Altium Designer Documentation

Schematic Placement & Editing Techniques in Altium Designer

Created: April 27, 2022 | Updated: June 30, 2022

Electronic design is the process of capturing a logical design in the schematic then representing that design as a set of objects in the PCB design space. Even for a small circuit, the schematic can include many components, each with numerous models and parameters. The PCB design space can also contain a large number of design objects that make up the board. During the course of the design process, the placement and properties of these objects need to change as you work to balance out the various design requirements.

Fundamentals of Object Placement

Grids and Cursors

Before placing objects in the Schematic Editor, set the grids to enable easier placement. Altium Designer offers three grid types: visible grids for navigation, snap grids for placement, and electrical grids for aiding the creation of connections. Grids are document options, meaning that they are saved with the individual design, and therefore, grid settings may differ between one design document and the next. Set the grids initially in the General region of the Document Options mode of the Properties panel.

Visible grids appear whenever the zoom level allows them to be sufficiently spaced, displayed as either lines or dots. The Snap Grid is the grid that the cursor is locked to when placing or moving schematic design objects. Electrical grids override snap grids since they allow connections to be made to off-grid parts. Enable Snap to Electrical Object Hotspots so that when moving an electrical object in the workspace, if it falls within the electrical grid range of another electrical object to which it could connect, it will snap to the fixed object and a hotspot (red cross) will appear. The electrical grid should be set slightly lower than the current snap grid or else it becomes difficult to position electrical objects one snap grid apart.

Grids can be quickly modified or toggled between enabled and disabled through keyboard or mouse shortcuts, for example, press G to cycle through the Snap grid settings of 10 mil, 50 mil, and 100 mil. You can also use the View » Grids sub-menu. Use the Schematic - Grids page of the Preferences dialog to set Imperial and Metric Grid Presets.

You can change the Cursor type to suit your needs in the Cursor region of the Schematic - Graphical Editing page of the Preferences dialog. For example, a large 90 degree cross that extends to the edges of the design window (Large Cursor 90 option) can be useful when placing and aligning design objects.

Altium components are designed on an Imperial grid, be aware that their pins will not fall on logical grid increments if you choose to use a Metric grid. You can use an Imperial grid with a Metric sheet, the sheet Template and Units are set in the Document Options mode of the Properties panel, which is displayed when there is nothing selected on the schematic sheet.

Placing Design Objects

The basic steps for placing schematic design objects are outlined below.

  1. Select the object type that you want to place by selecting an object type from the Place menu (e.g., Place » Wire) or by clicking on one of the icons on the Active toolbar. Shortcut keys for placement are also available (e.g., P, W to place a wire). To place components (parts), you can also click the Place button in the Components panel, or select the component name from an available library in the Components panel and drag it into the document.
  2. When an object is selected for placement, the cursor will change to a crosshair, indicating that you are in editing mode, and if relevant, the object will appear "floating" under the cursor.
  3. Press the Tab key to edit the properties of the object before placing it. This will open the Properties panel for that particular object, allowing you to change various options. Once you have finished setting the properties, click  to return to placement mode. The advantage of editing during placement is that objects that have a numeric identifier, such as a designator, will auto-increment.
  4. Position the cursor then left-click or press Enter to place the object. For complex objects, such as wires or polygons, you must continue the position-and-click procedure to place all vertices of the object.
Note:  The options on the Schematic - AutoFocus page of the Preferences dialog control the state of the schematic display. For example, the schematic can be configured to automatically zoom in when placing or editing connected objects or dim all wiring not related to the wire currently being placed. Other zooming and panning options are available using the shortcut keys or mouse wheel. Use the Ctrl key and scroll the wheel mouse to zoom in and out, push the wheel button down and move the mouse up to zoom in or move the mouse down to zoom out when placing. You can set up the behavior of your mouse on the System - Mouse Wheel Configuration page of the Preferences dialog.
  1. After placing an object, you will remain in placement mode (indicated by the crosshair cursor), allowing you to immediately place another object of the same type. To end placement mode, right-click or press the Esc key. In some cases such as placing a polygon, you may need to do this twice; once to finish placing the object and once to exit placement mode. When you exit placement mode, the cursor will return to its default shape.

Repositioning an Object

Click and hold on an object to reposition it. When you do, the cursor may snap to a different location on the object from where you clicked. This is intentional and is controlled by the following options. Note that the electrical objects (such as a net label, sheet symbol, or component) behave differently from non-electrical objects (such as a rectangle, or line) because the Always Drag option is on by default.

  • Center of Object - when enabled, for a graphical object move the cursor and hold at the geometric center of the object. For an electrical object, hold at the click location if the Always Drag option is enabled. If Always Drag is off, hold at the geometric center. For text strings, hold by the string reference point (determined by the string's current Justification property setting).
  • Object's Electrical Hot Spot - when enabled, if the object is an electrical object, hold at its Hot Spot (the Hot Spot is the point where connectivity is created). When enabled, this option overrides the Center of Object option for electrical objects.
  • When Always Drag is enabled, the software attempts to maintain the connectivity currently defined in that net. Always Drag can be temporarily inhibited by holding Ctrl as you click and drag.
  • Press the G key during object movement to cycle through the available Grid Preset settings. These are configured in the Schematic - Grids page of the Preferences dialog.
  • Press the Ctrl key during object movement to temporarily inhibit the current Grid Preset. This feature is useful when you need to carefully adjust the location of a string.

Re-Entrant Editing

The Schematic Editor includes a powerful feature called re-entrant editing that allows you to perform a second operation using the keyboard shortcuts without having to quit the operation you are currently carrying out. For example, pressing the Spacebar when placing a part will rotate the object but will not disrupt the placement process. Once you place the part, another part will appear ready at the cursor already rotated.

Re-entrant editing is also very useful if you start placing a wire that needs to be connected to a port that you have not placed yet. There is no need to exit Place Wire mode; just press the Place Port shortcut keys (P, R), place the port, press Esc to exit Place Port mode and then connect the wire to the port.

Measuring the Distance on a Schematic Document

The Schematic Editor has a distance tool located in the Reports menu (Reports » Measure Distance as well as the Ctrl+M shortcut keys). You can use this tool to measure the distance between two points on a schematic document. After launching the command, you are prompted to click on two points on the schematic document. Once you have chosen two points, an Information dialog appears with an overall Distance value, with the X Distance and Y Distance values displayed accurate to two decimal places.

The measurement units are determined by the Units chosen for the schematic document in the General region of the Document Options mode of the Properties panel. You also can switch to Imperial or Metric units by toggling the System units (View » Toggle Units).

Properties Panel

When the active document is a schematic document (*.SchDoc) and no design object is selected in the design space, the Properties panel presents the Document Options.

The following collapsible sections contain information about the options and controls available under the panel's General tab:

The options in this section of the panel determine which schematic objects may be selected in the design space.

  • All - On button – select to remove object filtering so that all types of objects may be selected.
  • Object buttons – toggle each object button to enable/disable the ability to select that object type.

  • Units – select the desired unit. Choose either mm or mils.
  • Visible Grid – enter the desired grid. Use the or to show/hide the grid in the design space.
  • Snap Grid – check the box to enable snap grids. Enter the desired grid in the text box or use the G shortcut to cycle through the different grids.
    • Snap to Electrical Object Hotspots – enable to use the snap grid to snap to an object's electrical hotspots or use the Shift+E shortcut.
  • Snap Distance – when the cursor is within this distance from an enabled object snap point (and snapping is enabled for the active layer), the cursor will snap to that point.
  • Document Font – set the font size, style and any additional font attributes that will be used for the text associated with all objects in the document sheet. For any given object, the font settings may be overridden in its corresponding Properties panel mode, which is enabled when that object is selected.
  • Sheet Border – check the box to enable a sheet border then click the colored box to change the border color.
  • Sheet Color – click the colored box to change the sheet color.

  • Formatting and Size
    • Template mode – set the page size and format by selecting from a range of predefined schematic sheet templates. The list includes local and Workspace templates found in the location specified in the Data Management – Templates page of the Preferences dialog. Note that a default schematic sheet to be used for new schematic documents can be defined in the System – New Document Defaults page of the Preferences dialog.
      • Template – use the drop-down menu to select from a list of Workspace and local templates, and if required, use the button to refresh the template.
      • Width/Height – the dimensions of the current page size shown in the current document units (see the General section above).
    • Standard mode – set the sheet size to a standard page format.
      • Sheet Size – use the drop-down menu to select from a list of standard page dimensions.
      • Width/Height – the dimensions of the current page size in the current document units.
      • Orientation – use the drop-down to select the desired orientation.
      • Title Block – enable this option to display one of two predefined title blocks on the schematic sheet. Use the associated drop-down to choose from either a Standard or ANSI title block style.
    • Custom mode – set the sheet size to specified custom dimensions.
      • Width – enter the required sheet width measurement.
      • Height – enter the required sheet height measurement.
      • Orientation – use the drop-down to select the desired orientation.
      • Title Block – enable this option to display one of two predefined title blocks on the schematic sheet. Use the associated drop-down field to choose from either a Standard or ANSI title block style.
  • Margin and Zones – defines the size of the sheet border graphics and its zone divisions. Uncheck the Show Zones box to hide the zone divisions in the border graphics.
    • Vertical – set the number of divisions (rows) in the vertical sheet margin. The alpha-numeric zone labeling type is defined by the Origin setting.
    • Horizontal – set the number of divisions (columns) in the horizontal sheet margin.
    • Origin – sets which corner of the document sheet(s) the perimeter zone alpha-numeric indicators will begin from (zone position A-1 or 1-A).
    • Margin Width – set the distance (in the current units) between the page edge and each of the four border lines as indicated by the arrows associated with each entry field.

The following collapsible section contains information about the options and controls available under the panel's Parameters tab:

The Properties panel Parameters tab lists all available Parameters and Rules available in the current project document.

  • All button – select to view both Parameters and Rules.
  • Parameters button – select to only view Parameters.
  • Rules button – select to only view Rules.
  • Parameters
    • Name and Value columns – lists the available parameters grouped by type.

When the same parameter exists in more than one location (Variant, Document, Project) and the Document parameter has no value, the parameter's value is inherited from the highest priority parameter that has a value (the parameter value defined in the schematic document overrides the value defined in the project options; the value defined in the variant overrides the value defined in the schematic document). When a Document parameter value is inherited (is being sourced from a Variant or Project parameter of the same name), the value is displayed in the Properties panel in gray italics, indicating that the parameter value is inherited. The Document parameter value can still be edited, as required.

  • Rules
    • Name and Value columns – these list the current specified rules and their values.
  • Add – use the drop-down menu to select to add a Parameter or a Rule. Selecting to add a new Rule will open the Choose Design Rule Type dialog to specify the type of rule to be used when adding a parameter as a rule to a supported design object in the schematic domain or a schematic document.
  • – only accessible when a rule is selected. Click to open the Edit PCB Rule dialog to edit the selected rule.
  • – click to delete the currently selected parameter or rule.

When a design object is selected, the panel will present options specific to that object type. The following table lists the object types available for placement on a schematic sheet – click a link to access the properties page for that object.

Arc Bezier
Blanket Bus
Bus Entry Comment
Compile Mask Designator
Ellipse Graphic
Generic Component Harness Connector
Harness Connector Type Harness Entry
Net Label No ERC
Note Offsheet Connector
Parameter Parameter Set
Part Polygon
Polyline Port
Power Object Probe
Rectangle Round Rectangle
Sheet Entry Sheet Symbol
Sheet Symbol Designator Sheet Symbol Filename
Signal Harness Text Frame
Text String Wire
Pin  

Modifying Data Strings

Using Formulas

The Properties panel has the ability to modify data strings using formulas in the Schematic Editor. Formulas and expressions offer a convenient method of modifying attribute parameters of multiple selected objects to change their location or string-based values such as the Designator and Comment. This allows you to apply a specific expression to the selected string objects. The expression can include any built-in arithmetic operators and functions that apply to strings (found in Pascal). If you want to use the current value for the attribute as part of the expression, you will need to make reference to this original value either by using the full name of the attribute or by using the exclamation character (the supported substitute for the name of the attribute currently being modified). When using attribute names, if any names contain spaces, these must be replaced by the underscore character. For example, use of the Component Designator field within a formula should be entered as Component_Designator.

Using the Smart Edit Feature

Some parameter string fields also provide access to the Smart Edit dialog when multiple objects are selected, which is opened from the associated button.

The Properties panel offers further support for string modification through its Smart Edit feature. Select the cell entries pertaining to the attribute that you want to modify for all required objects, right-click then choose Smart Edit from the menu that appears. The Smart Edit dialog will open.

The dialog offers two methods for performing string modification accessed from the Batch Replace and Formula tabs.

Object Placement and Editing Commonality

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

  1. Select the object to be placed from one of the toolbars or the Place menu.
  2. Use the mouse to define the location of the placed object in the schematic 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 (those that can logically be pre-defined) can be changed at any time on the Schematic – Defaults page of the Preferences dialog. These properties will be applied when placing subsequent objects.

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

Default values for the objects are saved, by default, in the file Advsch.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 panel for a Net Label object. 
Example Properties panel for a Net Label 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 Schematic – 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 Schematic - Graphical Editing 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 sheet, 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 Sheet Symbol object.
Example editing handles for a selected Sheet Symbol object.

When an object is selected, you can move the object or edit its graphical characteristics. Click on an object to select it; its 'handles' or vertices are displayed. To graphically change a selected object, click and hold on an editing handle. That point of the object will then become attached to the cursor. Move the mouse to a new location and release to resize. Click anywhere on a selected object to move it or press the Delete key to delete it.

Moving selected objects:

  • Selected schematic or PCB objects can be 'nudged' by the current snap grid value by pressing the arrow keys while holding down the Ctrl key.
  • Selected objects can also be 'nudged' by the snap grid value x10 by pressing the arrow keys while holding down the Ctrl+Shift keys.
  • For the schematic objects, the current Snap Grid is displayed on the status bar. The available Snap Grids are configured on the Schematic - Grids page of the Preferences dialog. Press G to cycle through the available grid values as you work.
  • For the PCB objects, the current Snap Grid is displayed on the status bar and is defined in the Grid Editor dialog. Press Ctrl+G to open the dialog and enter a new value.
  • You can select multiple PCB components and reposition them individually (in the order in which you selected them) using the Reposition Selected Components command (Tools » Component Placement » Reposition Selected Components or shortcut T, O, C). The components can be selected directly on the PCB using the PCB panel, or in the Schematic Editor if Cross Select Mode is enabled (Tools menu).

Using Copy and Paste

In the schematic editor, you can copy and paste objects within or between Schematic Documents, e.g. component(s) from a schematic can be copied into another Schematic Document. You can copy objects to the Windows clipboard and paste them into other documents. Text can be copied from the Windows clipboard into a schematic text frame. You can also directly copy/paste a table-type selection from another application such as Microsoft Excel or from any grid style control within Altium Designer.

More advanced copy/paste actions can be performed using the Smart Paste feature.

Select the object(s) you want to copy, click Edit » Copy (Ctrl+C) then click to set a copy reference point on the object that will be used to accurately position the object during pasting. You will only be prompted to click to set a reference point if the Clipboard Reference option is enabled on the Schematic - Graphical Editing page of the Preferences dialog.

When pasting copied component objects, their designators will reset if the Reset Parts Designators on Paste option is enabled on the Schematic - Graphical Editing page of the Preferences dialog.

Editing Group Objects

A group object is any set of primitives that has been defined to behave as an object. For example, a component on a schematic is a collection of drawing objects, strings, parameters, pins, and references to models. The primitive objects that belong to a group object are sometimes referred to as the child objects and the group object is their parent object.

Let's look at a typical group object edit that you might want to perform. Your design includes several capacitors. Currently, the voltage is specified as part of the components' comment string. You need to change this and specify the voltage as a component parameter instead and make this parameter visible on the schematic.

The steps we need to perform are (described in detail below):

  1. Select capacitors with a value of 100uF 16V.
  2. Change their comment to be 100uF (remove the 16V text).
  3. Add a new parameter to these components with a name of Voltage and a value of 16V.
  4. Change the visibility of this parameter so it's displayed on the schematic.

While this might seem like a complex set of edits to perform, it is actually quite straightforward.

Step 1. Selecting the Capacitors

To select all the 100uF 16V capacitors, right-click on the component symbol of one of them then select Find Similar Objects from the context menu.

We will use the approach covered in the previous example, except this time you want to match on components that have the same Comment and the same Current Footprint as shown in the image above.

Note that we can also match on components that have a designator starting with the letter C. This is done by changing the Component Designator to C*. Click OK to select the matching capacitors.

Step 2. Changing the Comment String

After clicking OK, the Properties panel opens (if the Open Properties option in the Find Similar Objects dialog was enabled). Behind it will be the schematic sheet displaying the matching objects selected on that sheet. If the Zoom Matching and Mask Matching options were enabled, the view will be zoomed and all the objects that did not match are faded or masked out.

You can check the status line at the bottom of the Properties panel to see if the same capacitors exist on other sheets. 

To change the comment string, delete 16V from the string then press Enter to apply the change. 

Step 3. Adding a New Parameter to the Component

The next change that we need to make is to add a new parameter. To do this, click Add in the Parameters region of the Properties panel in Component mode then select Parameter from the drop-down. A Parameter 1 entry will be added to the grid in the region. Enter the new parameter Name and Value

Click  to delete a selected parameter.

Step 4. Setting the Voltage Parameter to be Visible

The last step is to make the new Voltage parameter visible. Click the  icon to make the parameter visible (displays as ).

We have now updated the comment string for all 100uF capacitors. We have also added a new parameter called Voltage, set its value to 16V, and made this parameter visible.

Working with Components

A component within a library represents the physical device that is placed on the actual printed circuit board. On a schematic sheet, a component is represented by its schematic symbol model. Each component can contain one or more parts.

The Part represents the actual physical electronic component.
The Part represents the actual physical electronic component.

Summary

A Part is an electrical design primitive. It is a schematic symbol that represents an electronic device, such as a resistor, a switch, an operational amplifier, a voltage regulator, etc. Parts are stored within components in schematic component libraries. Note that each component can contain one or more parts. Along with a symbolic representation of the component, the part also includes links to models, such as the PCB footprint, and also parameters that are used to document details such as component parameters and supplier information. How the model links and parameters are added to the part depends on the type of library storage being used.

The terms Part and Component are both used to describe the symbol that represents the actual electronic device. The term Part is used because some components contain multiple parts. For example, a quad Op Amp component contains four separate Op Amps, or a resistor network can contain eight independent resistors. For these types of devices, you can create a separate schematic symbol to represent each Part during the component definition and place each of these parts independently. The terms Part and Component are used interchangeably on this page unless a multi-part component is being discussed.

Availability

Parts are available for placement in both the schematic and schematic library editors.

  • In the schematic editor, click Place » Part.
  • Right-click in the design space then choose Place » Part from the context menu.
  • From the Components panel, right-click on a component and select Place <ComponentName>.
  • From the Components panel, select a Generic Component as a placeholder.

    When connected to an Altium 365 Workspace, note that the Generic Components functionality is not supported with the Standard Subscription Plan. As such, this functionality will not be available with this level of access to Altium 365.

  • Dragging and dropping a component from the Components panel.
  • Select the Place button in the Details pane of the Components panel, or by using the Enter hotkey.
  • From the SCH Library panel when in the schematic library editor, select a component, then click Place.

Placement from the Components Panel

In the schematic editor, the part selection and placement process may be done from the Components panel.

  • The panel displays the contents of the currently selected library. Use the drop-down next to the library name to choose another library.
  • Use the mask field below the currently selected library field to filter the list and speed the searching process or scroll and select the required part.
  • Click Place, double-click, or click and drag to place the selected component onto the active schematic sheet. While the part is floating on the cursor, it can be rotated (press Spacebar), mirrored along an axis (press X or Y), or edited (press Tab) before placement.
  • The columns shown in the list of components in the currently selected library can be reorganized (click and drag) or reconfigured (right-click, then choose Select Columns).
  • Click on the  button within a Generic Component tile to attach the component to the cursor for placement in the active Schematic document. Selecting the tile itself will open that component type category in the Components panel.

Searching for a Component

The non-Workspace library menu options provide you the ability to set preferences, perform searches, and migrate database and file-based library content. To access these options, select the library menu button at the top right of the Components panel.

Select File-based Libraries Preferences to open the Available File-based Libraries dialog, where you may view controls to add or remove libraries, install libraries, and specify library search paths.

The current listing of database and file-based library components may be filtered by entering a search phase in the Components panel Search field. To access more advanced search capabilities for component libraries, select the File-based Libraries Search option from the panel’s menu (top right), which opens the File-based Libraries Search dialog. The dialog offers flexible search options including query-based filter constraints, and the ability to search through all available database and file-based libraries or those within a specified path.

  • The default search Scope is to search for Components in the Available File-based Libraries.
  • Alternatively, the dialog also supports searching through Libraries on path stored in folders on a drive. To do this, enable the Libraries on path option then configure the Path options as required.
  • The Filters use "AND" and, therefore, it is better to start with a simple filter and if there are many results, use the Refine last search mode to search within the results.
  • Query search results are presented in the File-based Libraries Search dialog when selecting Helper.

Placing from the Schematic Library Editor

A Part also can be placed directly from a library that is open in the schematic library editor from the SCH Library panel. Note that:

  • Clicking the Place button in the panel will place the selected part (component) in the last active schematic sheet.
  • While the part is floating on the cursor, it can be rotated (press Spacebar), mirrored along an axis (press X or Y), or edited (press Tab) before placement. The action can also be performed while dragging the object. Rotation is in increments of 90°.
  • If a part is placed directly from a library, that library does not need to be added in the Available File-based Libraries dialog first.

Graphical Editing

Graphical editing for a part is limited to moving, rotating, and mirroring. When a part is selected in the design space, a dashed selection box will appear around it. To graphically manipulate a selected component:

  • Press Delete to remove the selected part from the design.
  • Click and hold to move the selected part. The cursor will jump to the nearest electrical hotspot (the wiring end of the nearest pin).
  • Press the Spacebar to rotate the arc counterclockwise or Shift+Spacebar for clockwise rotation. The action can also be performed while dragging the object. Rotation is in increments of 90°.
  • While a part is moving on the cursor, press the X or Y key to mirror it along that axis.

A selected Part
A selected Part

When a component is rotated, its text strings are automatically repositioned to suit the new orientation. This behavior can be disabled if required. To do this, edit the string then clear the Autoposition checkbox in the Parameters Properties panel. Note that manually positioned text strings are denoted by a dot. These dots can be hidden if required by clearing the Mark Manual Parameters option on the Schematic – Graphical Editing page of the Preferences dialog.

Working Between the Schematic Component and the PCB Component

The software includes tools to help work between the component on the schematic and that same component on the PCB. These tools include Cross Probing, Cross Selection, and Selecting the PCB Components from the schematic.

Cross Probe

As the name implies, Cross Probe allows you to click on a component in one editor and jump to that component in the other editor. To Cross Probe:

  • Click Cross Probe located on the schematic or PCB editor menu on the Tools menu.
  • When you click the component in the schematic editor, it will be centered and zoomed in the PCB editor. The zoom level is set on the System – Navigation page of the Preferences dialog.
  • The default behavior is to remain in the same editor, ready to cross probe another component. To switch to the other editor as you Cross Probe, hold the Ctrl key.

Cross Select Mode

Cross Select Mode selects the same component in the other editor. Note that it does not zoom and center. Cross Selection is either on or off. Click Tools » Cross Select Mode to toggle the mode on/off. Select multiple components by holding the Shift key as you click to select.​

Selecting the PCB Components

This feature allows you to select multiple schematic components in a specific order, then place those same components in the PCB editor in the same order. To use this feature:

  • Select the components on the schematic one by one (hold Shift as you click to select multiple components).
  • Switch to the PCB editor then press the I, C shortcut to launch the Reposition Selected Components command. The Reposition Selected Components command is also available on the right-click menu after pressing the I shortcut.

 

General Tab

General

  • 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 – enter the designator. Toggle the eye icon to show/hide the designator. Use the lock icon to lock/unlock the designator.
  • Comment – enter the name. Toggle the eye icon to show/hide the name. Use the lock icon to lock/unlock the name.
  • Part <x> of Parts – displays the number of the selected part and the total number of parts. Use the drop-down to select the number of the associated part then enter the total number of parts. Click to lock/unlock the fields.
  • Description – the component/part description.
  • Type – select one of the following component types for the component footprint here. The available types are:
    • Standard – components that 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 – components that 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 – components that 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) – components that are used to short two or more different nets together, 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 (No BOM) – components that are used to short two or more different nets together, 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) – components that 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 want to exclude from the BOM.
    • Jumper – components that 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 – this field lists the name of the component selected. Click to open the Replace Component (Workspace) dialog or Replace Component (non-Workspace) dialog, depending on whether a Workspace or non-Workspace component is being edited. This dialog grants access to full details of the selected component (Parameters, Models, Part Choices, Supplier data, etc.), component comparison, and the ability to replace the current component with another, among other possibilities. If another component is selected as a replacement, this field will then display the full Design Item ID for the newly selected component. Click the Validate button () to display information regarding where the component resides. If it is a non-Workspace component, the file path in which it is saved on your computer will appear. If it is a Workspace component, the information will indicate that the component was simply found.
  • Source – displays the name of the source library of the component. Click  to search for and select the desired library.
  • Revision state – this field displays the current lifecycle state of the selected component revision, with the color icon and name of the revision state.

    When connected to an Altium 365 Workspace, note that configuration and use of lifecycle definitions is not supported with the Standard Subscription Plan. As such, the revision state will not be shown with this level of access to Altium 365.
    If a component used in a design (or managed schematic sheet) has been deleted, this will be indicated at the bottom of the General tab in the Properties panel by the associated icon.
  • Revision status – if the selected component revision is in an applicable state (allowed for use in designs) the entry will either reflect that the revision is the latest (Up to date) or not (Out of date). If the revision is in an inapplicable state (not allowed for use in designs) the entry will display Not applicable. Click the button to update the component to the latest revision.

    When clicking the button and not all parts of an out-of-date multipart component are selected, you will be prompted to update all parts of this component. Click Yes in the Confirm dialog that opens to continue.
  • Component issues (Properties panel only) – if a selected component sourced from the connected Altium 365 Workspace has any health issues, an indication of this will be presented by the (for errors) or (for fatal errors) icon. The number at the right of the icon indicates the number of found issues. Click the down arrow at the right of the number to see the short descriptions of the issues.

    An example of library health issues found.
    An example of library health issues found.

    Your Workspace library health can be explored in more detail through the Library Health dashboard page accessible from the Altium 365 Workspace browser interface. See Library Health Dashboard to learn more.
  • Supply Chain Data (Properties panel only) – this field displays the supply chain information from related Part Choice:
    • Median unit price. This entry will be displayed in red text if there are no prices, or the price = 0.
    • Stock. This entry displays the total sum of the stock available from the suppliers enabled as part of the Altium Parts Provider source for your Workspace.
    • Manufacturer Lifecycle Bar. Hover over the bar for an informative tool-tip. This can appear in one of four states:
      • White/Gray = Default, unknown or no information
      • Green = New or Volume Production states
      • Orange = Not Recommended for New Design
      • Red = Obsolete or EOL

      The manufaturer lifecycle status is designed to be used as an indicator, for a number of reasons:

      • Altium maintains a database of many millions of components, produced by thousands of component manufacturers. Since there is no single, consistent method used by those manufacturers to reflect a component's lifecycle state, the status is based on information aggregated from manufacturers, global distributors and global sales analysis.
      • A part is only reported as EOL or Obsolete when there is at least one authorized distributor or manufacturer that has confirmed this status.
      • Determining the Not Recommended for New Design status is more complex. Manufacturers sometimes just report if a part is active or not, and may not give advance warning that a part is to be discontinued or replaced. Therefore this lifecycle status does not always concur with the status provided by the manufacturer. The status algorithm uses various information, including real time and historical stock availability from all distributors, to try to determine the availability of the part. Parts which have consistently poor availability (when they have been generally available in the past), or cannot be sourced over a period of time after having previously having good availability, will eventually be flagged as Not Recommended for New Design (if they are not already EOL or Obsolete).
      • The idea of the lifecycle status indicator is to provide simple-to-understand information that helps you to make more informed decisions about a part, by highlighting those parts which may be problematic. However, due to the sheer volume of data and number of components that are managed, there is always a chance that the Altium status lags behind the instantaneous manufacturer status, and is therefore not up-to-date. It is not possible for Altium to guarantee the accuracy of the lifecycle status, it is recommended that if there is any doubt that you double-check with the manufacturer for authorized lifecycle information.

Location

  • (X/Y)
    • X (first field) – the current X (horizontal) coordinate of the reference point of the object, relative to the current design space origin. Edit to change the X position of the 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 object, relative to the current origin. Edit to change the Y position of the 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 – use the drop-down to select the rotation. Choices are 0 Degrees90 Degrees180 Degrees, and 270 Degrees.

Parameters

  • Grid – lists the Name and Value of the parameters associated with the currently selected component. Use to lock/unlock a listed parameter. Parameter values can be manually entered, or selected from a drop-down menu list that offers values sourced from all the available components of that type. You may toggle the eye icon to show/hide the parameter.
  • Favorites – parameters marked as Favorites will be shown in the Parameters list, while those not marked will be hidden. Hover to the right of a parameter filter’s name and click the  icon to set the filter as a Favorite. To remove a parameter as a Favorite, click the icon again.

    To see all hidden parameters, click the Show More link at the bottom of the list. Click the Show Less link to view Favorite parameters only.
    This feature is available by enabling the Schematic.UI.ShowMoreOrLessParameters option in the Advanced Settings dialog. When this option is disabled, the Favorite parameters and the Show More/Show Less features are disabled, resulting in all of the component parameters always being displayed in the Component mode of the Properties panel.
  • Font – click on the displayed font to change the font style.
  • Other – click to open a drop-down to change additional options:
    • Show Parameter Name – enable to show the parameter name.
    • Allow Synchronization with Database – enable to synchronize with the database. This option is used to control if the comment can be updated. By default, these options are enabled to always allow synchronization with the source library/database. You may disable this option to prevent that comment from being included in an update process.
    • (X/Y) – enter the X and Y coordinates.
    • Rotation – use the drop-down to select the rotation. Choices are: 90°180°, and 270°.
    • Autoposition – check to enable auto-positioning, meaning that the parameter is positioned automatically every time the associated component is rotated. Disable this option to keep the parameter position to the associated component when it is rotated.
  • Add – click to add a parameter, such as a footprint, model, or rule, among others. Click  to delete a selected entry from the grid. Click to edit the parameter via the parameter's respective dialog.

Graphical

  • Mode – use the drop-down to select the desired mode. If no modes other than Normal are available, this drop-down will be grayed out.
  • Mirrored – enable to mirror the part.
  • Local Colors – enable the local color option and the schematic component's fill, line, and pin colors are overridden with the colors from the FillLines, and Pins color boxes respectively. Disable this option to use the predefined colors from the library.

Part Choices

  • Part Name – click to be lead to additional information about the part, provided directly from the supplier.
  • Datasheet – click this button to be lead to the product's latest information, directly from the supplier's website.
  • SPN(s) – an SPN (Supplier Part Number) contains the following information:
    • Colored tile banner showing the supplier name and price. The color reflects the risk associated with choosing that supplier. The risk can change at any time based on the availability and price data received from the Altium Parts Provider.
      • Green = Best
      • Orange = Acceptable
      • Red = Risky
    • Supplier part number (linked to the part on the Supplier's website)
    • Last updated icon with details displayed in the tooltip, color indicates:
      • White/Gray = Default, updated less than one week ago
      • Orange = 1 week < last update < month ago
      • Red = last update > 1 month ago
    • Country code for the Supplier location (ISO alpha 2); colored red if unknown.
    • Part source, details displayed in the tooltip.
    • Stock quantity; red if no stock available.
    • Unit price, red if no price available. Unit price includes currency icon, currency is determined by the location of the supplier.
    • Available price breaks, with Minimum Order Quantities.
If no part choices are available, a button that will open the Edit Supplier Links dialog will be made available, which you may use to add supplier links for a component.

Pins Tab

  • Grid – this region lists the Pins and Names for all the pins of the selected component. Use the eye icon to show/hide the pin. Use the lock icon to lock/unlock the pins.

    For a multi-functional pin (a pin that has functions specified in the Functions filed in the Pins mode of the Properties panel), click in the pin's cell in the Name column and select the pin function in the drop-down that appears. The selected function will be shown as the pin name on the schematic sheet.

  • – when the button is enabled (the closed lock icon), the pins of the component are prevented from being edited. Only the component itself can be edited. If you wish to edit a pin by selecting it in the design space, disable this option.
  • – use this button to toggle visibility of the component's pin on the schematic sheet. 
  • Add – click to add a pin. Click  to delete a selected entry from the table. Click to open the Component Pin Editor dialog in which you can view all pins for either the component in the active schematic library document or a placed component (or part thereof) in the schematic editor.

Generic Components

Placing a Generic Component from the Components panel
Placing a Generic Component from the Components panel

When Altium Designer is connected to a Workspace, the available Generic Components can be accessed from the Components panel where they are exposed when the All option is selected in the Categories pane – or from the top drop-down menu when the panel is in its compact mode. Click on the button within a Generic Component tile to attach the component to the cursor for placement in the active schematic. Selecting the tile itself will open that component type category in the Components panel.

When connected to an Altium 365 Workspace, note that the Generic Components functionality is not supported with the Standard Subscription Plan. As such, this functionality will not be available with this level of access to Altium 365.

Generic Component Properties

General

  • Designator – enter the designator. Toggle the eye icon to show/hide the designator. Click the lock icon to lock/unlock the designator.
  • Comment – enter the name. Toggle the eye icon to show/hide the name.
  • Description – the generic component/part description.
    • Replace – select the Replace button when a design has progressed to the point where a Generic Component can be replaced with a specific physical component using the Replace Component dialog.

Location

  • (X/Y)
    • X (first field) – the current X (horizontal) coordinate of the reference point of the object, relative to the current design space origin. Edit to change the X position of the 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 object, relative to the current origin. Edit to change the Y position of the 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 – use the drop-down to select the rotation.

Parameters

  • Grid – lists the Name and Value of the parameters associated with the currently selected component. Use the lock icon to lock/unlock a listed parameter. Parameter values can be manually entered, or selected from a drop-down menu list that offers values sourced from all the available components of that type. You may the eye icon to show/hide the parameter.
  • Font – click on the displayed font to change the font style.
  • Other – click to open a drop-down to change additional options:
    • Show Parameter Name – enable to show the parameter name.
    • Allow Synchronization with Database – enable to synchronize with the database. This option is used to control if the comment can be updated. By default, these options are enabled to always allow synchronization with the source library/database. You may disable this option to prevent that comment from being included in an update process.
    • (X/Y) – enter the X and Y coordinates.
    • Rotation – use the drop-down to select the rotation.
    • Autoposition – check to enable auto-positioning, meaning that the parameter is positioned automatically every time the associated component is rotated. Disable this option to keep the parameter position to the associated component when it is rotated.

The Designator uniquely identifies each component in the design.The Designator uniquely identifies each component in the design.

Summary

The designator field is a child parameter object of a schematic component (part). It is used to uniquely identify each placed part to distinguish it from all other parts placed in all the schematic sheets in the project.

Availability and Placement

The designator is automatically placed when the parent component part object is placed. It is not a design object that you can directly place.

Graphical Editing

The designator string can be edited graphically using what is known as in-place editing. To edit a designator string in place, select the designator by dragging your cursor around it, then hit enter.

An example of in-place editing
An example of in-place editing

Once editing is complete, press Enter or click away from the string to exit in-place editing mode.

Non-Graphical Editing

There are two aspects to consider in relation to editing the designator: editing the value of the designator and editing the display properties of the designator. 

Rather than manually editing each component designator, it is more practical to leave the assignment of the designators until the schematic is complete. After that, all designators can be logically assigned for the entire project using one of the Schematic Editor Annotate commands (Tools » Annotation) which offer full control for sheet-by-sheet positional annotation. For more information about annotation, see Annotating the Components.

The designator (and comment) strings can be displayed in the schematic library editor then doubled-clicked on to edit the properties. The  icon associated with the field in the Properties panel is used to show or hide the designator.

Editing the Designator Value in the Schematic Editor

The designator can be defined in the schematic editor as the component is being placed or after the component has been placed on a schematic sheet in the Properties panel.

  • To edit the designator during component placement, press the Tab key while the component is floating on the cursor. The Properties panel will open; enter the required designator string. Click the design space pause button overlay () to resume placement.
  • Continue to place components or press Esc to terminate placement.
  • Press the Spacebar to rotate the arc counterclockwise or Shift+Spacebar for clockwise rotation. The action can also be performed while dragging the object. Rotation is in increments of 90°.
  • To edit the designator after placement, double-click on the placed component to open the Properties panel where the designator can be edited. 

Editing the Designator Display Properties 

The appearance of the designator string, which includes the font type, size, and color, can be configured on the Schematic - Defaults page of the Preferences dialog. These settings will apply unless overridden by settings defined in the component symbol in the Schematic Library Editor.

Fixing the Location of the Designator String

The default behavior of the Designator is to auto-position it as a component is rotated during placement. If this behavior is not required, turn off the Autoposition option in the Preferences dialog (refer to the previous image) either during symbol creation or after the component has been placed on a schematic sheet. Note that doing this sets this parameter to be classified as a manual parameter (meaning manually positioned parameter). Manual parameters are identified by a dot on the lower left corner of their selection box.

Control the display of manual parameter marker dots using the Mark Manual Parameters option on the Schematic - Graphical Editing page of the Preferences dialog.

Notes

  • The Schematic Editor includes a simple auto-increment feature for the designator that can be used during the placement of multiple instances of the same part. To use this, press Tab while the first component is floating on the cursor and enter a suitable designator, for example R1. Subsequent components will then be designated R2, R3, etc. Note that when you switch to placing a different component type you must again press Tab and enter a suitable designator prefix.
  • When placing multi-part components and the initial designator is assigned as just described, a part suffix will automatically be assigned, for example, U3A, U3B, etc. If the initial designator is not assigned, all parts will have the same suffix. This is resolved by the Schematic Editor's Annotation command. The part suffix can be alpha or numeric. Use the Alpha Numeric Suffix option on the Schematic - General page of the Preferences dialog to configure.

Location

  • (X/Y) 
    • X (first field) - the current X (horizontal) coordinate of the reference point of the object, relative to the current workspace origin. Edit to change the X position of the 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 object, relative to the current origin. Edit to change the Y position of the 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 - use the drop-down to select the rotation. 

Properties

  • Object  - displays the associated object.
  • Name -  enable this field by clicking the visibility icon () to added the prefix "Designator:" to the designator value itself. Doing so visually distinguishes and confirms that the text value is a designator within the schematic document.
  • Value - displays the designator name itself. Toggle the to show/hide the value.
    • Autoposition -  check to enable auto-positioning, meaning that the text will remain in the chosen position as the component is moved and rotated.
    • Lock Parameter - check to lock the parameter, which prevents the value from being edited from the Properties panel or schematic document.
    • Allow Synchronization with Database - enable to synchronize with the database. This option is used to control if the comment can be updated. By default, these options are enabled to always allow synchronization with the source library/database. You may disable this option to prevent that comment from being included in an update process.
  • Font - use the controls to select the font, font size, font color, and add any desired special characteristics to the font, such as bold, italics, and underlines.
  • Justification - click the arrows to configure the justification of the text or circle to center.  
  • Override Library Primitive (Preferences dialog only) - enable this checkbox to override the primitive settings defined for the designator object in a library. Therefore, when a component is placed, it will adopt the primitive settings that you have defined in the Preferences dialog, rather than those settings that have been defined for the component in the library.

A Comment allows displaying additional information for a component.A Comment allows displaying additional information for a component.

Summary

The Comment field is a child parameter object of a schematic component (part). It is used for displaying additional information for a component in a schematic sheet of the project.

Availability and Placement

The Comment is configured when the parent component part object is placed. It is not a design object that you can directly place.

Graphical Editing

The Comment can be edited graphically using what is known as in-place editing. To edit a Comment in place, click once to select, pause for a second, then click a second time to enter edit mode.

Click once to select the string.Click once to select the string.

Once editing is complete, press Enter or click away from the string to exit in-place editing mode.

Non-Graphical Editing

There are two aspects to consider in relation to editing the Comment: editing the value of the Comment and editing the display properties of the Comment. 

Editing the Comment in the Schematic Editor

The Comment can be defined in the schematic editor as the component is being placed or after the component has been placed on a schematic sheet in the Comment field of the Properties panel.

  • To edit the comment during component placement, press the Tab key while the component is floating on the cursor. The Properties panel will open; enter the required Comment. Click the design space pause button overlay () to resume component placement.
  • Continue to place components or press Esc to terminate placement.
  • To edit the Comment after placement, double-click on the placed component to open the Properties panel where the Comment can be edited. 

Editing the Comment Display Properties 

The appearance of comments, which includes the font type, size, and color, can be configured on the Schematic - Defaults page of the Preferences dialog.

Fixing the Location of the Comment

The default behavior of the Comment is to auto-position it as a component is rotated during placement. If this behavior is not required, disable the Autoposition option in the Preferences dialog (refer to the previous image) either during symbol creation or after the component has been placed on a schematic sheet. Note that doing this sets this parameter to be classified as a manual parameter (meaning manually positioned parameter). Manual parameters are identified by a dot on the lower-left corner of their selection box.

Control the display of manual parameter marker dots using the Mark Manual Parameters option on the Schematic - Graphical Editing page of the Preferences dialog.

Location

  • (X/Y)
    • X (first field) - the current X (horizontal) coordinate of the reference point of the object, relative to the current design spaceorigin. Edit to change the X position of the 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 object, relative to the current origin. Edit to change the Y position of the 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 - use the drop-down to select the rotation. Choices are: 0 Degrees90 Degrees180 Degrees, and 270 Degrees.

Properties

  • Component - displays the name of the associated component. Click the Component link to open the Part Properties panel, where you may edit component options, as well as the comment itself, which will be defined in the Comment field of that panel.
  • Name - enable this field by clicking the visibility icon () to add the prefix "Comment:" to the comment value itself. Doing so visually distinguishes and confirms that the text value is a comment within the schematic document.
  • Value - displays the comment name itself. Toggle the () to show/hide the value.
    • Autoposition -  check to enable auto-positioning, meaning that the text will remain in the chosen position as the component is moved and rotated.
    • Lock Parameter - check to lock the parameter, which prevents the value from being edited from the Properties panel or schematic document.
    • Allow Synchronization with Database -  enable to synchronize with the database. This option is used to control if the comment can be updated. By default, this option is enabled to always allow synchronization with the source library/database. You may disable this option to prevent the comment from being included in an update process.
  • Font - use the controls to select the font, font size, font color, and add any desired special characteristics to the font, such as bold, italics, and underlines.
  • Justification - click the arrows to configure the justification of the text or circle to center.  
  • Override Library Primitive (Preferences dialog only) - enable this checkbox to override the primitive settings defined for the comment object in a library. Therefore, when a component is placed, it will adopt the primitive settings that you have defined in the Preferences dialog, rather than those settings that have been defined for the component in the library.

Managing Footprints Across the Entire Design

Altium Designer's Schematic Editor includes a powerful Footprint Manager. Launched from the Schematic Editor's Tools menu (Tools » Footprint Manager), the Footprint Manager lets you review all the footprints associated with every component in the entire project. Multi-select support makes it easy to edit the footprint assignment for multiple components, change how the footprint is linked, or change the current footprint assignment for components that have multiple footprints assigned. Design changes are applied through the ECO system, updating both the schematic and the PCB if required.

Working with Design Object Parameters

Parameters are general purpose text strings that are child objects of a parent object. They identify and add additional information to that parent object and are accessed directly in the Properties panel when selected in a schematic sheet.

Parameters are used for objects (a component is shown in the above image), documents and projects to add detail information to the design.Parameters are used for objects (a component is shown in the above image), documents and projects to add detail information to the design.

Summary

Parameters are general purpose text strings that are child objects of a parent object. They identify and add additional information to that parent object and are accessed directly in the Properties panel when selected in a schematic sheet.

Schematic components, for example, make extensive use of parameters. They are used to define the Sheet Name and the Comment, as well as the general purpose data strings that can be added to a component to fully define it. General purpose (User) component parameters can be used for a variety of functions including; component details and ratings, supplier information, library references, and datasheet links.

Parameters also can be defined at the schematic sheet (document) and project levels. Document-level parameters are used for defining fields such as the document title and number, while project-level parameters are ideal for defining fields such as the designer or the project name.

Availability

Parameters are added or automatically included as a property of the parent object and are not placed independently like a Text String. The types of available parameters can be broadly grouped as System and User parameters, where the latter is manually added.

Identifier and System Parameters

A range of key system parameters is automatically included with objects placed in a schematic. These provide the base object information that is used by the system to distinguish the parent object's name, type and data source.

The inherent system parameters for objects include, but are not limited to, the Comment, Description and Design Item ID (Library Reference) properties.

Object system parameters are accessible in the General section of the Properties panel (under the General tab) when a parent object is selected. When visible and selected in the design space, an individual parameter is accessible via the associated mode of the Properties panel as outlined below.

Left: Component system parameters in the Properties panel. Right: An individual system parameter in the Properties panel.   Left: Component system parameters in the Properties panel. Right: An individual system parameter in the Properties panel.Left: Component system parameters in the Properties panel. Right: An individual system parameter in the Properties panel.

Several system parameters cannot be made visible (and be selected) on a schematic sheet, and are therefore not available to the Parameters mode of the Properties panel. For component objects, these are Description, Design Item ID, Footprint, model references and so on. Other system parameters that are not directly accessible in a schematic include Document (Sheet) and Project parameters.

User Parameters

Parameters are added as a property of the parent object and are not placed independently like a Text String. Parameters can be added to any of the following design objects:

  • Component – add user-defined parameters in the Parameters tab of the Properties panel when a Component (Part) object is selected, or during component definition in the Schematic Library editor. System parameters such as Designator and Comment are always present for a Component object, as outline above. The Properties panel is accessed by double-clicking on an object, or by right-clicking on an object and choosing Properties from the context menu. If the Properties panel is already active, select an object in the design space.
  • Part – in the Parameters region of the Properties panel when a Part object is selected.
  • Pin - on the Parameters tab of the Properties panel when a Pin object is selected within a .SchLib file.
  • Port – on the Parameters tab of the Properties panel when a Port object is selected.
  • Sheet Symbol – on the Parameters tab of the Properties panel when a Sheet Symbol object is selected.
  • Document – on the Parameters tab of the Properties panel when in Document Options mode (deselect all schematic objects or click in free space on the document sheet). A number of default parameters are automatically included in a new schematic sheet, as determined by the applied/default sheet template.
  • Project - in the Project Options dialog (Project » Project Options). Project-level parameters are listed and added on the Parameters tab of the dialog.
While placing an object (Component, Sheet Symbol, etc.,), press Tab to pause the placement and access the parent object mode of the Properties panel, from where parameters can be added or modified on the fly. Click the design space pause button overlay () to resume placement.

User parameters are available under the Parameters tab of the Properties panel, or modal dialog,  when the parent object is selected – parameters can be both added and edited. The exceptions are Project parameters (via the Project Options dialog) and Component Pin parameters (via the Pin Properties, or the modal-view of the Pin dialog). When visible and selected in the design space, an individual parameter is accessible via the associated mode of the Properties panel, or modal dialog, as outlined below.

Left: Component user parameters in the Properties panel (Parameters tab). Right: An individual system parameter in the Properties panel. Left: Component user parameters in the Properties panel (Parameters tab). Right: An individual system parameter in the Properties panel.Left: Component user parameters in the Properties panel (Parameters tab). Right: An individual system parameter in the Properties panel.

Parameters that are added to a parent object during its placement (see above) will become the default parameters for further placements of that parent object unless the Permanent option on the Schematic – Default Primitives page of the Preferences dialog is enabled for that object.
When this option is enabled, parameters added to the object being placed will be also added to subsequent objects placed during the same placement session, but not to any following placement sessions for that object.

Graphical Editing

Visible parameter strings can be edited graphically, directly in the design space.

Click and drag a parameter to reposition it. To edit the parameter string in place:

  1. Drag your mouse cursor around the parameter object while keeping the mouse button pushed down.
  2. Once selected, the object will be highlight by a green border.
  3. Select Enter to begin editing the text.
  4. Once editing is complete, press Enter again or click away from the string to exit in-place editing mode.

A parameter string can be selected and edited directly in the design space. (Right) Select the entire string to type over it.A parameter string can be selected and edited directly in the design space. (Right) Select the entire string to type over it.

Parameters that are visible and selectable in the design space may be dragged to a new location and rotated during the process. Click and drag the parameter string, use the Spacebar and Shift+Spacebar keys to rotate it in 90° steps, and then click to confirm its new position/orientation.

See Parameter String Positioning below for information on component parameter Autopositioning and related Properties panel options.

Locked Parameters

A parameter that is the child of a Component Part can be locked, where its Name and Value strings are made un-editable. This can be done by:

  • toggling the Lock icon () associated with its entry under the Parameters tab in the Properties panel or modal dialog for its parent object, or
  • checking the Lock Parameter option in the Properties panel when the parameter is directly selected in the design space.

Once locked, the parameter string cannot be edited in the Properties panel, modal dialog (under the Parameters tab for the parent object), or in the design space using in-place editing.

Component Parameters

Component parameters, the most obvious and frequently used Schematic parameters, include additional sets of dedicated parameters and features that expand the ability to define component objects.  

Defining Parameters in the Schematic Library

Prior to placement in a schematic, the child parameters of a parent component object can be defined in the component library source. Using the Properties panel in the same manner as when working with parameters in the Schematic Editor, the panel is used to edit and add parameters to a component entry in the Schematic Library Editor.

With a schematic component library document open, select a component entry in the SCH Library panel (View » Panels » SCH Library) to access its parameter properties in the Properties panel.

Access the properties of a library component by selecting its entry in the SCH Library panel.Access the properties of a library component by selecting its entry in the SCH Library panel.

A library component's Designator and Comment are not visible in the Schematic Library editor design space by default but can be enabled by checking the Show Comment/Designator option in the Library Options mode of the Properties panel  (Tools » Document Options) – available when no objects are selected in the design space.

Parameters that are owned by a library component are defined and edited by the same process applied to placed schematic components. The Tab key may be used to create or edit parameters on the fly, while an object is being placed in the editor design space. Parameters are accessed via the Properties panel or modal dialog, where the core system parameters are available under the panel's General tab, and user parameters are added/edited under the panel's Parameters drop-down.

To add a parameter to a component pin, for example, select the Pin object in the design space then the Parameters drop-down in the Properties panel or modal dialog. Click the Add button to insert a new parameter Name/Value pair in the list. Parameters that are associated with the entire component are added as described above.

The Designator Parameter

In the Library Editor, a component Designator parameter is typically given a suitable prefix followed by a question mark. When the component is placed in a schematic from the library, the question mark is detected by the Schematic Editor's Annotation tool and replaced with a suitable numeric suffix during project annotation.

The Schematic Editor also includes a simple auto-increment feature for the designator that can be used during the placement of multiple instances of the same part. To use this, press Tab while the first component is floating on the cursor to pause the placement, and then enter a suitable designator in the Properties panel; for example R1. Subsequent components will then be designated R2, R3, etc. 

When placing multi-part components and the initial designator is assigned in this way, a part suffix will automatically be added, for example U3A, U3B, etc. If the initial designator is not assigned, all parts will have the same suffix – this can be resolved by the Schematic Editor's Annotation feature. The part suffix can be alpha or numeric, as specified by the Alpha Numeric Suffix option in the Schematic - General page of the Preferences dialog.

Parameter String Positioning

The default behavior of a component parameter string is to autoposition it (maintain orientation) when a component is rotated during or after placement. If this behavior is not required, turn off the Autoposition option for that component parameter entry under the Parameters tab in the Properties panel – select the parameter in the list and click the Other link for access to the option.

Note that during component placement the Spacebar and Shift+Spacebar keys are used for rotation. A placed component object is rotated via the Rotation menu in the Location section of the Properties panel, or by selecting the component and pressing Ctrl+Spacebar or Ctrl+Shift+Spacebar.

Click and drag a visible parameter to manually reposition that parameter on the schematic – the standard orientation shortcut keys (Spacebar, Shift+Spacebar) will apply. If the Autoposition option is disabled for that parameter and the Mark Manual Parameters option is enabled in the Schematic - Graphical Editing page of the Preferences dialog, manually moved parameters will be identified by a dot on the lower left corner of their selection box.

Special Purpose Component Parameters

Special purpose component parameters are available for linking to related URL targets or file-based documentation. For a selected component, these are added in the Links section of the Properties panel, or under the Parameters tab for dedicated Help links that are activated via the F1 key.

Link Parameters

The Links feature enables the definition and presentation of named links to any number of reference URLs or documents.

To add a reference link for a component, select it in the design space, click the drop-down button in the Links section of the Properties panel, and then enter the link Name and its  Value (target URL or file path). The link is then accessible by right-clicking on the component in the design space and selecting the link Name from the References sub-menu.

 

The component links, as presented in the panel and design space, are internally based on Name/Value pairs in the format of ComponentLinknDescription/ComponentLinknURL (where n is number of the link in the list, based on the order of creation). See the Parameter Table Editor entry for that component to see more detail.

The HelpURL Parameter

Not unlike the Link parameter, the HelpURL parameter allows the definition of a link from a component to an external document, such as a PDF, or web page URL. When added as a component parameter, this link is activated when the F1 key is pressed over the component on the schematic sheet, or when that component is selected in the Libraries panel. Note that this action will override the normal F1 key feature, which links to the relevant page in the Altium online documentation.

The Help link is added as a user parameter under the Parameters tab of Properties panel, when a component is selected in the design space. Click the drop-down button to create a new parameter in the list, enter HelpURL as the parameter Name and then the target path/URL as the parameter Value.

When specifying the value for the parameter, this can be a URL, an absolute path to a document or just the document name. When F1 is pressed with the cursor hovering over the placed component object, or the References » Help option is used from the right-click menu, a search for the Help reference is conducted as follows:

  • If a path is specified, this location is searched first.
  • If the document cannot be found at this location, or if no path is specified, the \Help folder of the software installation is searched.
  • If the target is a URL, the web page will be opened in the software's internal browser or an external browser, depending on the state of the Open internet links in external Web browser option on the System - View page of the Preferences dialog.

Indirection - A Parameter as a String Value

Most component parameters can be displayed on a schematic sheet by checking their Visible option (where available) in the Properties panel (). Identifier and system parameters are available under the panel’s General tab, and user parameters are accessed under the panel’s Parameters tab.

Other parameters however, such as Document and Project parameters, cannot be directly displayed on the schematic sheet but may be inserted in a standard Text object using a technique known as String Indirection. Indirection is where the Value entry for a string object is the name of an available parameter (such as a Document or Project parameter) preceded by an equals sign – for example; =Title.

The software automatically detects such strings and checks for an available parameter Name that matches the Value entry of the placed Text object. The example of Title is found as a document parameter, causing the Text string to interpret and display the Title parameter Value – for example; MyDocument. A parameter Name may be indirected to a selected text string Value by in-place editing (typing =Title into it), or as a more informative approach, by using the Text drop down menu in the Properties panel to select from the available parameter strings.

Special Strings

Parameter strings that are available as indirected strings (see above) are known as Special Strings. The Value presented by these strings is actively inferred from templates or system and source data, so for example the special string =Time will detect and show the current system time, and =DocumentName will show the current schematic document file name (say, MySchematic.SchDoc).

There is a large number of predefined special strings available, which are listed below. Any user-defined document or project parameter can also be thought of as a special string and be indirected to a Text String on the schematic sheet.

Indirected strings are always interpreted and displayed during output generation, such as printing the schematic sheets. Many are also interpreted and displayed directly on-screen.

Special Strings are used to define fields in a title block, where the string indirection feature will ensure the correct information for the active schematic is extracted from the document parameters and displayed accordingly.

Parameters have a hierarchy, which means you can create a parameter with the same name at different levels of the project, each having different values. For a component parameter, Altium Designer resolves this in the following way:

  1. Component parameter (highest priority)
  2. Variant
  3. Schematic document
  4. Sheet Symbol (to see the value of the parameter of the sheet symbol above, select a compiled tab at the bottom of the design space)
  5. Project

Schematic Predefined Special Strings

The following are the predefined special strings available for use on a schematic document. The majority of these link to default parameter information defined for the active document on the Parameters tab of the Properties panel, when in Document Options mode (no objects selected). Any special strings available at a project level can be viewed/added on the Parameters tab of the Project Options dialog.

  • =Address1 – displays the value specified for the default document-level parameter Address1.
  • =Address2 – displays the value specified for the default document-level parameter Address2.
  • =Address3 – displays the value specified for the default document-level parameter Address3.
  • =Address4 – displays the value specified for the default document-level parameter Address4.
  • =Application_BuildNumber – displays the version and build for the current Altium software installation.
  • =ApprovedBy – displays the value specified for the default document-level parameter ApprovedBy.
  • =Author – displays the value specified for the default document-level parameter Author.
  • =CheckedBy – displays the value specified for the default document-level parameter CheckedBy.
  • =CompanyName – displays the value specified for the default document-level parameter CompanyName.
  • =ConfigurationParameters - displays the value specified for the default document-level parameter ConfirguationParameters.
  • =CurrentDate – the current date, automatically calculated from the user's system settings and in the format dd/mm/yyyy, updated upon editing the schematic or on refresh/redraw. Example: 10/12/2017.
  • =CurrentTime – the current time, automatically calculated from the user's system settings and in the format h:mm:ss AM/PM, updated upon editing the schematic or on refresh/redraw. Example: 2:39:47 PM.
  • =Date – used to display static date information. Displays the value specified for the default document-level parameter Date. Unlike the =CurrentDate special string, which is automatically calculated and presented in a set format, the user can enter static date information in any format they prefer.
  • =DocumentFullPathAndName – used to display the full path and name of the document into which the string is placed. Example: C:\MyTestDesign\PSU.SchDoc.
  • =DocumentName – used to display the schematic's file name only (without the file path). Example: PSU.SchDoc.
  • =DocumentNumber – displays the value specified for the default document-level parameter DocumentNumber. The source parameter can also be updated through the Sheet Numbering for Project dialog when using the Tools » Annotation » Number Schematic Sheets command.
  • =DrawnBy – displays the value specified for the default document-level parameter DrawnBy.
  • =Engineer – displays the value specified for the default document-level parameter Engineer.
  • =ImagePath – displays the value specified for the default document-level parameter ImagePath.
  • =IsUserConfigurable - user can configure.
  • =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 to which the generated data relates 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 to which the generated data relates (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).
  • =ItemRevisionLeve1 – the Level 1 portion of an Item Revision's naming scheme (e.g., A).
  • =ItemRevisionLeve1AndBase – 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).
  • =LibraryName - displays the actual name of the schematic library file. (e.g., SpiritLevel_2E.SchLib)
  • =ModifiedDate – the modified date stamp of the schematic, automatically populated. Example: 10/12/2015.
  • =Organization – displays the value specified for the default document-level parameter Organization.
  • =PCBConfigurationName – the name of the data set from which the output has been generated as defined in the Release view (Project Releaser).
  • =Project – displays the name of the project (excluding extension). 
  • =ProjectName – displays the actual name of the project (including extension). For example, for a project with filename MyPCB.PrjPcb, this special string will display MyPCB.PrjPcb.
  • =ProjectRev - displays the project revision.
  • =Revision – displays the value specified for the default document-level parameter Revision.
  • =SheetNumber – the sheet number of the current schematic. This value is calculated when using the Tools » Annotation » Number Schematic Sheets command. The assigned sheet number, in the Sheet Numbering for Project dialog, will be entered into the value for the default document-level parameter SheetNumber. The special string when used on the Editor tab view of the schematic sheet will source its information from here.
  • =SheetTotal – the sheet total for the project. This value is calculated when using the Tools » Number Schematic Sheets command. The sheet total, in the Sheet Numbering for Project dialog, will be entered into the value for the default document-level parameter SheetTotal. The special string when used on the Editor tab view of the schematic sheet will source its information from here.
  • =Time – used to display static time information. Displays the value specified for the default document-level parameter Time. Unlike the =CurrentTime special string, which is automatically calculated and presented in a set format, the user can enter static time information in any format.
  • =Title – displays the value specified for the default document-level parameter Title.
  • =VariantName - displays the variant from which output has been generated. This follows the entry for the current variant. If the base design is used to generate the output, the value will simply be [No Variations].
  • =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.

Note that the full list of special strings available in the Text drop-down menu in the Properties panel (when a text object is selected) will also include any derived from user-defined document-level and project-level parameters.

Special Strings for Use with Component Parameters

Several additional special strings (or special interpretations of existing ones) are available when defining component parameters. In each case, the special string is entered as the value for a parameter.

  • =CurrentFootprint – displays the name of the currently assigned footprint for the component as defined in the Models region of the Properties panel (General tab).
  • =Comment – displays the value appearing in the component's Comment field as defined in the Properties region of the Properties panel (General tab).
  • =Description – displays the value appearing in the component's Description field as defined in the Properties region of the Properties panel (General tab).
  • =[ParameterName] – displays the value defined for a specified component parameter. Enter the actual name of a component parameter as the special string name. For example, for a component parameter named PowerRating, enter =PowerRating. This approach can be used to display a component parameter such as Description by creating a user parameter (under the Parameters tab of the Properties panel) with a value of =Description, and then enabling that parameter's visibility in the schematic.

Location

  • (X/Y) 
    • X (first field) - the current X (horizontal) coordinate of the reference point of the object, relative to the current design space origin. Edit to change the X position of the 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 object, relative to the current origin. Edit to change the Y position of the 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 - use the drop-down to select the rotation.

Properties

  • Object type - displays the type of object (Component, Sheet Symbol, etc.,) and parameter type.
  • Name - the name of the parameter.
  • Value - the value of the parameter. Toggle ​ to show/hide the value.
  • Autoposition - check to enable auto-positioning, meaning that the text will remain in the chosen position as the component is moved and rotated.
  • Lock Parameter (Preferences dialog only) - enable this option to prevent editing of the parameter's value, either graphically in the design space
  • Allow Synchronization with Database (Preferences dialog only) - enable to synchronize with the database. This option is used to control if the comment can be updated. By default, these options are enabled to always allow synchronization with the source library/database. You may disable this option to prevent that comment from being included in an update process.
  • Font - use the controls to select the font, font size, font color, and add any desired special characteristics to the font, such as bold, italics, and underlines.
  • Justification - click the arrows to configure the justification of the text.  
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: