Search In: Doc:Documentation: NEXUS Client
Altium DesignerAltium 365Altium MCAD CoDesignerAltium CircuitMakerCompany DashboardAltium On-Prem Enterprise ServerAltium Infrastructure Server
Ver: Version: 4
5
Close
Search Search on Documentation

Working with Text Objects on a Schematic

Created: April 28, 2022 | Updated: June 17, 2022 | Applies to version: 5
Now reading version 4. For the latest, read: Working with Text Objects on a Schematic for version 5

This documentation page references Altium NEXUS/NEXUS Client (part of the deployed NEXUS solution), which has been discontinued. All your PCB design, data management and collaboration needs can now be delivered by Altium Designer and a connected Altium 365 Workspace. Check out the FAQs page for more information.

 

Parent page: Schematic Placement & Editing Techniques

Text objects are non-electrical primitives that can be used to add additional information to a schematic, place user notes, layout a schematic template, etc. These text objects can be placed as user-defined text on a schematic sheet or act as placeholders for design or system information – so called special strings.

Altium NEXUS's schematic editor supports Text Strings, Text Frames, and Notes. For information on these objects, and their associated settings in the Properties panel, refer to the collapsible sections below.

Special Strings

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

Default sets of predefined special strings are provided for use with new schematic documents. You also can add your own custom special strings by defining additional parameters at the document level (for use on current schematic only) or project-level (available for use across all schematic sheets and PCB documents in the project). Parameters can also be added to a variant in the Edit Project Variant dialog.

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. Altium NEXUS resolves this in the following way:

  1. Variant (highest priority)
  2. Schematic document
  3. Project

This means that the parameter value defined in the schematic document overrides the value defined in the project options, and the value defined in the variant overrides the value defined in the schematic document. Note that schematic-level parameters are not available on the PCB or in the BOM. For these types of output, you should use project or variant parameters.

Parameters can also be added to a Sheet Symbol object. If parameters with the same name are created at different levels of the project, including the Sheet Symbol placed on the parent schematic sheet, this situation will be resolved on the child schematic in the following way:

  1. Variant (highest priority)
  2. Schematic document
  3. Sheet Symbol
  4. Project

To see the value of the parameter of the sheet symbol above, select a compiled tab at the bottom of the design space.

► Learn more about Multi-sheet & Hierarchical Designs

Placing a Special String

To use a special string on a schematic, place a text object and set its text to be one of the special string names.

On a schematic sheet, special strings are characterized by the prefix '=' (e.g., =CurrentTime, =CurrentDate, etc.). The list of available special strings – both predefined and user-defined document-level and project-level parameters – can be seen when a Text String is selected, by clicking the drop-down arrow associated with the Text field in the Text mode of the Properties panel.

Parameters defined at the variant level are not listed. Such a parameter can be referenced using the special string notation (i.e. =<VariantParameterName>). The value of the parameter will be displayed only when the associated variant for which it is defined is made the current variant.

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

To assist in identifying Text String objects that are using special strings, the names of the special string can be shown on the schematic sheet. When the Display Name of Special String option is enabled on the  Schematic – Graphical Editing page of the Preferences dialog, each special string has its name displayed as a faint superscript (note that these superscripts will not be printed).

Concatenating Special Strings

Multiple special strings, along with regular text (fixed strings), can be concatenated into a single text string, according to the following rules:

Element Function Example Returns
= (equals) Indicates that the following string is an expression that must be interpreted. =Project Kame_FMU for the example project named Kame_FMU.PrjPcb
+ (plus) Used to concatenate the special string and fixed string elements required in the string. =Project + VariantName Kame_FMUDefault for the Default variant in the example project
' ' (single quotes) Used to include a fixed string anywhere within the required string. ='Project: ' + Project + ', Variant: ' + VariantName Project: Kame_FMU, Variant: Default  for the Default variant in the example project

Special strings can be concatenated with text and other special strings.Special strings can be concatenated with text and other special strings.

Active Links from Designators and Net Names

Component designators and net names can be included in Text Frames and Notes and function as Active Links, providing cross-probing capabilities within the schematic and also in generated PDFs. 

The link is defined as active in the Properties region of the Text Frame or Note in the Properties dialog, by typing the @ character followed by the Designator or Net name. A selection list will appear as you type, use it to select the desired object. 

Type the @ character to display a list of designators and net names, continue to type to search the list.Type the @ character to display a list of designators and net names, continue to type to search the list.

Active Links are highlighted by a box in the Text Frame or Note, click to cross probe to that component or net. Changes to a Designator value or a Net name are automatically applied to existing Active Links.

Each live link is highlighted by a box, click on a link to cross probe to that component or net.Each live link is highlighted by a box, click on a link to cross probe to that component or net.

The Zoom and Dimming levels used when you click on a link in the schematic editor are configured in the System - Navigation page of the Preferences dialog.

The Zoom level used in the PDF is defined in the Schematic PDF Settings dialog (PDF from an OutputJob), or the Smart PDF Wizard. 

 

If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.
Content