@ericbarber, Please study: [https://easyeda.com/forum/topic/How-to-avoid-DRC-errors-when-connecting-to-PCB-Footprints-a-k-a-PCB-Libs-90bf944fe3644b21a7d27a9e9d8df8d6](https://easyeda.com/forum/topic/How-to-avoid-DRC-errors-when-connecting-to-PCB-Footprints-a-k-a-PCB-Libs-90bf944fe3644b21a7d27a9e9d8df8d6)

You may need to use the convert pad to board cutout right click feature to make the through hole cutouts. Please post back if you need more help.

@andyfierman Thank you for your quick reply. I had already read the post that you linked, but made sure to look through it thoroughly again. I did not notice any new information that stuck out to me. In the post you linked: 1. The pads are top layer polygon style 2. Holes without copper (the only thing causing me any grief and the reason for my post) were made as a solid region set as "Board Cutout" 3. Both pads are numbered 4. Does not apply 5. Does not apply 6. I am not passing through any entities nor connecting to these fully enveloped holes.  7. No nets have been assigned 8. Does not apply 9. Does not apply Re: your second post 1. I have not seen the "convert pad to board cutout" right click feature in my usage of the footprint editor. I frequently see "convert to pad" when right clicking on a solid region, but I do not observe any such option for a board cutout when right clicking on a pad. I would like the board cutouts to occur exactly as they're placed in my sample project which I shared in my initial post, to mirror the vendor's recommended pad layout:  As a side note, I also cannot set the radius to 0.40 on these board cutouts, the lowest I am allowed is 0.50. I settled on square cutouts (knowing they will not be perfectly square anyways due to the drill radius).

@ericbarber, If you edit the footprint pads to not go over the slotted holes then it should work. Use the 'Edit points' button to edit the points around the hole... _  _ This removed the DRC error for me. _ Regards.

@MrToM, Thank you for the great suggestion! I am still curious if there is a way to keep the pads as specified in Omega's datasheet? Placing a hole through a pad should not be an issue? I agree completely that removing the pad from around the slots should be fine; I am aiming to create as close of a replica of their datasheet as possible.

@ericbarber, If you can accept round ended slots for the holes then yes, it can be done. _ 1\. Select the pad\. 2\. Change it's layer to 'Multi\-Layer' \(This will give access to the hole properties\) 3\. Set 'Hole shape' to 'Slot'\. 4\. Change the hole dimensions\.\.\.i think I used 1mm dia hole\, 3\.25mm length\.\.\.\.\.ish\. 5\. Click the 'Edit Points' button\. 6\. Move the hole in the 'X' direction \.\.\.\.\.\. 1\.8mm\.\.\.\.\.or something like that\.\.\.\.you'll see it top of the list\. 7\. Once you've edited the slot you need to remove the original rectangular slots\.\.\.\.\.easiest way is to select the pad and 'shift' it \(using your cursor keys 'n' number of times\.\.\.\.until the original hole is exposed\.\.\.\.\.delete the hole and then shift the pad back 'n' times\. I did it this way as to align the new 'slot' with the old\.\.\.\.\.you could just delete them first and go by the numbers from the datasheet\. 8\. Save and update everything and the DRC error should be gone\. _ Regards.

@ericbarber, Sorry, forgot to mention that the above is all done in the footprint editor, I don't think you can do it from within the PCB...? _ Regards.

@MrToM, I performed all of those steps and was excited that it would work out, but when rendering the board in 3D there are pads exposed on the bottom as well when using the above method :(.    I am going to try mapping more points next to go around the hole instead, will update this thread when I have more info. I really appreciate your effort working on this.

I am not especially proud of it but it does seem to work and passes DRC:  (four pads per pad) Looks like this in render: 

@ericbarber, LOL...I didn't think that would meet with your approval, although PTHs would give a stronger mounting. So....in that case, back in the footprint editor, try this... _ 1\. Revert back to the pads being on the 'Top Layer'\. \(Keep the original holes deleted\) 2\. On the 'Board Outline' layer draw your rectangular holes\.\.\. _  _ 3\. Save\, update a gazzillion times\, click the OK button till you're blue in the face and then\, if there is any time left in the week\, swap over to version 6\.4\.7\, open the project\, click the 3D button and\, cross your fingers\. You'll have to use 6.4.7, (locally), as the latest version doesn't show board outline holes properly in the 3D viewer....unless it's just me. _  _ Regards.