0
\$\begingroup\$

I made design rule for the power nets to ensure the minimum track width was being achieved. However, when I wanted to changed the rules, I had to go through each of the parameter set icons and update them individually. Is there a way to update all the net parameters belonging to the same class all at once?

\$\endgroup\$

1 Answer 1

0
\$\begingroup\$

There are a few steps here that I would take, and I'm not entirely sure which part you are needing help with.

  1. In the schematic editor, the parameter set directive gives the net a Net Class Name. These are tiny or large red circle objects attached to the net. (I find it odd that the only choices are "tiny" and "large.")

    Parameter Set: Net Class Name

  2. To select all parameters sharing the same class name, use the Edit > Find Similar Objects menu command or Shift+F and then click one of the parameter set directives that you want to change. Ensure that you have all project documents selected (if that's what you want) and change the "ClassName" property filter from "Any" to "Same."

  3. Modify the class name to change all selected net classes to some other class, etc. as needed.

  4. Push the changes to your PCB to ensure that net class membership is the same as the schematic. (Design > Update PCB Document)

  5. Modify the clearance and width rules as needed for the net class(es) in question in the Design > Rules... editor dialog.

  6. You can select all tracks of a given net class by using the View > Panels > PCB panel. Change the drop-down menu to Nets and select the desired net class from the Net Classes list.

  7. Once selected, you can "retrace" the tracks so they adopt the thickness you've assigned by selecting Route > Retrace selected...*. Caution: this can lead to unwanted results if you have a lot of complex rules and rooms, etc. Just as one should not rely on auto-routing, one should not rely on automatic retracing. But it can be useful.

  8. To address clearance gaps, you can "gloss" the tracks which will adjust gaps and positioning by having Altium attempt to optimize the tracks (what they call glossing) by selecting Route > Gloss selected...*. Again, this can really trash your design, so be prepared to undo! Like retrace, it can be helpful especially if you're just modifying one or two tracks at a time.

There's no substitute for giving each part of your design individual attention, but these tools can be handy depending on what stage of the design you are in. Hopefully you find one or more of the steps above helpful.

\$\endgroup\$
2
  • \$\begingroup\$ Thank you! The filtered highlighted all the net objects but it does not allow me to change the parameters all at once. \$\endgroup\$
    – yolt
    Jun 5, 2022 at 21:53
  • \$\begingroup\$ @yolt When you run the "find similar objects" command, ensure at the bottom left of the dialog that you have "select matching" checked. It may be that you just had "mask matching" checked. As long as objects with shared properties are selected, you should be able to edit them en masse. \$\endgroup\$
    – JYelton
    Jun 6, 2022 at 15:47

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.