Actions
Forum Thread Details
  • Replies 1129 replies
  • Subscribers 245 subscribers
  • Views 51283 views
  • Users 0 members are here
Related

Have a question about CadSoft EAGLE?  Ask our Expert, Richard! (Archive)

nlarson

This thread is now locked - but you can still ask Richard by posting your questions here.  If you'd rather browse other member's questions you can read the CadSoft EAGLE Forums for past questions and answers. Enjoy!

 

Browse past Q&A help on anything technical relating to CadSoft EAGLE!


image

 

Richard Hammerl

Richard is an engineer with 16 years experience in EAGLE customer support and is waiting for your questions.

Parents
  • Dear Richard,
    I am using a professional EAGLE 5.11.0.
    I have created a component made of 100 connections.
    The package is a series of 4 alignments of pads drilled at 0.66mm and spaced of 1.27mm pitch.
    In the library package editor, while using a grid resolution of 0.01mm, we can see that the distance free of copper in between two pads is 0.22mm which is perfect regarding the PCB manufacturing precision.
    We are very surprised to see on the board layout generated from the schematic using this component that the actual distance free of copper in between two pads has dramatically reduced to 0.11mm which is far too tight.
    We have discovered this discrepancy with the DRC.
    Can you please explain how to correct this issue, may be a setting somewhere?
    Best regards,
Reply
  • Dear Richard,
    I am using a professional EAGLE 5.11.0.
    I have created a component made of 100 connections.
    The package is a series of 4 alignments of pads drilled at 0.66mm and spaced of 1.27mm pitch.
    In the library package editor, while using a grid resolution of 0.01mm, we can see that the distance free of copper in between two pads is 0.22mm which is perfect regarding the PCB manufacturing precision.
    We are very surprised to see on the board layout generated from the schematic using this component that the actual distance free of copper in between two pads has dramatically reduced to 0.11mm which is far too tight.
    We have discovered this discrepancy with the DRC.
    Can you please explain how to correct this issue, may be a setting somewhere?
    Best regards,
Children
  • in reply to e14 Contributor

    Hi Sylvain,

     

    It's important to take into account the impact of the Restring tab in the DRC. In EAGLE, the drill size is immutable and will not be changed from whatever value you set. The actual diameter of the pad is a little more flexible and is subject to the restring settings. Basically EAGLE always enforces the minimum restring, if the size you setup in the library for the pad diamter is less than the restring then the restring wins.

     

    All you have to do is lower the minimum restring value until library diameters you set take over.

     

    hth,

    Jorge

  • in reply to e14 Contributor

       I think, by default "EAGLE" assume large copper ring around holes in pads and vias.

    Setting to check (I use EAGLE 4.16r2, hopefully difference is not dramatical) :

       Command   "DRC",  open "Restling", set both "Min" and "Max" equal 7 mils (<=0.2mm) for "Pads" and "Vias", set "%"  = 0.  "Apply".

    If it works, set values more siutable for your PCB.

           Best regards,

                Lev.