Can you please tell me if there is a way to import/copy all parameters (Design>Document options-Parameters) (at once) from other project in which I have already added. Or is there a way to make my parameters as default so they already exist when I create a new project. So that they can be included in BOM.

There are about 30 parameters (company requirement). And I don't want to add 30 parameters manually each time I create project.

There is one project complete with schematics and PCB layout in which these parameter exist and

There is another project also complete with schematics and PCB layout in which I need to add these parameters

parameters in yellow circle are few which I want to add in my another project parameter

  • \$\begingroup\$ For any readers interested in this topic: The same question was duplicated at Stack Overflow and was replied to there. \$\endgroup\$ – SamGibson Jul 22 '18 at 16:04

Yes, this is possible though probably not as straightforward as you want it. I don't believe there's a "bulk copy" type feature for copying all parameters and values between projects, but you can modify the schematic template to ensure that the proper parameters (and values) are populated when you create a new project.

First, find where the schematic template file you're using (or want to use) is located and open it for editing. For example, I'm using a custom schematic template for an 11x17 piece of paper called 11x17.SchDot

Open the document options by selecting Design > Document Options and clicking the "Parameters" tab as shown below.

enter image description here

I added a value called "TestValue" by clicking the "Add..." button and entering my desired parameters.

Then, I can open a schematic (or create a new schematic) and if this is the default schematic template for new schematics, it should already have the "TestValue" parameter in the document options. If it's not the default, or if you want to apply the template changes to an existing schematic/project, select Design > Templates > General Templates > Choose Another File... and load the template that you applied parameter changes to. You should see the following dialog pop up:

enter image description here

You can apply the template changes to all schematic documents in the current project, and likewise, you can choose to either only add new parameters that are in the template but not in the current document, or you can replace each matching parameter with the specified value.

If this is something you do for every new project, I suggest you copy the desired schematic template file from the default location to a common/custom location and give it a name that will differentiate it from the defaults (e.g., COMPANY_NAME_A4.SchDot) Then, in your Altium Designer preferences, ensure that the defaults are configured to use this template in new projects.


Remember that the parameters you showed are all local to the schematic. To have these parameters in all schematics of your project, select them and tap crtl + C. Then, go to Project > Project Options... tab Parameters and paste.

Now, if you want to have these parameters in another project, only copy and paste these parameters with the same steps.

To make this automatic in new projects and/or schematics, you can create an new schematic and/or project, set the parameters and save in some folder for templates. Then, go to DXP > Preferences and System > New Documents Default. In File Templates you can select your schematic/project template and every time you add a new one they will have that parameters.



Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.