Please see this Bug Report: [https://easyeda.com/forum/topic/Inconsistent-connection-to-pad-on-single-numbered-multi-padded-footprint-40071cd5cf5a478cac7be7d4334a02a1](https://easyeda.com/forum/topic/Inconsistent-connection-to-pad-on-single-numbered-multi-padded-footprint-40071cd5cf5a478cac7be7d4334a02a1)

@andyfierman I disable snap as per that instruction given in the link and it makes no difference whatsoever.

Another option I tried was to create a PCB module (a component just contained the pads and then the routing was added in the module, but that too did not work. However, iI do not understand how PCB modules work exactly as I found them difficult to include in a project if the component is already there from the schematic. Likewise, I found that you could not include a PCB module with a schematic component or... does a pcb module only work when linked with a schematic module. hmmm.

@gerriko.iot, "I disable snap as per that instruction given in the link and it makes no difference whatsoever." Correct. The first reply from support was before they had understood the issue. Don't bother with trying to do this with a PCB module. The problem is getting the track to snap to the right part of the multiple same numbered pad structure. You could try drawing the antenna as a track and then do "Convert to Pad".

If you're using a library PCB Footprint (a.k.a. PCB lib) then it almost certainly won't  conform to the rules described here: [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) so you'll probably have to build your own PCB Lib anyway.

@andyfierman "Convert to pad" sounds like the right option to me. So thanks for the suggestion. I will certainly give that a try.

@gerriko.iot, May still find that the track attachment snap point is in a very unhelpful place.

@andyfierman Thanks for the tip. Just one question about using the "convert to pad" option. Does this not then expose the copper trace. So, how do I ensure that this is not the case.

Yep, that's a fail too. If the bug in routing to the pads described in: [https://easyeda.com/forum/topic/Inconsistent-connection-to-pad-on-single-numbered-multi-padded-footprint-40071cd5cf5a478cac7be7d4334a02a1](https://easyeda.com/forum/topic/Inconsistent-connection-to-pad-on-single-numbered-multi-padded-footprint-40071cd5cf5a478cac7be7d4334a02a1) gets sorted the correct way to create an antenna structure like this is as illustrated in: [https://easyeda.com/andyfierman/how-to-make-a-connectable-antenna](https://easyeda.com/andyfierman/how-to-make-a-connectable-antenna) based on the instructions to make everything in a PCB Lib using only pads in: [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) then that is the way to make an antenna PCB Lib. Then you just have to be aware of the problems that because all the pads on it are the same number, then all the nets connecting to it must have the same net names to avoid DRC errors because - as far as the Design Manager is concerned - the pads is a simple short circuit so everything connecting to it is shorted together. This is also a problem of how to deal with copper floods around it if the flood is on the same net as the antenna (which will often have to be Ground) and this can be dealt with using the techniques described in: [https://easyeda.com/andyfierman/4-wire-sensing-using-the-kelvin-connection](https://easyeda.com/andyfierman/4-wire-sensing-using-the-kelvin-connection) * **But I might have found a reasonable workaround...** Another trick is to make the antenna shape using the Track tool and then select the track and do "**Convert to Board Cutout**" and then select the shape and set the converted Cutout to **Type = Solid**. This creates a single solid region of copper in the required shape of the antenna. **This works if the Solid Region is created directly in the PCB using the PCB Editor.** **Even better: it also works if the Solid Region is created using the PCB Editor but saved as a PCB Module.** * It does **not** work if the Solid Region is first created a a PCB Lib and then placed on the PCB. This is because there is no way to assign a net number to the Solid Region when it is created and placed in this way. Remember that the tracks connecting to the antenna **and** the Solid Region forming the antenna itself **must** have the same netname because they are all shorted together then just route tracks to overlap the ends of the antenna where the pads would normally be placed. Tracks placed like this will not snap as they do to pads but they will connect and the Design Manager will verify that they are indeed connected. So the same rules and tricks as for a single-numbered multi-padded pad construction have to be used to then deal with any surrounding or adjacent ground flooding.