Let's get some terminology straight. This is not a bug. It's a missing feature, and is worthy of a feature request. I've made one in the past, but it hasn't been "popular" enough to get attention. Maybe you'll have better luck.
So here's what you do. That soldermask opening you refer to can be defined as the terminal pin of a thermal pad. You also need solder paste for that area. So define a pad of the size of the soldermask opening. You can add soldermask and solder paste definitions to that pad if they're a different size. Check the "Flood Over" option for the thermal connection of this pad. Be sure that pin is also added to the the schematic symbol, so the correct net gets assigned to it, usually ground. On the layout, draw the larger copper pour the size you need it, and you have exactly what you need for a successful design.
David, thank you for explaining your solution, but I'm afraid it doesn't fit my needs. Just to to clearify what I'm trying to achieve:
If I understood you correctly, you are placing GND pour in the layout tool, not in a decal editor? The shape of the GND for the part I'm creating is quite unusual and I cannot let designers to draw it each time they use the part. It is manditory that decal is finished when placed in layout tool.
Can you please advise further?
Thanks for the picture. I was describing a simple rectangle, and this is more complex than what I pictured. But my advice still holds. I just have to add a step or two.
So what you need to do is draw the entire copper shape, and associate it to a surface mount pin. I hope your drawing skills are strong. PADS has capable enough drawing and editing tools, but it takes some practice to get used to them, and this will make you an expert when you're done. If you're doing a lot of RF, you'll be doing this kind of thing a lot. Even better, many of these RF parts are available in DXF, so you could import the pattern if it is.
You'll need to also add the solder paste pattern to the thermal pin, since it does not follow the copper in this case.
The via pattern is another issue. Another shortcoming of PADS is you can't put vias in a decal, and have them associate to a net at the board level. This is another feature request I've asked for to no avail. So these have to be entered as via-sized pins, and also added to the schematic symbol. There are other ways to do this that might work, but what I've described allows PADS' DRC and clearance checking routines to work without false errors.
David, I really appriciate your effort of explaining the procedure to me, but I still can't achive what I want to. First of all, I am a beginner, but I'm learning fast. In past I worked with Altium Designer, so I have to get used to PADS' way of drawing.
I created a thermal pin, that has a small circle on top land, and a desired rectangle on solder mask. I am in doubt if this pin saves a thermal, because even though I change it correctly to "thermal" in pad stack properties window, the next time I open pad stack property, it shows it as a normal "pad". Anyhow, I associated thermal pin to my copper pour. I drew cutouts for every BGA pin, but in CAM preview I still see an uniform rectangle of solder mask.
I am guessing I should edit CAM documents' setting of layers. Can you please provide me your settings for Solder Mask and Solder Paste at which your approach outputs right CAM preview. Thank you!
In case anybody ever needs to create similar footprint, I've managed to do it without thermal pad. I am not saying thermal pad was a bad approach, it just didn't work for me due to my beginner level of PADS.
First thing that is kind of obvious is to combine solder mask shape and sodler mask cutout shape. I wanted to achieve that before, but couldn't select both. I expected that I could use select shape, and then ctrl+right click->select shape, but it didn't work that way. It's actually more simple to just select both by drawing rectangle that touches both shapes. You have to manualy create circle for solder mask on all BGA pins. Also you have to create paste cutout in the shape of solder mask.
Another thing to check is CAM output settings. If you go to solder mask -> edit -> layers -> Top , you have to select "pads" and "advanced selection".
Same for solder paste.
David, thank you for your effort. Big thanks go to Terry from Mentor who showed me how to do this kind of footprint.