How to cover vias with solder mask?

[cristi_m90]

How can I cover vias with solder mask? I've tried setting the Stop property in Vias Properties, but it does not work.

[ADresden]

There was an ULP for that, but you're right, it would be easier if you could select VIA type in the settings for the top and bottom layers.

The ULP, you generate a separate set of VIA covers, as most PCB manufacturers apply via covering separately. (2 masks) Mostly only specialty companies generate vias covered with the first solder mask outright. (Sony Playstation for example :P)

[edwin.robledo · Accepted solution]

Hi cristi_m90,

Thanks for your participation of the EAGLE forum.  We will do our best to provide you as much detail to answer your queries.

EAGLE displays the solder mask in a negative way, in other words, if you enable to TStop layer or BStop layer you will notice your pads acquire this shaded hatched lines.  This means those pads or vias are exposed.  If you wish to tent (cover your vias with solder mask) then change the Limit Value for your DRC/Mask parameters.

The Limit indicates the solder mask threshold for vias. Vias that have a drill size value smaller than the Limit will be tented, and vias that have drill size value greater than the Limit will be exposed. 

You can setup a Limit value to a size greater than your via drill, that way all vias are exposed. Now go to the properties of each individual via you and you can change the STOP mask properties. 

I hope this helps.

Best Regards,

Ed

[ADresden]

While a brilliant reply, most users will use it so rarely that it will pose problem again and again. That is why I suggested the tooltip help. When I hover over the STOP like in your picture, it should explain about the tented vias. "Less than this = tented, more than this = exposed".

The whole of eagle should be as easily readable. That is why I never actually found DRC useful, lots of complaints, lots of work (with errors within a margin of error), 0 extra results.

[o.quedens]

Hello,

I am really sorry but this is not working. I did all the steps you explained but still, the vias are not covered with solder mask...

Is there anything else I have to do?

Using eagle 9.1.3

Thanks

[jm2morri]

I answered something very similar yesterday.  Remember, soldermask is mirrored so any feature on that layer will become an absence of soldermask (i.e. exposed).

You can see the previous discussion here : https://forums.autodesk.com/t5/eagle-forum/vias-tended-only-on-1-side/m-p/8331671/highlight/true#M17...

James.

[rprajapatiTLBJU]

it works for me....i am able to mask the open vias. 

[scottezM9E2D]

How do I cover a via with solder mask on one side of the PCB, but not on the other?

[jorge_garcia2]

Hi @scottezM9E2D ,

I hope you're doing well. It's not easy but you would use the limit procedure detailed above and then manually draw a stop mask opening on the side you want exposed. You would draw a filled circle on either tStop or bStop depending on what side you want visible.

Let me know if there's anything else I can do for you.

Best Regards,

[chris.rouxel88]

I am making a flex PCB where we want tented vias. I was able to remove the solder mask by changing the ECR rules first. The gerber files are correct. However, the 3D PCB model still shows holes in the solder mask layer. I think it is a bug. 

[jorge_garcia2]

Hello @chris.rouxel88,

I hope you're doing well. You are correct the 3D PCB does not reflect tented vias. I'll make an improvement request for this.

Let me know if there's anything else I can do for you.

Best Regards,