component before it is placed.
  2. Press Spacebar to rotate the component counterclockwise (Shift+Spacebar for clockwise). The default rotation step is 90 degrees. To change this setting, use the Rotation Step value in the PCB Editor - General page of the Preferences dialog.
  3. If the component is being rotated, the Designator and Comment strings can be configured to hold their orientation, or to rotate with the footprint. This behavior is controlled by the Autoposition setting for these strings. The defaults can be set by editing the default Component on the PCB Editor - Defaults page of the Preferences dialog. Note that setting the default will not affect any components that have already been placed.
  4. Press the L shortcut to flip the component to the bottom side of the board. Do not use the X or Y keys as this will mirror the part but not change its layer.
While attributes can be modified during placement (Tab to bring up associated properties panel), keep in mind that these will become the default settings for further placement unless the Permanent option on the PCB Editor – Defaults page of the Preferences dialog is enabled. When this option is enabled, changes made will affect only the object being placed and subsequent objects placed during the same placement session.

Placing From the Components Panel

To place from the Components panel:

  1. To enable desired components in the panel, connect to an available Workspace or click  then select File-based Libraries Preferences from the drop-down to open the Available File-based Libraries dialog. Use the dialog to add (on the Project tab) or select (on the Installed tab) a library.
  2. Once footprint libraries have been enabled, the Components panel will refresh with the available components for that library.
Click  then select File-based Libraries Search to open the File-based Libraries Search dialog to search for available libraries.

With the part selected in the panel, placement of the component can be made in the following ways:

  • Right-click then select Place <ComponentName> from the context menu.
  • Double-click on the selected component. The component will appear floating in the design space. Place the component in the desired location then click to place.
  • Click and hold the component's name in the Components panel then drag the component to the desired location and click to place it. This is a 'single shot' placement technique, meaning only a single instance of the chosen component can be placed. The other methods allow multiple instances to be placed.
The Components panel also includes a Search feature that can search across available libraries or all libraries in a folder path. Refer to the Components panel page for more information.

Graphical Editing

Graphical component editing is limited to moving, rotating, and flipping. When a component is selected in the design space it is highlighted in the current selection color as shown in the image below. To graphically manipulate a selected component:

  • Press Delete to remove the selected component from the design.
  • Click, hold and drag to move the selected component. The cursor will jump to the component reference point, or the nearest pad center if the Smart Component Snap option is enabled on the PCB Editor - General page of the Preferences dialog.
  • While a component is moving on the cursor press the Spacebar to rotate it (Shift+Spacebar to rotate in the other direction).
  • While a component is moving on the cursor press the L key to flip it to the other side of the board.

Click once to select a component or click, hold and drag to move it.Click once to select a component or click, hold and drag to move it.

To learn more about component placement, refer to Component Placement.
If attempting to graphically modify an object that has its Locked property enabled, a dialog will appear asking for confirmation to proceed with the edit. If the Protect Locked Objects option is enabled on the PCB Editor – General page of the Preferences dialog and the Locked option for that design object is enabled as well, that object cannot be graphically edited. Double-click the locked object to select it then disable the Locked property in the Properties or List panel or disable the Protect Locked Objects option to graphically edit the object.

Component Selection

When you click and select a component, the selection bounding box appears. Traditionally, the default bounding box behavior has been to use the smallest rectangle that encloses all of the primitives in that component, excluding the designator and comment strings.

To provide better support for more complex component shapes, the PCB.ComponentSelection Advanced Setting was added (click Advanced Settings on the System – General page of the Preferences dialog). This option gives the designer control over which layers are used to define the bounding box. After changing the PCB.ComponentSelection value in the Advanced Settings dialog, you will need to restart Altium Designer in order for the change to take effect.

The advanced option supports three modes (enter the value 0, 1 or 2; the default mode is 2):

  • 0 - legacy mode - this mode combines geometries from all layers, except the Silkscreen Designator and Comment strings.
  • 1 - by layer mode - use the geometries from the first of the layers listed below that contains objects, with the following priority:
    1. Courtyard Layer Type
    2. 3D Body Layer (STEP models are stored in a 3D Body object sized to the smallest rectangular prism that holds the model. This 3D Body is used, not the shape of the STEP model)
    3. Silkscreen Layer plus Copper Layers
    4. Copper Layers
  • 2 - by graphic mode - this mode combines geometries on the Courtyard Layer Type, the Silkscreen, 3D Body objects and Copper layers. Strings are excluded.

0 - legacy

1 - by layer

2 - by graphic

  • References to the Courtyard layer are for a Component Layer Pair with the Layer Type = Courtyard, the name of the layer pair is not considered.

  • If the component includes a 3D model the actual 3D model shape is used for component collision checking, while the shape of the component selection box is determined as described above.
  • Mechanical layer objects are excluded from the selection bounding box but are included in the collision checking bounding box when there are no 3D Bodies or Courtyard layer objects defined. The exceptions to this are the .Designator and .Comment text strings, which are always excluded. Learn more about Working with Mechanical Layers.
  • The component selection bounding box is used to calculate the component area, learn more about the component area.

Accessing Clickable Links to Reference Information

When named document links have been added to the component, the indicated document/page URL - specified through a defined underlying URL link parameter - for the selected component or the component under the cursor can be opened. This feature allows named document links that have been transferred from schematic components to be presented as named PCB component links to PDFs, text files, or HTML pages. That occurs when the named document links for the component have been updated from the Schematic to the PCB (Design » Update PCB Document). During that update process (via an ECO), the schematic named document links are converted to ComponentLink parameter pairs (ComponentLinknDescription/ComponentLinknURL) for the matching PCB component. For example:

Schematic Component Parameter   PCB Component Parameters
Name Url

 

Name Value
STM32 Family Web Page http://www.st.com/stm32 ComponentLink1Description STM32 Family Web Page
ComponentLink1URL http://www.st.com/stm32

The link index number (n) used in the component parameters will define the ordered position of the matching PCB Component Link in the References submenu. With a component on the PCB selected, the defined ComponentLink parameter pairs are presented in the Parameters section of the Properties panel.

After launching the command, the web-based URL target page or indicated document will open directly (if available).

  • A web-based URL will be open either in an external browser, or as a tabbed document within Altium Designer, as determined by the Open internet links in external Web browser option, on the System - View page of the Preferences dialog. Bear in mind that to open in an external browser, the value (URL) of the link parameter must include the http:// prefix.
  • For more information about establishing document link parameters in the schematic space, see Defining Clickable Links to Reference Information.

Adding Primitives to a Component

Selected primitives can be added to a component by choosing the Tools » Convert » Add Selected Primitives to Component command from the main menus. After selecting a command, choose the component to which you want to add the selected primitives. When confirmed, the new primitives will be recognized as part of the single component object and may be used in conjunction with the component's original primitives.

The target component must have its primitives unlocked to carry out this operation. Use the Primitives lock icon in the component's properties to unlock component primitives.

Exploding a Component to Primitives

A component can be converted to its constituent primitive objects using the Tools » Convert » Explode Component to Free Primitives command from the main menus or by right-clicking over a placed component (selected or not) then choosing the Component Actions » Explode Component To Free Primitives (or Explode Selected Components To Free Primitives) command from the context menu. An exploded component is no longer a component, so the designator and comment will be removed and the component will revert to the various primitives from which it was made.

Explode has no effect on the footprint model stored in the applicable source library, only on the converted instance(s) of the component(s) placed on the PCB document.

  • Explode is a one-way process, there is no command to regroup an exploded component. You can use the Undo command to achieve this.
  • The Explode command should not be used to modify the properties of a component. The primitives in a component can be edited by unlocking the component primitives (using the Primitives lock icon in the component's properties), editing them as required, then re-locking the primitives.

The Component mode of the Properties panel.
The Component mode of the Properties panel.

General Tab

Location

The  icon to the right of this region must be displayed as  (unlocked) in order to access the below fields. Toggle the lock/unlock icon to change its lock status.
  • (X/Y)
    • X (first field) – the current X (horizontal) coordinate of the reference point of the component, relative to the current design space origin. Edit to change the X position of the component. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. The reference point for a component footprint is set in the Library Editor.
    • Y (second field) – The current Y (vertical) coordinate of the reference point of the component, relative to the current origin. Edit to change the Y position of the component. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. The reference point for a component footprint is set in the Library Editor.
  • Rotation – the component's angle of rotation (in degrees), measured counterclockwise from zero (the 3 o'clock horizontal). Edit to change the rotation of the component. Minimum angular resolution is 0.001°.

    Use the Tools » Optimize Component Rotation command from the main menus to optimize component rotation from 360 to 0 degrees.

Properties

  • Layer – sets the layer on which the component is placed. Components can be assigned to the Top layer or Bottom layer. Use the drop-down to select a different layer. Changing the layer status swaps all of the component primitives to each layer's respective opposite layer. For example, moving a Top layer component to the Bottom layer means: single layer pages are swapped from the Top to the Bottom layer, primitives on the Top Overlay are reassigned to the Bottom Overlay, and primitives on a paired mechanical layer are swapped to the other mechanical layer in that pair. The orientation of the component will be flipped along the X-axis and the component overlay text will read from the bottom.
  • Reuse Block – when the component is a part of a reuse block, this field shows the name of the parent reuse block. Click the Reuse Block hyperlink to see the properties of this reuse block.
  • Designator – the designator of the component is an alphanumeric string of up to 255 characters. Each component must have a unique Designator string. Toggle  or  to show/hide the designator. Click the Designator hyperlink to open the properties of the component's designator.
  • Comment – the comment of the component is an alphanumeric string of up to 255 characters. Toggle  or  to show/hide the comment. Click the Comment hyperlink to open the properties of the component's comment.
  • Area – the area of the placed component, displayed in the current board units. The area can be user-defined, if it is not it is automatically calculated from the component's selection area:
    • To define the component area, edit the Area in the PCB Library Footprint dialog in the PCB library editor. To push an updated footprint to an open PCB, right-click on the footprint name in the PCB Library panel then select Update PCB With <ComponentName> from the context menu.
    • You can also user-define the area of a component already placed on a PCB by selecting the component then entering the value in this field.
    • To switch from a user-defined area to a calculated area for a component placed on a PCB, delete the value in this field; the field will automatically be re-populated with the auto-calculated value.
    • The automatically calculated area is the area that highlights when you click to select the component. The selection area is determined from the geometries on the Courtyard layer, i.e. when that layer is not present, the combination of the geometries on the Silkscreen, 3D Body objects, and Copper layers (strings are excluded). The upper images displayed below show the component's area when there is an outline defined on the courtyard layer; the lower image shows the area when it is calculated from the geometries on the Silkscreen, 3D Body objects, and Copper layers.

      • The edge of the Courtyard is the centerline of the outline tracks and arcs that form the Courtyard boundary.
      • A curved component Courtyard shape can be created using arcs, as shown in the upper of the images above, where the Courtyard curves around pad 3.

      Learn more about how the selection area is calculated, and the other modes available to determine the selection area.

      Learn more about Working with Mechanical Layers.

  • Description – enter the desired description.
  • Type – select one of the following component types for the component footprint here. The available types are:
    • Standard – these components possess standard electrical properties, are always synchronized between the schematic and PCB (the footprint, pins/pads and net assignments must all match), and are included in the BOM. An example is a standard electrical component, such as a resistor.
    • Mechanical – these components do not have electrical properties, are not synchronized (you must manually place them in both editors), and are included in the BOM. An example is a heatsink.
    • Graphical – these components do not have electrical properties, are not synchronized (you must manually place them in both editors), and are not included in the BOM. An example is a company logo.
    • Net Tie (in BOM) – these components are used to short two or more different nets together. They are always synchronized between the schematic and PCB (the footprint, pins/pads and net assignments must all match), and are included in the BOM. They differ from a Standard component in that connectivity created by copper within the footprint is not checked – it is this copper that allows the nets to be shorted. Note: enable the Verify Shorting Copper option in the Design Rule Checker dialog to verify that there is no unconnected copper within the component.
    • Net Tie – these components are used to short two or more different nets together. They are always synchronized between the schematic and PCB (the footprint, pins/pads and net assignments must all match), and are not included in the BOM. They differ from a Standard component in that connectivity created by copper within the footprint is not checked – it is this copper that allows the nets to be shorted. Note: enable the Verify Shorting Copper option in the Design Rule Checker dialog to verify that there is no unconnected copper in the component.
    • Standard (No BOM) – these components possess standard electrical properties, are always synchronized between the schematic and PCB (the footprint, pins/pads and net assignments must all match), and are not included in the BOM. An example is a testpoint component that you wish to exclude from the BOM.
    • Jumper – these components are used to include wire links in a PCB design, for example, on a single-sided PCB that cannot be fully routed on one layer. For this component type, the component footprint and pins are synchronized between the schematic and PCB but the net assignments are not, and the component is included in the BOM. As well as selecting this option at the component level, both of the pads in the component must have their JumperID set to the same non-zero value. Jumper-type components do not need to be wired on the schematic; they only need to be included on the schematic if they are required in the BOM. If they are not required in the BOM, they can be placed directly in the PCB where the Component Type is set, the JumperIDs are set, and the Nets manually assigned for the pads.
  • Design Item ID – displays the Design Item ID for the selected component. This field is not editable.
  • Source – displays the source document of the component. Click to open a dialog to browse and select a different source document.
  • Revision State – shows the state of the revision of the Workspace library component in terms of its lifecycle state and also its revision status, i.e. whether it is the latest released revision of that component (Up to date) or is an earlier revision (Out of date).

    For information on how to update Workspace library components, see Component Management with a Connected Workspace.
    When connected to an Altium 365 Workspace, note that configuration and use of lifecycle definitions is not supported with the Altium Designer Standard Subscription. As such, the Revision State field will not be available.
  • Height – a height field for the component, this field was used before the introduction of the 3D Body object, which provides a superior method of defining the component height.
  • 3D Body Opacity – enter the desired opacity percentage or use the slider bar.
  • Primitives – click the associated lock icon to lock/unlock.  – lock all the primitives of the component so that it can be treated as a single object. – unlock to modify the individual primitives that make up the component. After editing, the component primitives should be re-locked. Note: Component pad properties can be accessed without unlocking the primitives by double-clicking directly on the pad.

    Note that when component primitives are locked, the most of properties of these primitives cannot be modified by graphical (e.g. using drag-and-drop) and non-graphical (e.g. using the Properties or a List panel) editing methods.
  • Strings – click the associated lock icon to lock/unlock.  – lock all the strings of the component. – unlock to modify the strings of the component.
Select the clickable links of the Designator and Comment from the Component mode of the Properties panel to be redirected to those objects' respective Properties panels where you may edit their options.

Footprint

  • Footprint Name – displays the name of the footprint corresponding to the chosen component.
  • Design Item ID – the identification of the chosen component.
  • Source – displays the name of the Workspace in which the chosen component has been placed.
  • Description – displays the description of the component, which can also be seen in the Components panel.

Swapping Options

  • Enable Pin Swapping – check to allow the pin swapping function.
  • Enable Part Swapping – check to allow the part swapping function (e.g., four parts of a 74 series IC).

Schematic Reference Information

Schematic reference information is transferred from the schematic to the PCB editor when the design is initially transferred. To refresh this data at a later stage, click the Perform Update button in the Edit Component Links dialog.
  • Designator – the designator of the schematic component to which this PCB component has been matched.
  • Hierarchical Path – displays where, in the hierarchical structure of the schematic, this component can be found.
  • Channel Offset – when a design is first transferred from schematic to PCB, each component on each schematic sheet is given a unique channel offset.

Parameters Tab

  • Table – displays the Name, Value, and Source of each listed parameter.

The designator and comment fields are a child parameter object of a PCB component (part). The designator is used to uniquely identify each placed part to distinguish it from all other parts placed in all the PCB documents in the project. The comment is used to add additional information to a placed object. Both comment and designator are configured after the parent component part object is placed. It is not a design object that you can directly place.

A placed Designator object
A placed Designator object

A placed Comment object
A placed Comment object

PCB 2D/3D component designators will auto-increment by one during placement if the initial component has a designator ending with a numeric character. Change the designator of the first component prior to placement from the Properties panel.

To achieve alpha or numeric designator increments other than 1, use the Paste Array feature. Controls for this feature are provided in the Setup Paste Array dialog, accessed by pressing the Paste Array button in the Paste Special dialog (Edit » Paste Special).

The graphical method of editing allows you to select a placed designator or comment object directly in the design space and change its location, rotation, orientation, and size.

When a designator or comment object is selected, the following editing handles are available:

A selected Designator
A selected Designator

  • Click and drag B to rotate the designator/comment about its reference point A (denoted by the small x).
  • Click and drag C to resize the designator's/comment's bounding box in the vertical and horizontal directions simultaneously.
  • Click and drag D to resize the designator's/comment's bounding box in the vertical and horizontal directions separately.
  • Click anywhere on the designator/comment away from editing handles and drag to reposition it. While dragging, the comment can be rotated or mirrored:
    • Press the Spacebar to rotate the designator/comment counterclockwise or Shift+Spacebar for clockwise rotation. Rotation is in accordance with the value for the Rotation Step defined on the PCB Editor – General page of the Preferences dialog.
    • Press the X or Y keys to mirror the designator/comment along the X-axis or Y-axis.

The properties of a Designator or Comment object can be modified in the Parameter mode of the Properties panel.

The Tools » Add Designators for Assembly Drawing command from the main menus can be used to automatically add and update assembly component designators on the Designator Component Layer Pair within the PCB document. After launching the command, a dialog will appear displaying the total number of assembly component designators that were added/updated. If the PCB document does not include the Designator Component Layer Pair, a dialog will open suggesting adding the Component Layer Pair.

The Parameter mode of the Properties panel.
The Parameter mode of the Properties panel.

Location

  • (X/Y) 
    • X (first field) - the current X (horizontal) coordinate of the reference point of the designator, relative to the current workspace origin. Edit to change the X position of the designator. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. 
    • Y (second field) - The current Y (vertical) coordinate of the reference point of the designator, relative to the current origin. Edit to change the Y position of the designator. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default. 
  • Rotation - the designator's angle of rotation (in degrees) measured counterclockwise from zero (the 3 o'clock horizontal). Edit to change the rotation of the designator. Minimum angular resolution is 0.001°.

Properties

  • Parameter type - displays the type of parameter (Component, Sheet Symbol, etc.,) and parameter name.
  • Name - the name of the designator.
  • Value - use this field to enter the desired value of the designator. Click the eye icon to toggle the value between being visible and not visible in the design space.

    The display of the designator or comment can be toggled between not hidden and hidden for a placed component by right-clicking the component in the design space and choosing the Component Actions » Hide Designator / Component Actions » Show Designator or Component Actions » Hide Comment / Component Actions » Show Comment command, respectively, from the context menu.
  • Layer - use the drop-down to select the desired layer. Enable Mirror if desired.
  • Autoposition - use the drop-down to select the desired automatic position in relation to the associated object.
  • Text Height - use this field to enter the desired text height.
  • Font Type 
    • TrueType - select to use fonts available on your PC (in the \Windows\Fonts folder). TrueType fonts offer full Unicode support. By default, the software links to a used TrueType font (they are not stored in the PCB file), which means the same font must be present on each PC to which the design is moved. Alternatively, embed used TrueType fonts in the PCB file using the options in the PCB Editor - True Type Fonts page of the Preferences dialog, where you can also select a Substitution Font to be used if a non-embedded Font is not available.
      • Justification - use to set the location of the designator within the border rectangle.
        • Left () - click the left button to align the horizontal text on the left.
        • Center () - click the center button to align the horizontal text in the center.
        • Right () - click the left button to align the horizontal text on the right.
        • Above () - click the above button to align the vertical text above.
        • Middle () - click the middle button to align the vertical text in the middle.
        • Below () - click the below button to align the vertical text below.
      • Font - use the drop-down to select the desired TrueType font. Use the (bold) and/or I (italic) options to add emphasis to the text as required. 
        • Inverted - use to have the text displayed as inverted with control over the size of the border around the text. You can use the following options to further configure the text:
          • Size (Width/Height) -
            • Width - the width of the border rectangle.
            • Height - the height of the border rectangle.
    • Stroke
      • Justification - use to set the location of the designator within the border rectangle.
        • Left () - click the left button to align the horizontal text on the left.
        • Center () - click the center button to align the horizontal text in the center.
        • Right () - click the left button to align the horizontal text on the right.
        • Above () - click the above button to align the vertical text above.
        • Middle () - click the middle button to align the vertical text in the middle.
        • Below () - click the below button to align the vertical text below.
      • Font - use the drop-down to select the desired Stroke font. Choices are:
        • Default - a simple vector font designed for pen plotting and vector photo plotting. 
        • Sans Serif - a complex font that will slow down vector output generation, such as Gerber.
        • Serif - a complex font that will slow down vector output generation, such as Gerber.
      • Stroke Width - displays the width of the stroke.
  • Border Mode
    • Margin - click this button to enable the editing of the Margin Border option.
      • Text Offset - the amount the designator is offset back from the edge/corner that it is justified against. This option has no effect when the Center justification mode is chosen. This option is not available for Margin.
    • Offset - click this button to enable the editing of the Text Offset option.
      • Margin Border - use to specify the size of the margin border surrounding the designator. This option is not available for Offset.

A placed Rectangle
A placed Rectangle

A rectangle can be placed on any layer. Rectangles of varying sizes can be combined to cover irregularly shaped areas and can also be combined with track or arc segments and be connected to a net.

Rectangles also can be placed on non-electrical layers. For example, place a rectangle on the Keep-Out layer to designate a 'no-go' area for auto-routing. Place a rectangle on a Power Plane, Solder Mask, or Paste Mask layer to create a void on that layer. 

Availability

Rectangles are available for placement in both the PCB and PCB library editors in the following ways:

  • PCB Editor - the following methods of access are available:
    • Choose Place » Rectangle from the main menus.
    • Click the Rectangle button () in the drop-down on the Active Bar located at the top of the design space. (Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the topmost item on that section of the Active Bar.)
    • Right-click in the design space then click Place » Rectangle from the context menu.
  • PCB Library Editor - the following methods of access are available:
    • Choose Place » Rectangle from the main menus.
    • Click the Rectangle button () in the drop-down on the Active Bar located at the top of the design space. (Click and hold an Active Bar button to access other related commands. Once a command has been used, it will become the topmost item on that section of the Active Bar.)
    • Right-click in the design space then select Place » Rectangle from the context menu.

Placement

After launching the command, the cursor will change to a cross-hair and you will enter rectangle placement mode. Placement is made by performing the following sequence of actions:

  1. Click or press Enter to anchor the first corner of the rectangle.
  2. Move the cursor to adjust the size of the rectangle then click or press Enter to anchor the diagonally-opposite corner and complete placement of the rectangle.
  3. Continue placing further rectangles or right-click or press Esc to exit placement mode.

Additional actions that can be performed during placement are:

  • Press the Tab key to pause the placement and access the Rectangle mode of the Properties panel in which its properties can be changed on the fly. Click the design space pause button overlay () to resume placement.
  • Press the Spacebar to cycle through the various corner modes. Select Rectangle for straight corners, Fillet for rounded corners, or Chamfer for sloped/angled corners. 
  • Press the + and - keys (on the numeric keypad) to cycle forward and backward through all visible layers in the design to change the placement layer quickly.
  • Press and hold the Alt key to constrain the direction of movement to the horizontal or vertical axis depending on the initial direction of movement. 
While attributes can be modified during placement (Tab to open the Properties panel), keep in mind that these will become the default settings for further placement unless the Permanent option on the PCB Editor – Defaults page of the Preferences dialog is enabled. When this option is enabled, changes made will affect only the object being placed and subsequent objects placed during the same placement session.

Graphical Editing

This method of editing allows you to select a placed rectangle object directly in the design space and change its size, shape, or location graphically.

When a rectangle object is selected, the following editing handles are available.

A selected rectangle A selected rectangle

  • Click and drag the corners to resize the rectangle in the vertical and horizontal directions simultaneously.
  • Click and drag the centers of the sides to resize the rectangle in the vertical and horizontal directions separately.
  • Click anywhere on the rectangle away from editing handles and drag to reposition it. While dragging, the rectangle can be rotated or mirrored:
    • Press the Spacebar to rotate the rectangle counterclockwise or Shift+Spacebar for clockwise rotation. Rotation is in accordance with the value for the Rotation Step defined on the PCB Editor – General page of the Preferences dialog.
    • Press the X or Y keys to mirror the rectangle along the X-axis or Y-axis.
To convert a Rectangle object to its original set of primitive parts, choose the Tools » Convert » Explode Rectangle to Free Primitives command from the main menus. Although there is no actual command to regroup an exploded rectangle, you can use the Undo command to achieve this.

The Rectangle mode of the Properties panel.
The Rectangle mode of the Properties panel.

Location

The lock icon to the right of this region must be displayed as unlocked in order to access the below fields. Toggle the lock/unlock icon to change its lock status. 
  • (X/Y) 
    • X (first field) - the current X (horizontal) coordinate of the reference point of the rectangle, relative to the current design space origin. Edit to change the X position of the rectangle. The value can be entered in either metric or imperial, include the units when entering a value whose units are not the current default. 
    • Y (second field) - The current Y (vertical) coordinate of the reference point of the rectangle, relative to the current origin. Edit to change the Y position of the fill. The value can be entered in either metric or imperial, include the units when entering a value whose units are not the current default. 
  • Rotation - the rectangle's angle of rotation (in degrees), measured counterclockwise from zero (the 3 o'clock horizontal). Edit to change the rotation of the rectangle. The minimum angular resolution is 0.001°.

Properties

  • Corner Mode - use the drop-down to select the desired corner mode of the rectangle from the following options: 
    • Rectangle - specifies that the placed rectangle will have square corners. 
    • Fillet - specifies that the placed rectangle will have rounded corners. 
    • Chamfer - specifies that the placed rectangle will have sloped or angled corners. 
The corner mode can also be chosen during placement by pressing the Spacebar.
  • Track Width - displays the current width of the track. Edit this field to change the track width within the range 0.001mil to 10000mil.
  • Fillet/Chamfer Size - this is available only when Fillet or Chamfer is selected from the Corner Mode drop-down or if fillet or chamfer mode was chosen during placement.
  • Layer - the layer to which the rectangle is currently assigned. Rectangles can be assigned to any available layer. Use the drop-down to select a different layer.
  • Width - displays the (X-axis) width of the selected Rectangle.
  • Height - displays the (Y-axis) height of the selected Rectangle.
  •  - click this icon to retain the existing X to Y ratio of the rectangle. 

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
You are reporting an issue with the following selected text
and/or image within the active document: