Solder Masks
Printed From: PCB Libraries Forum
Category: PCB Footprint Expert
Forum Name: Questions & Answers
Forum Description: issues and technical support
URL: https://www.PCBLibraries.com/forum/forum_posts.asp?TID=1380
Printed Date: 07 Nov 2024 at 5:47pm
Topic: Solder Masks
Posted By: Todd Manning
Subject: Solder Masks
Date Posted: 27 Jul 2014 at 10:50pm
|
Hello, I'm having trouble trying to work out how the parameter "Minimum Gang Solder Mask Web" works under the "Rules" tab. I have it set to 0.08mm and am assuming this is the minimum width of the solder mask sliver between pads. When I build my part, which in this case is a QFP50P1200X1200X160-64 and then import it into Altium my solder mask sliver between pads is 0.06mm??? Can anyone please tell me if I'm understanding this rule correctly and if so, how do I get it to work correctly. Thanks Todd |
Replies:
Posted By: Tom H
Date Posted: 28 Jul 2014 at 8:00am
|
Altium globally produces its own solder mask by design rules and Altium does not support true "Pad Stacks". You cannot control individual solder mask on pads except to use copper on the solder mask layer. Your fabrication shop will do the gang mask for you if they find any slivers less than their manufacturing tolerances. ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: Todd Manning
Date Posted: 28 Jul 2014 at 5:30pm
|
Hi Tom, Thanks for you reply. I've attached an image of the property box for a pad in Altium. In the bottom-right there is the option to manually overwrite the global solder mask expansion setting and then specify a custom expansion value. Are you somehow able to ulitise this feature to automatically generate the correct minimum sliver width?  Regards Todd |
Posted By: Tom H
Date Posted: 28 Jul 2014 at 6:01pm
|
Todd, I have never been concerned with Solder Mask Web Slivers. Most fabrication shops use Valor Genesis as the front end CAM tool and it rules DRC rule checks for everything you can think of. Every manufacturer has a minimum solder mask to solder mask clearance. The norm is 3 mils or 0.08 mm web width is doable and anything below that web thickness is not. I leave this up to the fabrication shop. I've worked as a volunteer for IPC for the past 15 years and every time the subject of Solder Mask Swell comes up the response is always "Solder Mask should be 1:1 scale of the pad size and allow the fabrication shop to swell (oversize) the mask per their manufacturing tolerance. Altium is slightly different as they DRC check Silkscreen to Solder Mask so you tend to try and swell the solder mask in the CAD tool and then run DRC checks to find violations. But I agree with IPC and that Solder Mask Swell and Gang Masking is the fabrication CAM operator's job and not the PCB designer's. They know what they can manufacture, they use tools that cost 10 times Altium list price and they have the experience with their equipment. But if you insist, in Altium (and other PCB design tools), the only way I know how to Gang Mask is to add copper on the solder mask layer. ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: Todd Manning
Date Posted: 28 Jul 2014 at 6:20pm
|
Hi Tom, I have always liked the idea, that what information I supply the manufacturer is exactly what they will produce giving me 100% control over the design, so therfore have always incorporated solder mask swell in my design. I understand your point as well, as it would allow you to change manufacturers without the worry of whether or not they could produce to my specified tolerances. I think at this stage I will continue with the way I do things as it has worked without issues up to now and manually edit the solder mask swell after I import the parts into Altium. Thanks for your input. Regards Todd |
Posted By: Tom H
Date Posted: 28 Jul 2014 at 6:41pm
|
Todd, Every manufacturer will modify your Gerber data to match their manufacturing tolerances to insure that the delivered boards match your fabrication notes. They will swell your outer layer pads, traces and vias to compensate for their etching process. They will trim all silkscreen that violates solder mask overlap. They will swell through-hole annular rings to meet IPC minimum annular ring to compensate for their drill machine accuracy and drill drift. The fabrication shop will always manipulate your Gerber data to increase yield and reduce scrap. ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: Todd Manning
Date Posted: 28 Jul 2014 at 7:53pm
|
Hi Tom, Thanks, I appreciate the extra information. Regards Todd |