Adding part to component does not show up in schematic

Drawing Schematics, Hierarchical Design, BOM, Exporting net-lists, etc.
Post Reply
Message
Author
guitardenver
Posts: 3
Joined: 14 Feb 2018, 11:10

Adding part to component does not show up in schematic

#1 Post by guitardenver » 14 Aug 2020, 17:23

Hello,

When making a multi-part component. In my case it had 13 parts. This part was used in the design and is all wired up on schematic and PCB.

I wanted to split the component up more to 14 parts. So I added the 14th part in component editor and saved.

When I go back to the schematic and click "Update Component From Library"->"Selected Component", it updates only the original 13 parts. The 14th part does not show up. I tried "Select Parts" and "Replace Part".

When I add a completely new part from the library, the 14th part is there. But I have to re-wire it.

How do I get my new part to show up in the existing schematic?

Tomg
Expert
Posts: 1571
Joined: 20 Jun 2015, 14:39

Re: Adding part to component does not show up in schematic

#2 Post by Tomg » 14 Aug 2020, 22:44

It depends upon how you split up the component. The safest path would be to place a new instance of the component (all 14 parts) into the schematic and rewire. Because of the way it has been changed, you have essentially made a completely new and different component. But if you are determined to try an unknown path, go ahead and update the current component. Then select the same component from the library list on the left side of the screen, choose "Part 14" and place that part into the Design Area. Compare all 14 parts to what is in the library before continuing with your project. Don't forget to run the ERC.

If the parent RefDes of newly-placed part "14" doesn't match the parent RefDes of the original component...
1) Double-click on newly-placed part "14" to bring up the Component Properties dialog window.
2) In the Component Properties dialog window click on the [Parameters] tab, make sure the [x]Enable Parts option is active, change the parent RefDes to match the parent RefDes of the original component, make sure the Part RefDes is "14" and click on OK.
3) If a "...part will be moved to..." warning pops up, click on OK.

p.s. Assuming the new parts have the same pin locations as the originals, rewiring a new component into the circuit can be made a little more tolerable by using the "Disconnect Wires" selection in the right-click context menu for each of the original component's parts and then deleting them. The wires should remain intact. Next, move the new component's parts into the same locations formerly occupied by the original's parts (where possible) while using the "Connect Wires" option in the right-click context menu to reconnect the nets (or manually extend the wires to the correct pins). Double check the parent RefDes to make sure it is the same as the original and run the ERC.
Tom

guitardenver
Posts: 3
Joined: 14 Feb 2018, 11:10

Re: Adding part to component does not show up in schematic

#3 Post by guitardenver » 17 Aug 2020, 10:41

The problem with placing a completely new part using "disconnect wires" is that when you update the PCB layout via schematic, the part is new and completely un-routes the part and puts it to the side. Re-routing a 180pin BGA is not going to be an option. Unless there is a solution to prevent it from doing that as well.

However, your other suggestion seems to work. I just added Part 14 and it had the same refdes and PCB layout did not move the existing part at all. It seems to have linked it to the original part.

Thanks for that tip!

Tomg
Expert
Posts: 1571
Joined: 20 Jun 2015, 14:39

Re: Adding part to component does not show up in schematic

#4 Post by Tomg » 17 Aug 2020, 11:09

guitardenver wrote:
17 Aug 2020, 10:41
The problem with placing a completely new part using "disconnect wires" is that when you update the PCB layout via schematic, the part is new and completely un-routes the part and puts it to the side. Re-routing a 180pin BGA is not going to be an option. Unless there is a solution to prevent it from doing that as well.
There is. Try the Renew Layout from Schematic tool using its "By RefDes..." option the first time around. This should re-link the hidden identifiers between the component in the schematic and the component in the PCB without messing up the original traces.

If that doesn't work...
1) Use the "Disconnect Traces" selection in the right-click context menu for the PCB component to preserve the traces during the next step.
2) Run the "Renew Layout from Schematic" tool. The original component should vanish and a new one should appear to the right of the PCB.
3) Move the new component into position to match up with the traces and use the "Connect Traces" selection in its right-click context menu.
Tom

Post Reply