Updating Component Connections from Schematic - Page 1
Forum section: electronics / general

author: themadhatter106
author_rank: Newbie
timestamp: March 27, 2015, 06:30:48 pm
content: Hi,So I am making my first PCB in DipTrace but I have a problem. I found a component connection in the PCB that does not reflect the schematic. It's just plain wrong. I found that the net which is in the schematic file is missing from the PCB file. I want all of the nets in the schematic file to be the same as the nets in the PCB file. Using the renew from schematic function does not seem to do this.How do I make sure that all of the connections in the schematic file are the same as the connections in the PCB file. There may also be other errors that I didn't happen to notice and I want to compare the two.Any help is much appreciated. Thanks.

author: BloodyCactus
author_rank: Frequent Contributor
timestamp: March 27, 2015, 11:06:32 pm
content: I dont quite get your question.try File -> Renew Desgin from Schematic -> Related Schematicthis will bring any changes from schematic to pcb.

author: John Coloccia
author_rank: Super Contributor
timestamp: March 27, 2015, 11:34:33 pm
content: If you post the files, and which net you're talking about, maybe someone here will look at it.

author: Farley
author_rank: Regular Contributor
timestamp: March 28, 2015, 12:36:01 am
content: This usually happens when a net gets disconnected while editing the schematic. Drag the offending net (wires) coming from the component in question around (in the schematic) and you'll notice that it is not connected to anything.The easiest fix is to delete the wire in the schematic and reconnect it. After that do a renew from schematic.Each time I've encountered this issue it is because of something I've done. More often than not it occurs where wires meet at a junction or where I've changed components.

author: sleemanj
author_rank: Super Contributor
timestamp: March 28, 2015, 01:35:42 am
content: Quote from: themadhatter106 on March 27, 2015, 06:30:48 pmVerification > Compare To Schematic

author: themadhatter106
author_rank: Newbie
timestamp: March 30, 2015, 06:42:06 pm
content: Hi,Thanks for the suggestions. I am attaching the schematic and PCB files. The main problem is with Net 91. Looking at CT2, on the schematic pin 2 is connected to Net 24 and pin 1 is connected to Net 91. On the PCB both pins are connected to Net 24. Renew from related schematic does not fix the issue, even when deleting the component and Verification > Compare To Schematic says there are no errors when there is actually a problem.

author: DerekG
author_rank: Frequent Contributor
timestamp: March 30, 2015, 07:57:55 pm
content: Quote from: themadhatter106 on March 30, 2015, 06:42:06 pmWhat happens when you select (in PCB Layout):VerificationCheck Net ConnectivityI have looked at both your schematic & your layout. I have not added your components to any of my libraries.I believe the problem originates from the manual cleanup of your pcb.

author: John Coloccia
author_rank: Super Contributor
timestamp: March 30, 2015, 08:56:28 pm
content: Go to the schematic, right click on the component and select "Attach Pattern". If you hover your mouse over the pads, you'll see that they're connected to each other. When you changed the pattern, you accidentally also dragged a ratline from pad1 to pad2. If you want to see this better, in the Attach Pattern view, move the component a bit so that you can clearly see the ratlines (just right click in the window and drag, just like scrolling in the PCB or Schematic view). The ratline in question is an error, and shows up red, I think. To fix, simply click and drag a ratline from pad1 to pad2 again, and it will ask if you want to disconnect the one that's there. Do that, and your problem is solved.

author: themadhatter106
author_rank: Newbie
timestamp: March 31, 2015, 01:04:33 am
content: Quote from: John Coloccia on March 30, 2015, 08:56:28 pmWow! Thanks. That fixed the problem. I never would have thought of that myself!