DipTrace Forum
http://www.diptrace.com/forum/

Pad connecting to wrong net
http://www.diptrace.com/forum/viewtopic.php?f=4&t=11779
Page 1 of 1

Author:  bdring [ 03 Sep 2017, 11:47 ]
Post subject:  Pad connecting to wrong net

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.

Author:  Tomg [ 03 Sep 2017, 16:42 ]
Post subject:  Re: Pad connecting to wrong net

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.

Author:  bdring [ 04 Sep 2017, 09:41 ]
Post subject:  Re: Pad connecting to wrong net

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.

Author:  Tomg [ 04 Sep 2017, 10:43 ]
Post subject:  Re: Pad connecting to wrong net

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?

Author:  bdring [ 04 Sep 2017, 12:01 ]
Post subject:  Re: Pad connecting to wrong net

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.

Author:  Tomg [ 04 Sep 2017, 12:58 ]
Post subject:  Re: Pad connecting to wrong net

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?

Author:  Alex [ 05 Sep 2017, 02:47 ]
Post subject:  Re: Pad connecting to wrong net

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.

Page 1 of 1 All times are UTC - 5 hours [ DST ]
Powered by phpBB © 2000, 2002, 2005, 2007 phpBB Group
http://www.phpbb.com/