Re: [PEDA] Gerber clearance violations not found by Protel DRC
I have had this very problem when I had metric and inch mixed and the gerbers were done in 2.3 format, I then changed to 2.4 or 2.5 and the same file produced usaeble gerbers. So now whenever I have something with primitives smaller than 10 and 10 I use 2.4 or 2.5 format. Roundup error will kill you when your at clearances of 5 mils. Rob * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Gerber clearance violations not found by Protel DRC
Good to here that your issue is solved Ken. Yeah you have to watch that Gerber round off with 2.3 data format these days. It is becoming more and more of an issue with smaller parts, tracks and off-grid routing. Many years ago I ran into this for the first time, since then I adapted the standard rule of using 2.4 data, someday possibly I will see the need for 2.5 data on soft PCBs before I retire. Brad Velander, Lead PCB Designer, Norsat International Inc., #300 - 4401 Still Creek Dr., Burnaby, B.C., V5C 6G9. Tel. (604) 292-9089 direct Fax (604) 292-9010 website www.norsat.com -Original Message- From: Ken Pelic [mailto:[EMAIL PROTECTED]] Sent: Wednesday, September 05, 2001 1:22 PM To: Protel EDA Forum Subject: Re: [PEDA] Gerber clearance violations not found by Protel DRC We re-generated using 2.4 format and our gerbers now match our Protel PCB. Thanks to all for your feedback, especially to Rob and Brad V! Ken Pelic * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Gerber clearance violations not found by Protel DRC
At 05:14 PM 9/4/01 -0500, Jon Elson wrote: Don't use measure primitives, use Report Measure Distance. You may have to set the snap grid to a small value, like .01 mil while you are doing the measuring. Reports/Measure Distance is not particularly good at accurately measuring the distance between two primitives because one must visually attempt to locate the edges of the primitives. If it falls on the snap grid, fine, but otherwise Reports/Measure Primitives directly measures the gap between any two primitives. It seems to be quite accurate. Yes, if you are going to use Reports/Measure Distance, you may need to be on a fine grid. Abd ul-Rahman Lomax LOMAX DESIGN ASSOCIATES PCB design, consulting, and training Protel EDA license resales Easthampton, Massachusetts, USA (413) 282-0013, efax (419) 730-4777 [EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * http://www.techservinc.com/protelusers/leave.html * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/proteledaforum@techservinc.com * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *