How do I create PCB Templates?

[budi]

       PCB Template files (and Projects) are just normal PCB documents (*.PcbDoc, or Projects, *.PrjPcb) that are usually saved in the ...\Altium Designer\Templates  folder.  There are a number of example templates in that folder.  Templates can contain board outlines, title blocks, or any other information that can be placed onto a regular PCB.

To get started, create a new PCB document by going to File » New » PCB.  To set up the board, follow the instructions below:

    * Board options such as grids and sheet position can be controlled through the Board Options dialog ( Design » Board Options )

    * A default layer stackup can be created through the layer stack manager ( Design » Layer Stack Manager )

    * A board outline can be created by drawing primitives on a mechanical layer, selecting them, then using Design » Board Shape » Define From
       Selected Objects.  Alternatively, a DXF file could be imported, then used in the same manner.

    * Borders, dimensions, and title blocks can be placed as usual on mechanical layers, using the appropriate primitives.

    * To place information that may change between documents, such as file names, use special strings.  These can be placed by using Place »
       String, then pressing Tab, and using the drop down box labeled Text in the dialog box that appears.  By default, these are shown as, eg,
       .Layer_Name .  To replace them with the correct text, bring up the Board Layers & Colors dialog ( shortcut L ), choose the View Options tab,
       and tick the box labeled Convert Special Strings.

    * It is also possible to link title blocks, reference zones, etc. to the sheet, so that they are turned on and off with the sheet.  To do this, go to
       the Board Layers and Colors dialog ( shortcut L ), find the mechanical layer that the information is on, and tick the box labeled Linked to Sheet.

        Once the template is finished, save it as a normal .PcbDoc file.  To use it, go to the Files panel ( View » Workspace Panels System » Files ), and go down the list to the heading New from Template; it may be necessary to collape other parts of the panel using the up arrows next to the other headings.  Under the New from Template heading, click on PCB Templates.  Altium Designer will then ask which template to use - select the file that was created earlier, and a new PCB file will be created from that template.

Note: Unlike schematic templates, it is not possible to apply a PCB template to a document which already exists.  If a template is required, it must be selected when the document is initially created.