How and where to connect an EPAD pin in Kicad6

[newtekuser]

As I understand an EPAD (exposed PAD) is a thermal area used for heat-sinking an IC. My DRV8825 IC has one, but I don't know how it needs to be connected. By default, the footprint I got from UltraLibrarian designates the EPAD pin as "unspecified".
I'd like to connect it to the ground plane (bottom layer) using VIAs:
In eschema I tried leaving this pin unconnected, then dropped a few dozen vias on it in PCB layout. Not sure if that's the way to go. If I connect this pin to GND in schema I get all sort of errors in DRC.

Either way I also get these mysterious errors in PCB layout DRC (attached) about clearances within the pad itself. Don't know what it wants from me. Any ideas?

[JoeyG]

This is a common question to many  silicon manufacturers.

You are best to ask the manufacturer

Many data sheets have no electrical connection and some ( not all)  say connect to Vss.

Hence to be 100% sure contact the manufacturer.

[selcuk]

PPAD is connected to the ground in the datasheet. If you have this pin (29) on the schematic symbol, connect it to the ground. Then connect it to ground in the layout as well. You may consider it as a regular ground pin.

I don't have that footprint, but I've attached a sample footprint having a center pad.

[newtekuser]

PPAD is connected to the ground in the datasheet. If you have this pin (29) on the schematic symbol, connect it to the ground. Then connect it to ground in the layout as well. You may consider it as a regular ground pin.

I don't have that footprint, but I've attached a sample footprint having a center pad.

Done, dropped a few VIAs on it to GND. About the DRC error in my original screenshot, is it safe to ignore?

[selcuk]

No need to ignore it. I think there is a pad somewhere in the picture not numbered as 29. Make sure all active pads in that area (smd or through hole) have the number 29. When you connect the pin to gnd in the schematic, all of them will be grounded in the layout. You won't get DRC error in that way.

[newtekuser]

No need to ignore it. I think there is a pad somewhere in the picture not numbered as 29. Make sure all active pads in that area (smd or through hole) have the number 29. When you connect the pin to gnd in the schematic, all of them will be grounded in the layout. You won't get DRC error in that way.

I have already connected the pin to GND in the schematic, but DRC error is not about an unconnected pin, it's about clearance violation.

[SiliconWizard]

But it gives you a clearance violation *because* the pad is unconnected (and I'm guessing the clearance is with a nearby pad that is connected to GND? hopefully), as shown with the "x" symbol.
You need to get this pad connected to GND (if it has to be).

[newtekuser]

But it gives you a clearance violation *because* the pad is unconnected (and I'm guessing the clearance is with a nearby pad that is connected to GND? hopefully), as shown with the "x" symbol.
You need to get this pad connected to GND (if it has to be).

That "x" was from the earlier version where the EPAD was not connected to anything. I since had it connected to GND using several vias as in the new screenshot. Am I not connecting it correctly?
I get the DRC error even if I only drop one single via onto the pad.

[selcuk]

Can you clear the previous DRC markers, rerun DRC and paste the result here? In the previous error, one of the conflicting items is a polygon. It may be still there. Vias and the pad seems like they are in the GND net.

[SiliconWizard]

Yes, we need more details for the new violation. I'd say the footprint is still ill-formed (as per KiCad's rules anyway), could you post a screenshot of the footprint in the footprint editor?

[newtekuser]

Thanks for suggesting to open the footprint editor! Looks like the culprit are the two pesky pads circled in yellow. If I remove them and re-run the DRC, the errors are gone.

[SiliconWizard]

I guess these shapes were suggested in the datasheet, or something.
This issue in KiCad footprints is relatively common - usually comes from an incomplete knowledge of how to make pads with "complex" shapes, or possible old footprints that were made when KiCad was less strict with its DRC.

To solve the issue, you need to do the following:
- Right click on the main pad and select the "Edit pad as graphic shapes" menu;
- The editor then goes into this special pad edit mode - you'll note that all pads and copper shapes are visible, and the rest is dimmed;
- Select the central pad and the two extra shapes;
- Right click and select "Finish pad edit".

If all went well, the 3 shapes should be merged into one single pad.

[newtekuser]

I guess these shapes were suggested in the datasheet, or something.
This issue in KiCad footprints is relatively common - usually comes from an incomplete knowledge of how to make pads with "complex" shapes, or possible old footprints that were made when KiCad was less strict with its DRC.

To solve the issue, you need to do the following:
- Right click on the main pad and select the "Edit pad as graphic shapes" menu;
- The editor then goes into this special pad edit mode - you'll note that all pads and copper shapes are visible, and the rest is dimmed;
- Select the central pad and the two extra shapes;
- Right click and select "Finish pad edit".

If all went well, the 3 shapes should be merged into one single pad.

Is this in Kicad6? I do not have this option. I'm using version 6.0.11.

[julian1]

In 6.0.11, there's a default  0.65mm pitch, tssop-28 with centre-pad. Might be an alternative to check, against the DRV8825 datasheet.

TSSOP-28-1EP_4.4x9.7mm_P0.65mm.kicad_mod

[newtekuser]

In 6.0.11, there's a default  0.65mm pitch, tssop-28 with centre-pad. Might be an alternative to check, against the DRV8825 datasheet.

TSSOP-28-1EP_4.4x9.7mm_P0.65mm.kicad_mod

Thanks! Unfortunately, with this footprint I get more clearance violation errors in the DRC.

[Doctorandus_P]

Thanks! Unfortunately, with this footprint I get more clearance violation errors in the DRC.

Yes, of course you have DRC violations. The tracks leaving pads are overlapping with the clearance area of adjacent pads.

To fix it you have to drag the tracks around a bit to get them out of the clearance area.
Maybe you have to check / fix the settings of the interactive router too, because normally KiCad won't let tracks enter the clearance zone of other nets in the first place.

[SiliconWizard]

I guess these shapes were suggested in the datasheet, or something.
This issue in KiCad footprints is relatively common - usually comes from an incomplete knowledge of how to make pads with "complex" shapes, or possible old footprints that were made when KiCad was less strict with its DRC.

To solve the issue, you need to do the following:
- Right click on the main pad and select the "Edit pad as graphic shapes" menu;
- The editor then goes into this special pad edit mode - you'll note that all pads and copper shapes are visible, and the rest is dimmed;
- Select the central pad and the two extra shapes;
- Right click and select "Finish pad edit".

If all went well, the 3 shapes should be merged into one single pad.

Is this in Kicad6? I do not have this option. I'm using version 6.0.11.

In KiCad 6, there is the "Edit pad as graphic shapes". It's in the context menu as well. Alternatively it's accessible with CTRL+E.
The context menu shown in the above screenshot is not that of the footprint editor, it looks as though you were in the PCB editor. You need to open the footprint in the footprint editor, and you'll see this option in the context menu when you right click on a pad.

Note that when you're done modifying a footprint in the footprint editor and saved it, you'll need to update the corresponding footprint in the PCB editor (right click/update footprint). Otherwise you'll still have the old version of the footprint in your layout.

[newtekuser]

I guess these shapes were suggested in the datasheet, or something.
This issue in KiCad footprints is relatively common - usually comes from an incomplete knowledge of how to make pads with "complex" shapes, or possible old footprints that were made when KiCad was less strict with its DRC.

To solve the issue, you need to do the following:
- Right click on the main pad and select the "Edit pad as graphic shapes" menu;
- The editor then goes into this special pad edit mode - you'll note that all pads and copper shapes are visible, and the rest is dimmed;
- Select the central pad and the two extra shapes;
- Right click and select "Finish pad edit".

If all went well, the 3 shapes should be merged into one single pad.

Is this in Kicad6? I do not have this option. I'm using version 6.0.11.

In KiCad 6, there is the "Edit pad as graphic shapes". It's in the context menu as well. Alternatively it's accessible with CTRL+E.
The context menu shown in the above screenshot is not that of the footprint editor, it looks as though you were in the PCB editor. You need to open the footprint in the footprint editor, and you'll see this option in the context menu when you right click on a pad.

Note that when you're done modifying a footprint in the footprint editor and saved it, you'll need to update the corresponding footprint in the PCB editor (right click/update footprint). Otherwise you'll still have the old version of the footprint in your layout.

Found it, thank you! However, even after doing the above and selecting update footprint, I'm back to square 1 and DRC errors are still there.
The only way I can seem to get rid of those errors is if I remove the shapes and NOT click on update footprint. If I update the footprint it looks like Kicad restores it from how it was before the edit.

[SiliconWizard]

I bet you used "open in footprint editor" from the PCB editor... in which case, it will only modify the footprint in the current layout, and not in the footprint library. So when you select "update footprint", it reverts back to what's in the library, as this is what "update footprint" does - update the current footprint with the one in the library. (Which is technically an "update" only if the footprint has been modified in the library itself.)

What I suggested is to modify the footprint in the footprint editor, but you'll need to open it in the footprint editor directly, and not from the PCB editor. If you do that and save your changes, then "update footprint" will work.
The reason I suggested this workflow is so that next time you use the same footprint in another design, you'll have the modified footprint in the library.

[newtekuser]

I bet you used "open in footprint editor" from the PCB editor... in which case, it will only modify the footprint in the current layout, and not in the footprint library. So when you select "update footprint", it reverts back to what's in the library, as this is what "update footprint" does - update the current footprint with the one in the library. (Which is technically an "update" only if the footprint has been modified in the library itself.)

What I suggested is to modify the footprint in the footprint editor, but you'll need to open it in the footprint editor directly, and not from the PCB editor. If you do that and save your changes, then "update footprint" will work.
The reason I suggested this workflow is so that next time you use the same footprint in another design, you'll have the modified footprint in the library.

Indeed, found it! However, I did the same, saved it then updated the footprint in the PCB editor and it's still back to how it was before.
Actually, even in the footprint editor, if I search for the footprint again after editing it I can still see the two square shapes are not merged with the main pad 

Really appreciate the patience!

[selcuk]

What is the DRC error after editing the shape? Are there any polygons (not pads) in the area? If there are, can you remove the polygons and create them as pads and assign them number 29?