Hi Lum, In Fablink, under Change Artwork Format, set the output format to 4 decimal places rather than the default of 3 (provided your units are inches). 3 decimal places only gives you 0.001 resolution Gerber files so traces routed on a smaller grid or no grid will snap to the nearest 0.001. This can produce 0.005 spacing with 6/6 rules even though you will not see it in Layout. For more Mentor specific info check out the MUG pcb_sig at mentorug.org Regards, Roy Roy H. Beckman, C.E.T. Senior PCB Designer / System Administrator Harris Canada, Inc. 6732 - 8th Street, N.E. Calgary, Alberta, Canada T2E 8M4 Phone: 403-295-4758 Fax: 403-295-4622 email: [log in to unmask] -----Original Message----- From: Lum Wee Mei [mailto:[log in to unmask]] Sent: Tuesday, June 22, 1999 10:35 PM To: [log in to unmask] Subject: [DC] Inconsistent Gerber Output I have a question regarding Gerber output. Most of our designs are done with 6/6 (trace/spacing). One one occassion, our regular PCB vendor called us up and inform us that they found some 5/5 on a particular layout. However, when we call up the layout on our workstation with grid at 1mil setting, we found that the so-called problem area to be a perfect 6/6. Recently, this problem cropped up again with another new PCB vendor. Once again, our layout show a perfect 6/6. Can anyone throw me a light on what could be the problem. My Mentor Graphics rep mentioned that it could due to the CAM system used by our PCB vendor. Thanking in advance. Regards.