Silk over via for protection
Hi @sergey8R4XS,
May I ask why do you need to do this? Wouldn't via soldermask tenting be sufficient?
Silk-screen objects, e.g.: text, lines, etc. can be placed over vias but the DRC Solder-Mask Clearance rule will be violated if this check is on, see: DRC dialog / Misc tab: Check solder mask check-box. You can Appove these violations if this is your intention. Either way you should tent the vias if you intend to cover them with silk-screen.
Please let me know if there is anything else I can help you with.
Kind Regards,
Constantin Popescu
Principal Software Engineer
Hi @sergey8R4XS,
Can't you achieve this by tenting all the vias if this is what you require? Then the solder-mask will cover all vias so no posibility of short-circuits to happen.
The way to tent the vias is as follows:
- In the DRC Dialog / Masks Tab you'll need to set the Limit value to the largets via drill diameter you have in your design. This way all your vias that will be below this limit will be tented (no solder-mask opening);
- In the via properties the Solder Mask field should be un-checked for all the vias that will be tented:
I have tested this using a simple design and the tStop mask is removed for all vias that have a diameter <= to Limit value. You can see it in the picture below:
The tStop (Solder-Mask) layer is turned ON and the vias don't have any solder-mask opening so they are tented (solder-mask will cover them fully).
I hope this will help you.
Please let me know if there is anything else I can help you with.
Kind Regards,
Constantin Popescu
Principal Software Engineer
Hi @sergey8R4XS,
This would not work if you need to have solder-mask opening. Then the only way is to cover them with silk-screen. This is possible and the default DRC settings will not generate any DRC violations. You'll need to turn off the options shown below (if any of them are ON) and this will stop the DRC from flagging any silk-screen over solder-mask opening violations then you can cover your vias that are not tented with slik-screen if this is what you need to do.
Please let me know if there is anything else I can help you with.
Kind Regards,
Constantin Popescu
Principal Software Engineer
Hi @sergey8R4XS,
Thank you for posting in the Electronics Forum; we really appreciate your participation. This is a really good question, but I have never heard of placing Silk Screen on top of Vias as a method to protect the via from Heat. Was this a recommendation from the Manufacturer?
As Constantine replied, this is usually accomplished by tenting the vias. I wanted to add just a few points to consider. -
- You can set the limit so that all your vias are tented, then go to each via property that needs to be exposed.
- Another method I have seen is to use two different via sizes. Then, set the DRC/Annular Ring limit to a smaller size.
- If you plan to use an output such as ODB++, then consider changing the DRC Layer Properties for your bottom Solder Mask to a thicker value. Before you do this, you need to ask the manufacturer which values are supported.
I hope this helps.
Best Regards,
Ed
Edwin Robledo
Tech Marketing Manager
Thank you for your reply.
I just wanna mention a main idea which I wanna rich.
1. as you see in the image back side of PCB board has contact with the radiator. So all vias should be protected from short circuits.
2. some of ICs have a termal pads which should contain vias as well as in the image below.
So diameter could be the same and even more for termal pad vias we may have to tint from one side (back) and stay clean (for soldering) from another.
Or maybe is it possible to set that one side of board should to have tint layer over all components?
