I have generated a PowerPAD with the size of 3.4mm x 5mm (Standard Pad with 12 plated holes) and only 2.6mm x 2.59mm is not covered by solder mask as proposed by TI. To do this I drawn 2 rectangles of 2.6mm x 2.59mm the first on the TOP Stop Mask layer and the second on the TOP Solder Paste to have the right stencil. So I get the following pattern:
LibrePCB give me the following error:
Invalid Origin of pad ‘15’ in ‘default’
Solder Resist on pad ‘15’ in ‘default’
If I select ThermalPad instead of Standard Pad I get the errors listed before and one warning
List item Suspicious function of pad ‘15’ in ‘default’
Function is intended for THT pads but pad is SMT
Function is intended for SMT pads but pad is THT
Function is electrical but pad is not connected
Function is fiducial but pad is connected
This pad is SMT, so you should place an SMT pad instead of a THT pad. Then disable automatic stop mask and solder paste and draw them manually as polygons. The “solder resist on pad” warning can be approved as you added it manually. You can use the 3D preview (Ctrl+3) to check if all the masks look correct. If you’re unsure, post the screenshot of both 2D and 3D view here.
For the vias currently we don’t have a clear solution. I’d recommend to draw the footprint without them, and add them later in the board. I agree it is not ideal, but this will work fine and the advantage is you are more flexible with their placement (avoid conflicts with traces on other layers by slightly changing their position, since their exact position is not very critical).
If you really want to have the vias in the footprint, you could try to add them as individual THT pads (overlapping with the SMT pad, but assigned to the same net). I never tried it and I don’t know if this causes any problem. Maybe the DRC is happy when you connect one of them, so be careful to really connect all of them. And let me know how it worked if you want to try this way
But I have the Power-PAD also on bottom although I didn’t draw a pad on bottom. My settings on the Power-PAD are as follow:
I have inserted on the PAD 12 Plated Holes. Is for this reason?
For me is OK having also a PAD on the bottom because it helps to dissipate power so I will leave it. But it was only to know in the future if I don’t want a PAD also on the bottom
Yes that’s the effect of adding holes to the pad. It turns an SMT pad into a THT pad and automatically adds bottom copper.
The Gerber look good to me and if you’re fine with the pad on the bottom I think you can take this approach. But generally I’d suggest what I wrote above (make it SMT by removing the holes) to not waste space on the bottom copper layers (and possibly even on inner layers, depending on board settings).
You need to be careful with board settings anyway (“Board Setup” in the board editor). It is possible to configure THT pads to have the full copper area only on solder side, but not on component side. Maybe this could even be useful for your case, but it requires you to set “Component side: Bottom” on the thermal pad. Then I think the bottom copper won’t be filled, just an annular ring around the holes. But this all feels a bit hacky
