Altium NEXUS Documentation

PCB Placement & Editing Techniques in Altium NEXUS

Created: February 22, 2022 | Updated: September 1, 2022
This documentation page references Altium NEXUS/NEXUS Client (part of the deployed NEXUS solution), which has been discontinued. All your PCB design, data management and collaboration needs can now be delivered by Altium Designer (with Altium Designer Enterprise Subscription) and a connected Altium 365 Workspace. Check out the FAQs page for more information.

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 NEXUS, 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.

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  X or Y keys to flip the object along the X-axis or Y-axis where applicable.
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.

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. The alignment sub-menu contains a number of options for distributing selected objects.

For more information on the individual alignment options, see the AlignComponents command page.

Via the PCB List Panel

Panel Page: PCB List

The PCB List panel allows you to display design objects in tabular format, enabling quickly 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.

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.

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.

Priorities When Pasting 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 the 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 the 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.

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 fount in the \Windows\Fonts folder is 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.
  • For a selected Track, Arc or Via object, the calculated Max Current and Resistance values are also provided.

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.

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.

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.

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

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 String objects
Placed String objects

A string places text 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.

Strings are available for placement in both PCB and PCB Library Editors. After launching the string placement command, the cursor will change to a cross-hair and you will enter string placement mode. A string will appear floating on the cursor:

  1. Position the cursor then click or press Enter to place a string.
  2. Continue placing further strings or right-click or press Esc to exit placement mode.

Additional actions that can be performed during placement are:

  • Press the Spacebar to rotate the string 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 string along the X-axis or Y-axis.
  • Press the L key to flip the string 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 string object directly in the design space and change its location, rotation, orientation, and size.

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

A selected String
A selected String

  • Click and drag B to rotate the string about its reference point A (denoted by the small x).
  • Click and drag C to resize the string's bounding box in the vertical and horizontal directions simultaneously.
  • Click and drag D to resize the string's bounding box in the vertical and horizontal directions separately.
  • Click anywhere on the string 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.

Special Strings

While string 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.
  • 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

  • If a string starts with the "." character, the entire string is treated as a 'special' string.
  • To include more than one special string within a PCB string, 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.

Placing a Special String

To use a special string on a PCB, place a string 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_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_RevNumber – 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 String 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 String 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 string, relative to the current design space origin. Edit to change the X position of the string. 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 string, relative to the current origin. Edit to change the Y position of the string. 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 String. 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 String object section 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 String object section 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.
  • 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 selected, a bounding box will appear containing a small (x) on the bounding handle.

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.

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.

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.
  • 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

  • If a string starts with the "." character, the entire text is treated as a 'special' string.
  • 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_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_RevNumber – 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.
  • 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 NEXUS. 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 NEXUS 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.

A component can be converted to its constituent primitive objects using the Tools » Convert » Explode Component to Free Primitives command.

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°.

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.
  • 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 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.
  • 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.

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: