Copy a clump of components from one project to another?

Upverter Support
#1

Hello
Relatively new here. I have two project files going - each already has a mostly complete schematic and the components have already been laid out in layout mode complete with traces and all.

However, I now have a need to copy an entire “clump” of about 150 components from one project to the other. I don’t want to have to redraw that part of the schematic over again, or lay it out again either. It would be super amazing to just use old fashioned copy and paste but that doesn’t work here, from one project to another, as far as I can tell. I’d even settle for being able to copy the schematic only, if not possible to copy that AND that part of the layout, too.

I saw one other post asking this same or similar question, the answer was to use “Extract Module” but there are two things that come to mind: 1. I can’t figure out how to use that, or find an explanation as to its use, and 2. I have a feeling that’s not exactly what I needed anyway.

Thoughts? Thanks!

1 Like
#2

i think if there is a method to copy things which are same at the same category , it’ll be helpful

1 Like
#3

Hi there!
Extracting and adding a “module” is currently the only way you can accomplish this. The steps involved go like this:

  1. In schematic, click the knife tool. The tooltip reads ‘Extract Module’

  2. Select all of the symbols for the components you want to transfer.

  3. Also select all of the wires for the traces you want to keep.

  4. Click the checkmark next to the knife tool, at which point you will be taken to a new workspace that has these parts and wires in it.

  5. Review and make changes to the schematic that might make it more universally useful so that you might be able to re-use it. This can be done later without impacting your current project, however it will be possible to apply any changes you make to the module into any design that uses it.

  6. Any signals you would like to connect to from your project will require a flag. These will be made available to you when you create a schematic symbol for the module.

  7. Switch to layout. The traces associated with the wires the schematic will be carried over. You’ll want to check for unwanted stubs and unconnected traces.

  8. Once the schematic and layout for the module is to your liking click the ‘publish module revision’ button above the workspace. This will ask for a revision title and rationale. It will also ask you to create a schematic symbol. The simplest way to do this is to go to the pins panel on the right and click ‘handle unassigned’.

  9. In the Attributes panel, open the attribute manager, give your module a part ID, “manufacturer” and a description, and click save on the dialog

  10. Click ‘save’ at the bottom of the symbol editor.

  11. You can now save the module revision and go into the target design.

  12. Click components, then the Modules button in the top-left corner, and then search for your module (if you haven’t changed its name, it will be “Module Extracted From .” This will be a private project in your dashboard and can be edited in the same way as any other project).

  13. add the part and connect it as you would any symbol. When you switch to the layout view, the parts and traces will be linked as if they are a single component. You can unlink the layout components if you need to edit all or part of it. To do that, click on the module symbol in schemaitc, open properties and check the ‘unlink layout components’ box and click save.

Here’s a Gotcha:
If you have included copper layers other than “Top” and “Bottom,” you may have issues with your layout. I tried exporting a module that included 2 internal signal layers and they caused problems when I tried to open the layout tool.

I hope this helps. I am planning related course material in Upverter Education but it’s not ready yet.

Best,
Keith

1 Like
#4

Keith,
FANTASTIC! This mostly worked for me and saved me a ton of time. Thank you!!

Some notes, might be a bug: After completing step 4, it “appeared” as if nothing had happened. I assumed maybe the browser was slow and working hard on something so I let it sit. After about 2 minutes, the whole browser flashed white and reloaded from scratch. I proceeded to step 5, my schematic was intact. Layout mode still had all of my components in their relative positions, but all traces and vias were gone. Even so, this still saves me a great deal of time and effort, I’ll gladly re-run my traces, I am just happy I didn’t have to redraw the whole schematic.

I found the optional part of step 13 useful, I like being able to break it back out into schematic form in my target project, although I can see how having it represented as one neat little module “component” can be handy sometimes as well.

I only had a two-layer design, so I wasn’t able to test the four-layer.

Definitely one worth putting in the Education page.

Thanks again!