Minimum Gang Solder Mask Web
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=3344
Printed Date: 06 Oct 2024 at 10:20am
Topic: Minimum Gang Solder Mask Web
Posted By: yvoren1
Subject: Minimum Gang Solder Mask Web
Date Posted: 19 Dec 2023 at 1:17pm
|
Hi, I’d like to understand how work Minimum Gang Solder
Mask Web in SMD Pad Stack Rules I have these specifications in Component Data
If I use 0.10 mm for the Minimum Gang Solder web mask, I get a 0.83 x 0.40 mm mask, so the web mask = 0.10 mm that is correct
If I use 0.10 mm for the Minimum Gang Solder web mask, I get a 0.83 x 0.50 mm mask, hence the web mask. I don't understand why the mask becomes 0.40 mm to 0.50 mm. I expected the mask to stay at 0.40 mm for a 0.10 mm web
|
Replies:
Posted By: Tom H
Date Posted: 19 Dec 2023 at 4:35pm
|
Are you wondering why the
solder mask excess isn’t limited to prevent a sliver instead of increased to
fill the sliver? ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: yvoren1
Date Posted: 20 Dec 2023 at 6:43am
| Yes, that’s what I would like to know! |
Posted By: Tom H
Date Posted: 20 Dec 2023 at 9:57am
|
First, setting the solder mask web to 0.10 is overkill. Fabrication shops can easily produce a 0.07 solder mask sliver. Where the Fabrication industry needs is a 0.05 mm solder mask swell and a 0.05 solder mask web. This will ensure a solder mask sliver between every SMD pad stack and eliminate Gang Masking of entire rows of pads. Ask your fabrication shop how accurate is their solder mask application process. ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: yvoren1
Date Posted: 20 Dec 2023 at 10:04am
|
OK , Some of my fab shop don't want to go under 0.1mm , but now i know how far i can go Thank you Tom!
|
Posted By: Tom H
Date Posted: 20 Dec 2023 at 10:12am
|
There is something you need to know. If your fabrication shop requires a 0.10 mm solder mask sliver, if you don't Gang Mask the row of pads in your PCB library, your fabrication shop will run a check on your Gerber data to find every pad that has a sliver less than 0.10 mm and they will gang mask the row of pads without even asking you. So either you provide the correct data or they will correct your data. ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: bab27
Date Posted: 03 Sep 2024 at 5:58am
|
I'm looking for an IPC for these kinds of specification. IPC-7352 Page 34, there is an example with 0.50 mm Pitch SOP with 0.05 mm Solder Mask from copper and 0.075 mm from Solder Mask to Legend (silkscreen). Do you know if there is more information according to the fabrication level, A, B or C about that? |
Posted By: Tom H
Date Posted: 03 Sep 2024 at 8:15am
|
I provided IPC-7352 with the silkscreen and solder mask illustration on page 34. As PCB designers we all create prototype boards that require silkscreen for small batches. We recommend a silkscreen line width between 0.12 mm minimum, 0.15 mm nominal and 0.20 mm maximum. IPC has no rules or guidelines on solder mask. The current range for solder mask annular ring in the electronics industry (from component manufacturers recommendations) is between 0.05 mm minimum, 0.07 mm nominal and 0.10 mm maximum. The gap between the silkscreen and solder mask would be the tolerance of the application of both, which is 0.07 total. You don't want any silkscreen encroaching in the solder mask removal area. If there is silkscreen in the solder mask removal area, the fabrication shop will automatically trim it off for you. ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: bab27
Date Posted: 11 Sep 2024 at 7:40am
| Thank you very much for your reply. |