Why is Gang Mask shape option removed?
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=3452
Printed Date: 08 Jan 2025 at 11:53am
Topic: Why is Gang Mask shape option removed?
Posted By: ulissescastro
Subject: Why is Gang Mask shape option removed?
Date Posted: 06 Jan 2025 at 11:13am
|
Hi Tom, Could you please elaborate on why the Gang Mask option was removed in the latest version? I also noticed that FPE does not visually show the "block" until it is imported into Altium (in my case). Adding individual "lines" to construct the "block" in the solder mask layer may not be efficient when the user wants to delete it. Could you please create a shape that can be easily removed with a single selection? Best regards, |
Replies:
Posted By: Tom H
Date Posted: 06 Jan 2025 at 11:27am
|
The Gang Mask shape is now determined by the pad shape. Rectangle pad shape will automatically produce a rectangle gang mask. Rounded Rectangle pad shape will automatically produce a rounded rectangle gang mask. Oblong pad shape will automatically produce an oblong gang mask. The V25.02 Footprint Expert gang mask feature has been updated and improved. The gang mask feature will appear in the Footprint Expert viewer.  ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: Tom H
Date Posted: 06 Jan 2025 at 11:33am
Other V25.02 improvements to the Altium interface:
------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: ulissescastro
Date Posted: 06 Jan 2025 at 1:31pm
|
Hi Tom, I'm having some trouble understanding how to disable the Gang feature and control it as needed. The only guidance I found is a comment saying, "set sm grid array options in terminal density settings" in the SMD Pad Stack Rules. I can manage the solder mask web using mask expansions and pad-to-pad settings to ensure the minimum web. However, I want to be able to enable or disable this control. Our assembly house prefers to have a mask between pads to minimize the risk of solder bridging and to allow more width for the stencil apertures. Therefore, I would rather trim the leads, knowing exactly what I'm doing |
Posted By: Tom H
Date Posted: 06 Jan 2025 at 1:59pm
|
Altium has it's own Preferences for solder mask control. Regardless of any setting you establish in Footprint Expert Options, Altium Preferences will overwrite the Footprint Expert settings. The disable the gang mask feature, make your solder mask swell 0.00 (or 1:1 scale of the pad stack). When you import the footprint into Altium, the Altium Preferences will take over. You need to do the math to establish a solder mask sliver between every pad stack. Start with the minimum solder mask sliver size of 0.075. Then add the solder mask swell of 0.05. The minimum pad to pad spacing rule needs to be set for 0.175 for pad trimming. Only the pads for a 0.50 pin pitch will need to be trimmed. ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: ulissescastro
Date Posted: 06 Jan 2025 at 2:31pm
|
I usually don't use the Altium solder mask Rule. in most cases it's useless. I do prefer to define the mask what Altium called "Manual" in my Footprints. I do trust more in FPE than Altium, if the only solution now is to do 1:1 in FPE and then control it in the CAD tool, I do think this is going backwards, you should bring the option back.
What you describe at the end is what I was mentioning defining the pad to pad clearance. My question again is. Where can this feature be turned on or off or what is the value that will trigger FPE to to add the shape or not. is it the trimming of leads in your code preceding the mask feature or is it after? Thanks |
Posted By: Tom H
Date Posted: 06 Jan 2025 at 2:40pm
|
You do not need to do 1:1 scale solder mask if you set the Minimum Pad to Pad Spacing to allow for a solder mask web. What Solder Mask annular swell do you use? 0.05, 0.07 or 0.10? What is your Minimum Solder Mask Web? 0.07, 0.08 0.09 or 0.10? Multiply the Solder Mask annular swell by 2 and add the Minimum Solder Mask Web. Then use that value to set your Minimum Pad to Pad Spacing rule. This will effectively turn off the Gang Mask feature. ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: ulissescastro
Date Posted: 06 Jan 2025 at 3:51pm
|
Hi Tom, it looks to me that the gang feature is added before FPE compute the trimming.. Please try to replicate the following and these are my settings.. uploads/16854/FP.PNG" rel="nofollow - uploads/16854/FP.PNG uploads/16854/FPX.PNG" rel="nofollow - uploads/16854/FPX.PNG uploads/16854/Options.PNG" rel="nofollow - uploads/16854/Options.PNG
|
Posted By: ulissescastro
Date Posted: 06 Jan 2025 at 4:00pm
| Fix it. it looks like the comparison should be >= instead or >... did a test and added 1 mil to the pad to pad and now it trims the leads and with no more gang mask... |
Posted By: Tom H
Date Posted: 06 Jan 2025 at 4:12pm
|
I entered all your dimensions and concluded the same result. Footprint Expert is trimming the pads per the SMD Pad Stack Rules and turns off the Gang Mask feature.  ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: ulissescastro
Date Posted: 06 Jan 2025 at 4:34pm
|
I think the problem is in the resolution and how many decimal points are used, please try to use at least 4 or 5 decimal points in your preferences. I do know is not realistic but please give it a try... Found the Fix, Thanks for helping... by the way thanks for sharing the FED Vol 18 standard, for some reason I did came up to the same conclusions over the time... are you planning to give a quick update and presentation about it? I'm not sure if we can buy it or what its include on it. so a quick summary may help to justify it ;)
|
Posted By: Tom H
Date Posted: 06 Jan 2025 at 4:55pm
|
I was able to reproduce the issue using 4 place calculations. When I use 3 places it works OK. But that's because when 4 places are rounded to 3 places, the rounding is up. Try this - use 4 places and for the Minimum Pad to Pad Spacing use 0.2033. The new FED Vol 18 Nominal Calculation Mode comes with V25.02 Footprint Expert. Switch between Min/Max and Nominal Mode in "Tools > Options > File > Calculation Mode > Min/Max or Nominal". The new feature is located in the "Help > User Guide > Option Settings > Calculation Mode Options".  ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |
Posted By: ulissescastro
Date Posted: 07 Jan 2025 at 4:34pm
| Thanks. All good now... |
Posted By: Tom H
Date Posted: 07 Jan 2025 at 4:41pm
|
More information regarding the Nominal Calculation Mode: https://www.pcblibraries.com/Forum/footprint-expert-nominal-dimension-calculator_topic3450.html?FID=1&PR=3" rel="nofollow - https://www.pcblibraries.com/Forum/footprint-expert-nominal-dimension-calculator_topic3450.html?FID=1&PR=3 ------------- Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn |