Solder mask missing on only one chip for seemingly no reason

[GadgetWusky]

I used SnapMagic to place a chip in this design. The chip's original pattern had already provided thermal vias in the heating tab pad. These holes in the original pattern supplied with the chip had so many non-removeable DRC errors that I had to change the original pattern with the matching pattern from the DipTrace pattern library (this pattern is SON11P50_300X300X100L55X25TM_API), which has no pre-provided thermal vias in the heating tab pad.

Now that I'm done with the board and I'm looking at the 3D model, I notice that the chip has no openings in the solder mask (fig 1), which is not the first time I have seen this bug. We can see that the chip has the solder paste applied (only to the pins but not the tab for some reason), but not the solder mask. Notice how the other components nearby are not missing the solder mask (fig 2). In the pattern editor, I open the exact footprint I used and it is not missing the solder mask.

Why would the solder mask be missing on the layout editor, and how do I make it include the solder mask?

[GadgetWusky]

I do not understand why this board will not accept all the information for this pattern. I've copied it and tried replacing the part with a copied one that does have the solder mask, I've updated from library, I created a new library with only this pattern and the PCB editor will not accept the mask or heat tab paste, why is the editor removing this information? I don't understand. Literally it is removing information that is present in the pattern. Is there a setting to ignore solder mask on a per-component basis that is turned on by default for this pattern only? This does not make sense at all

[Serg]

I do not understand why this board will not accept all the information for this pattern. I've copied it and tried replacing the part with a copied one that does have the solder mask, I've updated from library, I created a new library with only this pattern and the PCB editor will not accept the mask or heat tab paste, why is the editor removing this information? I don't understand. Literally it is removing information that is present in the pattern. Is there a setting to ignore solder mask on a per-component basis that is turned on by default for this pattern only? This does not make sense at all

It looks like the default Solder Mask settings are applied to the new footprint you’ve added. Try right-clicking each pad, opening the context menu → Mask/Paste Settings, and adjusting the Solder Mask settings.

Screenshot.png (34.51 KiB) Viewed 3703 times

[GadgetWusky]

I do not understand why this board will not accept all the information for this pattern. I've copied it and tried replacing the part with a copied one that does have the solder mask, I've updated from library, I created a new library with only this pattern and the PCB editor will not accept the mask or heat tab paste, why is the editor removing this information? I don't understand. Literally it is removing information that is present in the pattern. Is there a setting to ignore solder mask on a per-component basis that is turned on by default for this pattern only? This does not make sense at all

It looks like the default Solder Mask settings are applied to the new footprint you’ve added. Try right-clicking each pad, opening the context menu → Mask/Paste Settings, and adjusting the Solder Mask settings.
Screenshot.png

I opened the Mask / Paste settings (I did not know that existed in the board editor) and the pins' top and bottom solder mask are set to "tented" and the tab's top and bottom mask are set to "tented" and the tab's top and bottom paste are set to "no solder."

Is this something that could have been done by me in a couple accidental keystrokes? I can't imagine why it would be set like this right out of the Diptrace standard library. I have no memory at all of changing it (I didn't even know this was a setting). How could it be like this?

Thank you for your answer.

[Serg]

If you replace a component’s pattern in the schematic and then update the PCB from the schematic, the paste and mask settings of that component on the board will not be updated. The logic is designed this way so that updating from the schematic does not overwrite the existing paste and mask settings in PCB Layout. So you need to replace the package in the Component Editor → delete the component in the schematic and place a new one → then update the board from the schematic.

[GadgetWusky]

Thanks for the info.