Creating a Schematic Template in Altium Designer

When applied to a schematic sheet, a schematic template defines the size, graphics (such as title block), and the list of sheet-level parameters of the sheet. You can create your own set of schematic templates to help provide consistent-looking schematics created by you or your entire team.

Creating a Workspace Schematic Template

To create a new schematic template in your connected Workspace:

1. Open the Templates tab of the Data Management – Templates page of the Preferences dialog.

2. Select the Schematic command from the menu of the Add button or the context menu of the template grid.

   

3. 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.

4. 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 the use of a default title block, and set margin and zones;

      

     Do not select Template in the Formatting and Size region of the panel and choose a template. Doing this means you are applying a template to your new template; if you do, your template will not behave correctly.

5. 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.

   

6. Using drawing objects (line, image, etc.), define the look of the schematic template. For example, if you opted not to 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).

   
   An example custom title block created using line and text objects.

7. 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 the Drawn 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.

   
   An example custom title block with special strings added. These special strings will be updated with actual parameter values when the template is applied to a schematic sheet.

   When creating a schematic sheet template, it is recommended not to use spaces in the names of parameters that are used as special strings - when applying such a template to a schematic sheet and parameters with spaces in their names are not added to the sheet from the templates, an apostrophe character (') or the #NAME? string will be shown on the sheet instead of the actual parameter name.

8. Save the template to the connected Workspace by selecting the File » Save to Server command from the main menus. The Edit Revision dialog will open 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:

1. Open the schematic template within Altium Designer.

2. Choose the File » Save to Server command from the main menus.

   The file must be locally saved (File » Save) prior to saving to the Workspace.

3. The Choose Planned Item Revision dialog will open. In the dialog, choose the target schematic template item for the next revision (or an established revision in the Planned state) of which the sheet will be saved, then click OK.

   If the target Schematic Template Item doesn't exist, you can create it through the Choose Planned Item Revision dialog on the fly in the chosen Workspace folder by right-clicking in the revision list region of the dialog (or, if the folder does not contain any item yet, by clicking the Add an item control) and selecting the Create Item » Schematic Template command. If doing so, be sure to disable the Open for editing after creation option (in the Create New Item dialog), otherwise you'll enter direct editing mode.

4. The Edit Revision dialog will open in which you can define the Name and Description and add release notes as required.

5. After clicking OK, the template will be saved and stored in the revision of the Item.

Example of sending an existing schematic template to the Workspace to which you are currently connected.

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 in the next revision of the schematic template.

Creating a Local Schematic Template

A local schematic template can also be created. To do this:

1. Create a new schematic document by selecting the File » New » Schematic command from the main menus.

2. Use the document to define the schematic template as required and described above.

3. Select the File » Save As command from the main menus. In the Save As dialog that opens, 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 select Advanced 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).