Pad connecting to wrong net

Making PCB Layouts, Manual routing, Auto-routing, Copper pouring, Updating from Schematic, Manufacturing Output
Post Reply
Message
Author
bdring
Posts: 4
Joined: 13 Jul 2017, 10:26

Pad connecting to wrong net

#1 Post by bdring » 03 Sep 2017, 04:47

Some pads are connecting to the wrong net. I have a USB connector with one pin connecting to a "Gnd" and several connecting to an "Earth" net. In layout all pins are connecting to the "Gnd" net. I have attached images of the schematic and layout. I am highlighting the "Gnd" net in the layout image. You can see the incorrect pins highlighting on the USB connector.
Attachments
Layout
Layout
layout1.png (34.69 KiB) Viewed 323 times
Schematic
Schematic
schm1.png (20.94 KiB) Viewed 323 times

Tomg
Expert
Posts: 2028
Joined: 20 Jun 2015, 07:39

Re: Pad connecting to wrong net

#2 Post by Tomg » 03 Sep 2017, 09:42

Try right-clicking on one of the errant pins and selecting "Delete from Net" in the pop-up menu. (Be ready with the Undo tool just in case.) If that is successful, do the same thing for the rest of the errant pins. Once all of the errant pins have been disconnected, re-connect them one-by-one (right-click > Add to Net > etc.) to the desired Net. Let me know what happens when you run the Renew Layout from Schematic tool. If that blows it up again, you might have to use the "By RefDes..." option first to fix it (make sure the reference designators are the same as the schematic's). If that is successful, then you should be able to use the "By Components..." option after that.
Tom

bdring
Posts: 4
Joined: 13 Jul 2017, 10:26

Re: Pad connecting to wrong net

#3 Post by bdring » 04 Sep 2017, 02:41

Thanks Tom,

I was able to complete my project with that fix. If I renew "By RefDes" it does not create any design rule violation markers, but it does fail the "Check Net Connectivity"

It is strange that both the schematic and the layout have the exact same connections in "Connection Manager", but the "Earth" net is lost when imported into the layout.

Tomg
Expert
Posts: 2028
Joined: 20 Jun 2015, 07:39

Re: Pad connecting to wrong net

#4 Post by Tomg » 04 Sep 2017, 03:43

bdring wrote:"...the "Earth" net is lost when imported into the layout..."
I think DipTrace requires that a Net have a minimum of two component pin connections before it can make an appearance on the PCB. (Netport pins do not count as component pins.) What kind of a "Net Connectivity" failure are you seeing?
Tom

bdring
Posts: 4
Joined: 13 Jul 2017, 10:26

Re: Pad connecting to wrong net

#5 Post by bdring » 04 Sep 2017, 05:01

The Earth net is being lost and all connections are moving to the Gnd net.

I don't think the are any Netports. The image on the original post shows (6) pins from J1 and one each from C2 and R4.

Here is the Connection Manager from the Schematic. You can see all connect to Earth but when imported into Layout these all go to Gnd.
Attachments
Schematic Connection Manager
Schematic Connection Manager
con_manager.png (13.78 KiB) Viewed 305 times

Tomg
Expert
Posts: 2028
Joined: 20 Jun 2015, 07:39

Re: Pad connecting to wrong net

#6 Post by Tomg » 04 Sep 2017, 05:58

bdring wrote:"...The Earth net is being lost and all connections are moving to the Gnd net..."
Have you tried disconnecting the Nets from C2(2) and R4(1) and then reconnecting those pins to the correct Net? If this doesn't work, would you be willing to attach your DipTrace files here so I can try to find the problem?
Tom

Alex
Technical Support
Posts: 3897
Joined: 13 Jun 2010, 23:43

Re: Pad connecting to wrong net

#7 Post by Alex » 04 Sep 2017, 19:47

Please right click on J1 in schematic and open "Attached Pattern". Make sure there is no internal connection from pad 5 (GND) to pads 6 through 11 (Case). If there is internal connection then disconnect pad 5 from pads 6-11, save schematic and renew board from schematic.

Post Reply