I’m having trouble with copper pours. As seen in the image below, the MOSFET’s drain pad is electrically linked to the net SB but the fill won’t cover that pad. Why? The MOSFET has a SuperSO8 footprint. I downloaded the symbol and the footprint from SnapEDA. I’ve attached the footprints, library symbols, and the project archive here. Any help would be appreciated!
DC-Motor-Driver-revA.zip (67.5 KB) SuperSO8.kicad_mod (4.6 KB) SuperSO8.lib (1.3 KB)
The big pad has an “inverting” bar over it which means it has a different net name (starting with a tilde) and therefore it is a different net.
Thats actually not an inverting bar. The pad number is “5_8”.
Yep, but the net names are “SB” and “~SB”
Ah, Duh, now I see.
My mistake.
The problem is in the footprint of the MOSfets.
KiCad can not draw copper to the pads, because it has to stay clear of the polygons that are drawn on the copper layer.
In the screenshot below I moved the pad (after renumbering from “5_8” to “5”, but that was not the problem) to see what else is in that location.
Also:
You have “Fabrication Attibutes” set to “Through hole” for your MOSfets.
I don’t precisely know what it does, but it feels wrong for an SMT component.
This attribute will cause problem when he tries to export his position file, as normally only the SMD parts listed in the position file.
@paulvdh You are right! I changed that to SMD and updated the footprint on the board but that still does not solve the problem 
I still cannot get the fill zone to include that pad. In the footprint, SnapEDA seems to have created a pad called 5_8 for pins 5 to 8 and this correlates to the pins on the symbol. Also they’ve unchecked the mask and paste checkboxes on the pad and then created separate polygons on the mask and paste layers.
@der.ule Yes that would cause problems when exporting the fabrication and pnp position files.
I took a closer look at the footprint and there seems to be a copper layer not connected to any net. Its the same size as the pad. I removed that and now the pour encompasses the whole pad.
I think you got distracted by the second issue (Fabrication Attributes) and did not spend enough brainpower on the first issue.
You have to remove the polygons from the footprint before KiCad can use it “normally”, or at least remove those polygons from the copper layer to another layer.
For your items on the Mask and Paste layers. To keep it simple you can just enable those layers for the existing pad.
On you Snapeda footprint I see there are 4 pads which are probably meant for the paste layer, (with a bit of separation in between). In KiCad this is handled differently. I think Paste only pads are normally drawn from a pad without a pad number. But I’m not sure, so look this up if you want to go this way.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
