Actions
Forum Thread Details
  • State Suggested Answer
  • Locked Locked
  • Replies 7 replies
  • Answers 1 answer
  • Subscribers 89 subscribers
  • Views 937 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

Clearance Constraint Errors on Eagle Import

emerlily

Hi,

 

I've imported a project from Eagle into CircuitStudio that had no DRC errors in Eagle (same generic clearance rules of 5mil), but in CircuitStudio I have literally thousands of clearance constraint errors. They mostly seem to be associated with through hole components and any traces connected to them. When I try redrawing the traces the errors persist and decreasing the clearance constraints doesn't help either. Has anyone else seen anything like this?

  • 0

    Here's one pad with multiple clearance constraint errors for seemingly no reason.

    image

    I also tried drawing a new project with the library I had imported from Eagle and got the same clearance constraint errors!

    image

  • 0 in reply to emerlily

    Hi Emily,

    That first image looks to me like a component clearance problem - if you were to zoom out you might see that the component outline interferes with an adjacent component, or is closer than the design rules allow (presumably the default CS rules will be applied; I don't think these will be imported from Eagle.  Depending on your configuration, CS may do a 'quick and dirty' online check using a bounding rectangle, but a more detailed check using the 3D shape when you perform a manual Design Rule Check.

     

    In the second image, are the tracks are part of the library part?  If so they won't automatically pick up the net name of the pads to which they make contact.  There may be a way to automate this but I don't know it.

     

    I hope that helps a little.

  • 0 in reply to frog

    Another thing to consider is that there may be some rounding errors when importing (I don't know what distance units Eagle or CS use internally).  If a nominal 5mil were to round to 4.999 then it would generate a violation even though for practical purposes it's ok.  For this reason I often set the design rules to be slightly less restrictive, e.g. 4.9mil rather than 5mil, so small rounding errors won't flag a violation.

  • 0 in reply to frog

    Another thing to check for after importing are duplicate design rules.

  • 0 in reply to e14softwareuk

    So design rules are imported form Eagle?

  • 0 in reply to frog

    Not certain but just thought something worth checking for in case you had unexpected rules in action causing the conflicts.

  • 0 in reply to e14softwareuk

    It looks like the DRC rules were imported from Eagle with the project and it created some funny ones relating to polygon classes (these didn't exist in Eagle) and one duplicate. When I deleted all of the DRC rules and put the default ones in it fixed *most* of the errors. Another thing to look out for is the solder mask on through hole footprints somehow expanding when imported, a bunch of my test points were causing short circuit constraint errors (CircuitStudio left, Eagle right) you can see in Eagle that the polygon edge touches the Battery trace but the test point itself doesn't. Editing the test points to round from octagonal fixed these errors. Hopefully this helps someone else in the future.

    imageimage