Re: [PEDA] Gerber clearance violations not found by Protel DRC

2001-09-05 Thread rlamoreaux



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

2001-09-05 Thread Brad Velander

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

2001-09-04 Thread Abd ul-Rahman Lomax

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
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *