Creating a Schematic Template in Altium Designer
When applied to a schematic sheet, a schematic template defines the size, the graphics (such as title block) and the list of sheet-level parameters of this sheet. You can create your own set of schematic templates to facilitate providing consistent-looking schematics created by you or the entire team.
Creating a Workspace Schematic Template
To create a new schematic template in your connected Workspace:
- Open the Templates tab of the Data Management – Templates page of the Preferences dialog.
-
Select the Schematic command from the menu of the Add button or the context menu of the template grid.
- After selecting the command, click OK in the Close Preferences dialog that opens to close the Preferences dialog and open the temporary schematic editor. A planned revision of the new schematic template will be created automatically in a Workspace folder of the
Schematic Templates
type. -
Configure options of the design space using the General tab of the Properties panel in its Documents Options mode:
-
in the General region of the panel: select the units and configure the grid options;
-
in the Page Options region of the panel: select Standard or Custom and configure the provided options as required – set sheet size and orientation, enable or disable use of a default title block, and set margin and zones;
-
-
Define the set of parameters on the Parameters tab of the Properties panel in its Documents Options mode. These parameters will become sheet-level parameters of the schematic sheet to which the template will be applied. Use the controls at the bottom of the panel to add and remove used-defined parameters.
-
Using drawing objects (Line, Image, etc.), define the look of the schematic template. For example, if you opted to not include a default title block, create a custom title block using these objects.
You can also use Text String objects to define the static text strings of the template, i.e. the text that will not be changed on a schematic sheet (e.g.
Drawn By
text).
-
Use Text String objects as Special Strings to define placeholders for design or system information that will be substituted with parameter values when the template is applied to a schematic sheet. Define the Text property of a selected Text String object in the format
=<ParameterName>
. When applied to a schematic sheet, this Text String will show the value of the parameter with the same name. This can be a sheet-level parameter (predefined or user-defined), a project-level parameter, or a variant-level parameter.For example, a Text String with the
=DrawnBy
text will show the value of theDrawn By
parameter (where, for example, the name of the designer is entered) when the template is applied to a schematic sheet.Learn more about Special Strings.
- Save the template to the connected Workspace by selecting the File » Save to Server command from the main menus. The Edit Revision dialog will appear, in which you can define the Name and Description of the Schematic Template Item being created in the Workspace, and add release notes as required.
The template can now be applied to a schematic sheet: learn more.
Saving an Existing Local Schematic Template to the Workspace
If you have an existing schematic template (*.SchDot
), you also have the ability to save this template directly to the Workspace. The process is as follows:
- Open the schematic template within Altium Designer.
-
Choose the File » Save to Server command from the main menus.
-
The Choose Planned Item Revision dialog will appear. Use this to choose the target Schematic Template Item into the next revision (or an established revision in the
Planned
state) of which the sheet will be saved, then click OK. - The Edit Revision dialog will appear, in which you can define Name, Description, and add release notes as required.
- After clicking OK, the template will be saved and stored in the revision of the Item.
Editing a Workspace Schematic Template
At any stage, you can come back to a schematic template in the Workspace and edit it. From the Templates tab of the Data Management – Templates page of the Preferences dialog, right-click on the template entry and choose the Edit command from the context menu. The temporary editor will open, with the template contained in the revision opened for editing. Make changes as required, then save the document into the next revision of the schematic template.
Creating a Local Schematic Template
A local schematic template can also be created. To do this:
- Create a new schematic document by selecting the File » New » Schematic command from the main menus.
- Use the document to define the schematic template as required and described above.
-
Select the File » Save As command from the main menus. In the Save As dialog that appears browse to the local templates folder for your installation of Altium Designer (denoted in the Local Templates folder field at the bottom of the Data Management – Templates page of the Preferences dialog;
C:\Users\Public\Documents\Altium\AD<Version>
for the default installation), enter the desired name of the template and selectAdvanced Schematic template (*.SchDot)
from the Save as type drop-down.
Local schematic templates will be listed on the Templates tab of the Data Management – Templates page of the Preferences dialog, in the Local region of the grid (visible only if the Template visibility option is set to Server & Local
on this page).