2
\$\begingroup\$

I have some pads and tracks that are different primitives but are the same net in an Altium layout.

Altium keeps flagging these as ShortCircuit DRC violations, but they're the same net, so I don't want to keep seeing these come up.

How can I shape a DRC rule to ignore shorts between nets that are the same?

Thanks

\$\endgroup\$
3
  • 1
    \$\begingroup\$ I guess I have not enough information to answer your question. Screenshot? Why should Altium flag something as short circuit, if it is the same net?? Are they different nets, but logical the same, like PowerGND and GND? then you should look into Net Ties. \$\endgroup\$
    – jwsc
    Commented Mar 16, 2016 at 15:05
  • \$\begingroup\$ Are you sure that there is no another track (that you don't see maybe, below)? Try to switch to Transparent view configuration and look at the tracks..Or, check if your track is linked to correct net (double click or PCB inspector for track) \$\endgroup\$
    – Haris778
    Commented Mar 16, 2016 at 15:12
  • \$\begingroup\$ The DRC report should tell you the objects and nets, can you post the exact message from the report? \$\endgroup\$
    – Evan
    Commented Dec 4, 2016 at 18:56

3 Answers 3

Reset to default
2
\$\begingroup\$

If you are getting a short circuit DRC error, then your nets are not the same. I would double and triple check that you are correct (a zoomed in screenshot would help.)

There is a short circuit rule you can mess around with. It's right under "Clearance," but I am inclined to think (with the information at hand,) that your nets are not the same (not in Altium's eyes anyways.)

\$\endgroup\$
2
\$\begingroup\$

Do you have the "Different Nets Only" option selected in the Clearance rule?

Design Rules

\$\endgroup\$
6
  • \$\begingroup\$ Wouldn't the clearance just indicate how close you can be ? I do not believe the error would be short circuit, it will most likely give you a clearance error. \$\endgroup\$
    – efox29
    Commented Mar 16, 2016 at 15:08
  • \$\begingroup\$ If it's not the clearance rule that creates a short circuit error, then I don't know which rule it is! \$\endgroup\$
    – Armandas
    Commented Mar 16, 2016 at 15:11
  • \$\begingroup\$ I just noticed on your picture the short-circuit clearance ! lol \$\endgroup\$
    – efox29
    Commented Mar 16, 2016 at 15:22
  • \$\begingroup\$ @efox29 Again, this rule allows you to have short circuits in your design. This is not something you should enable in a normal PCB. \$\endgroup\$
    – Armandas
    Commented Mar 16, 2016 at 15:24
  • \$\begingroup\$ I agree. But the rule allows you to select which nets are allowed to short, and if OP wants to remove his errors where he is sure is a false error, the option is there. \$\endgroup\$
    – efox29
    Commented Mar 16, 2016 at 15:30
2
\$\begingroup\$

As others are mentioning, the Short Circuit DRC violation is likely appearing if the primitives you're working with are not actually on the same net. A good way to check this is by double clicking one of the tracks with a violation and check the net shown (red box below) matches the net of pad it's connected to.

Checking the net of a track

One possible cause: it sometimes can be tempting to try "Place" then "Line" to create traces (shortcut "p", then "l") rather than using the standard interactive routing mode (shortcut "p", then "t"). Placing lines defaults to "No Net" for any tracks created, while the interactive routing mode will default track nets to match whatever pads they originate from.

\$\endgroup\$
1
  • \$\begingroup\$ Thank you. but I don't understand why Altium doesn't automatically add this Net parameter, while we start a Line from that specific Net? \$\endgroup\$
    – 2i3r
    Commented Jul 16, 2021 at 14:48

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.