Working with Text Objects on a Schematic in Altium Designer

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.

Text Strings, Text Frames, and Notes

Altium Designer supports text strings, text frames, and notes.

Placed text string, text frame, and note (in its expanded and collapsed modes).

Placing a Text Object

Text strings, text frames, and notes are available for placement by using the Place » Text String, Place » Text Frame, and Place » Note commands of the corresponding editor's main menus, respectively.

After launching the command, the cursor will change to a cross-hair and you will enter text object placement mode.

• For the text string, it will appear floating on the cursor. Position the object then click or press Enter to effect placement.
• For the text frame or note, position the cursor and click or press Enter to anchor the first corner of the object. Move the cursor to adjust the size of the object, then click or press Enter to complete placement.

Continue placing further text objects or right-click or press Esc to exit placement mode.

Additional actions that can be performed during placement while the text object is still floating on the cursor (and, for a text frame or note, before its first corner is anchored) are:

• Press the Alt key to constrain the direction of movement to the horizontal or vertical axis depending on the initial direction of movement.
• Press the Spacebar to rotate the text object counterclockwise or Shift+Spacebar for clockwise rotation. Rotation is in increments of 90°.
• Press the X or Y keys to mirror the text object along the X-axis or Y-axis.

Toggling the Display Mode of a Note

A placed note can be displayed in either expanded (fully expanded) or collapsed (small triangle) modes. Toggle the display mode by clicking on the top left corner of a placed note.

Click the triangle in the top-left corner to collapse a note.

When a note is in collapsed mode, hover the cursor over it to access a pop-up containing the name of the note's author and the actual text content of the note.

Hover over a collapsed note to display information.

Graphical Editing of Text Objects

When a text object is selected in the design space, you can change its location and orientation graphically. For a text frame and note (when fully expanded), you can also graphically change its size or shape using the available editing handles.

Selected text objects

• Click anywhere inside the dashed box (for a text frame or note, away from editing handles) and drag to reposition the text object as required. While dragging, the text object can be rotated (Spacebar/Shift+Spacebar) or mirrored (X or Y keys to mirror along the X-axis or Y-axis).
• Click and drag A to resize the text frame / note in the vertical and horizontal directions simultaneously.
• Click and drag B to resize the text frame / note in the vertical and horizontal directions separately.

The textual content of a text string, text frame or note (fully expanded) can be edited in-place, which enables you to edit text entries directly in the design space rather than having to edit through the Properties panel – refer to the Schematic Placement & Editing Techniques page to learn more. Note that if the Word Wrap option is disabled in the Properties panel for the selected text frame / note, a horizontal scroll bar will also be available when editing the text in place – show image.

Properties of Text Objects

Schematic text objects have a range of configuration options. Open the Properties panel for one or more selected text objects to edit their properties. 

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 Designer 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.

Placing a Special String

To use a special string on a schematic, place a text object and include a special string name in its text.

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.

Accessing special strings for a placed text string object.

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:

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

Truncating Special Strings

Special strings can also be truncated using the Copy() and Length() functions. The example below shows how to remove the file extension from a schematic document:

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.

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.

Hyperlink Text Strings

A text string can be turned into a hyperlink to a website page, or to a document on a local or shared drive by entering a target URL into the URL field in the selected Text String object's Properties panel. This offers a fast, convenient alternative when providing access to datasheets for components used in a design. Such text strings can also provide a beneficial link to your own organization's website, within the title blocks of your schematic source documents.

Once a URL has been configured as required, it can be used from within the design space. To do so, hover the cursor over the text string. After a short delay, a pop-up with the URL will appear. Click this to open the URL either within Altium Designer or in an external browser, in accordance with your defined preference.

Following an example hyperlink to its target URL.

The pop-up containing the URL is a feature of the software's Design Insight System. Specifically, it is obtained by enabling the Hyperlink Insight aspect of the system. This is done on the System – Design Insight page of the Preferences dialog. As with other elements of the system, you can configure the launch style for the pop-up – Mouse Hover and/or Alt+Double Click.

Alternatively, a link can be followed by right-clicking over it and accessing the URL from the Hyperlink sub-menu. This would be the way to follow a link if Hyperlink Insight is disabled.

Access the URL for a text string from the right-click menu.