Altium unexpectedly soldermask covers random copper region in pcb editor

[king.oslo]

Hello there,

I specified that some of my footprints use regions with solder mask expansion for odd-shaped pad.

But somehow a few of these copper regions appear to have been covered by solder mask both in the 3d viewer and resulting gerber. This is against my will, so I need to discover how to reverse the process.

I searched google and the forum, but couldn't find relevant information.

What should I check?

Thank you for your time.

Kind regards,
Marius

[king.oslo]

Hello world,

It seems the affected regions changes from one time to another. Today, these regions were affected. See the attachment.

Are anyone able to suggest things which I may check to overcome this serious problem?

Thank you for your time.

Kind regards,
Marius

[free_electron]

how did you define this ? did you draw this as an opening in the component footprint library, or is it create by rule ?
if created by rule : check the order of the rules... there may be a conflict. for example : soldermask sliver less than x is not allowed ... then altium would clip the offending region

[king.oslo]

how did you define this ? did you draw this as an opening in the component footprint library, or is it create by rule ?
if created by rule : check the order of the rules... there may be a conflict. for example : soldermask sliver less than x is not allowed ... then altium would clip the offending region

Hello,

Thank you so much for your reply. The solder mask expansion is set manually to 4mil in the footprint lib. Soldermask silver less than 0mil did not solve the problem. I notice that Rule violations are often marked by the software. The errors in question are not marked. It looks like this somehow defaults randomly to most regions on the board. Hmm, any other options which are relevant for regions?

Can you think of anything else?

Thank you for your help.

Kind regards,
Marius

[free_electron]

care to email me the pcbdoc ? that way i can take a look at what is going on

[king.oslo]

Thanks so much. Where should I mail it to?

Thanks M

[free_electron]

my email is in my profile

[king.oslo]

my email is in my profile

I sent you a PM. Thanks.M

[free_electron]

The letter O and N in the logo had expansion set to manual an 0.1mm applied. all other polyregions were set to AUTO with zero applied -> fixed

The solder expansion for the AMP connectors was not defined . I unlocked the polyregion and applied a manual override of 0.1mm

On the thermal pads for U1 U2 and Q1 i altered the paste mask to have a lattice. For QFN packages the paste spread on the central pad should be between 65% and 80% max otherwise the part will 'float' on a blob of liquid solder and you run the risk of solder failures at the edge contacts. Normally the PCB assembly house will inject such lattices in the stencils, but sometimes they forget ...

I painted the thermal via's shut on U1 and U2. you do NOt want the solder to disappear in the via ... painting the vias shut with soldermask on the backside creates a trapped cavity so minimal solder wicking will occur.

You have a PM where you can grab the files and a screenshot before and after the fixes

[king.oslo]

Dear free_electron,

I am sorry to let you know that it seems to me that the problem is not fixed. If you open the file with your changes, you will see that the solder mask expansion has vanished (at least it does on my computer). It seems the information doesn't "stick" when the file has been written to.

If you open the file yourself, I think you will find that the changes you made to the solder mask expansion are gone.

What do you think is going on?M

[king.oslo]

I solved the problem, I think. This is a bug in my version of Altium designer. Users facing the issue can update to 10.890.23450. You can read about it the software bug "5863 An issue whereby the solder mask expansion and paste mask expansion properties for regions were incorrectly loaded from PcbDoc files has been resolved."

Where? Here:

http://wiki.altium.com/pages/viewpage.action?pageId=34210039

I hope this is helpful to someone else.

Kind regards,
Marius