Actions
Forum Thread Details
  • Locked Locked
  • Replies 5 replies
  • Subscribers 88 subscribers
  • Views 1951 views
  • Users 0 members are here
Related
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

DRC Rule minimum copper width

mf_ibfeew

Hello,

In the design rules I can define rules for minimum trace width. this works well for standard traces.

But the appended picture shows a problem with a minimum copper width in a special case. The net connects to the pad only with a very small edge, but none of the design-rules catches this event. Neither  the "unrouted" nor the "minimum trackwidth" - rules are complaining at this picture. Is there a rule which marks this picture as failure? How can I avoid such a situation? (the production of this board could easily produce an error at this point, it was pure luck that I catched this glitch)

Nice weekend, Maik Freitag

Attachments:
image

  • Hi,

     

    The rules are similar to the Altium Designer rules for width.  I found them for AD18 as described here: https://www.altium.com/documentation/altium-designer/pcb-dlg-maxminwidthrule-framewidth-ad?version=18.1

     

    Did you try the selection for physical connected copper?  I'm not sure but otherwise I think it only checks the routing meets the expected rules and would not catch what you noted.

    image

     

    Darn, you got me curious and now I'm going to have to try this myself.

  • in reply to tarribred61

    I confirmed that for CS1.5.2 using the width rule with the check box set for physically connected copper that it caught the condition I artificially made for a small connection area. It did this using both batch and on-line DRC.

    Screen shot below shows what I see for detecting a copper connection less than the rule of 10mil.

    image

  • in reply to tarribred61

    Thanks for your effort.

    At  first I have to admit that until now I have overlooked and ignored the 4 checkboxes to the right of the min/max-sketch.

    The "check for physically connected copper" improves the situation and detects at least problems if 2 wires don't overlap properly. (middle of my picture, top half).

    The insufficient connection from wire to pad (bottom of the picture) is still not flagged as an error.

    I have now tried to play with another design (to exclude project-specific failures), but same behavior.image

    rule settings (now with the found physical-copper-switch set):

    image

    Can you upload a picture from your small-connect-test?

    Maik

  • in reply to tarribred61

    thanks for the picture. It has clarified something and after some "play around" I think there are some bugs in the width-calculation for "special cases".

    If I connect the wire like your example (wire straight to the pad) I get an error (like you). (pic1)

    If my wire touches the corner of the pad (45degree wire), I get no error. (pic2)

    If I have a combination of 1+2 (straight wire connection and a 45 degree touch-connection), I also get no error. Also not on the place where pic1 showed an error.

    This situation is not ideal for pcb-check before manufacturing. Hopefully this will be fixed in the soon-to-be-released circuitmaker pro (probably around 2025...2027?).

    So for now I have to accept this restriction.

    image

    image

    image

  • in reply to mf_ibfeew

    I rechecked my example and found that there is a point of contact where the unrouted net length goes to 0 but the DRC does not indicate the rule violation.  If I move the net a little bit to give more contact then the rule shows the violation. 

     

    It is possible that Altium Designer also does this.  I have posted this issue in the CircuitMaker Pro beta forum since it seems to have the same issue.