Platform forum

Solder mask

oscargomezf , 05-31-2016, 04:24 AM
Hi everyone,

Is it necessary to use solder mask in a project where I'm not going to use ​immersion or wave soldering?

I used to configure the rule. "SolderMaskExpansion" to 0mm Do you think it's ok?

Best regards.
mairomaster , 05-31-2016, 07:20 AM
The solder mask generally does not allow the formation of solder bridges between pads that are close together. It is not only about immersion and wave soldering. It is very important to have it for Reflow soldering for example, widely used nowadays for SMD boards. The solder mask serves other purposes as well, such as protecting the tracks on the surface layers, reducing the chance of shorts, corrosion, etc.

It is not a good practice to leave the solder mask expansion rule to 0 mm. This way during fabrication you might get solder mask partially covering your pads, because of fabrication tolerance. If it is a less dense design, I would use something safe like 0.1 mm. If it is a dense design and that creates clearance problems, I normally use 0.05 mm.

If you are creating new footprints, I recommend you to leave the solder mask expansion value for the pads set to "Expansion value from rules", and set a general value from the rule for the entire board. That way you can easily change the value for all pads on the board if necessary.
oscargomezf, 06-01-2016, 01:42 AM
Thak you very much, @mariomaster.
robertferanec , 05-31-2016, 07:26 AM
Excellent answer from @mairomaster.

@oscargomezf may I know why you are considering not using solder mask? I am don't think it influences the PCB cost too much.

BTW: maybe, if you really do not want o use mask, create your project properly (using the mask) and just tell your PCB manufacturer do not use it.
oscargomezf, 06-01-2016, 01:32 AM
Thank you robertferanec. I have no reason for considering no use solder mask. I thought it was better, but I don't have any problem to add 0.05mm. I've design all my footprints with soller mask expansion from rules, so it's easy to add solder mask.Does paste mask expansion has to be zero?Best regards
mairomaster , 06-01-2016, 01:37 AM
I always leave the paste mask expansion to 0. The manufacturers can adjust that themselves.
robertferanec , 06-01-2016, 01:41 AM
we also leave paste expansion 0
oscargomezf , 06-01-2016, 01:46 AM
Hi everyone,

Now I have a lot of errors related to MinimumSolderMaskSliver [I've got this parameter set to 0.08 mm], But this parameter depends on the manufacturer, doesn't It?

Best regards.
mairomaster , 06-01-2016, 01:50 AM
Yes, you have to verify with the manufacturer what is the minimum value you can use. Normally is in the range 0.05 - 0.15 mm. If you have those error, probably you have pads too close together (either in different components or the same component) which leave too little solder mask between them. This little solder mask bridge (sliver) might break during production which increases the chance of solder bridges between pads.
oscargomezf, 06-01-2016, 03:25 AM
Thank you, I see what you mean.
oscargomezf , 06-01-2016, 03:37 AM
Sorry, I've got another concern.

The parameter solder mask expansion for through hole vias have to be 0.05 too or, Is it better cover it with solder mask?

Best regards.
mairomaster , 06-01-2016, 03:54 AM
I prefer tenting (covering) my vias, since this is better in terms of solder mask violations and also silk screen text over such vias looks a bit better. If you need to use some vias as test points for debugging, it is easy to scrape the solder mask off them. I am not really sure what is the advantage (if any) to have the vias uncovered.
robertferanec , 06-01-2016, 04:50 AM
I mask the vias too.

Once we had problems with unmasked VIAs under BGA (it may create short circuits). Also when I had a PCB with unmasked VIAs, I had to be extremely careful when working with PCB - even a little bit of tin could make short circuit on PCB (especially dangerous when re-working stuff and when you place your board on the table where you normally solder)
oscargomezf, 06-01-2016, 04:54 AM
Ok thank you. I'm pretty sure you told me that in the course: "Schematic and PCB Design Course". But It has been a long time since I finished it, around two years (I have to review my notes) and I haven't the opportunity to design a real PCB.
oscargomezf , 06-01-2016, 04:50 AM

I've passed the design rules check and I've got this error in the 4 corners of my IC. I've set the MinimumSolderMaskSliver = 0.08mm and Solder Maks Expansion = 0.06mm.

What do you think it's the better option to solve this issue? I can only modify the Solder Maks Expansion in this 4 pins... but I'm not sure if this is the best option.

Best regards.
robertferanec, 06-01-2016, 04:52 AM
In critical places I make the solder mask expansion 1 mil (0.0254mm). That should fix your problem.
mairomaster , 06-01-2016, 04:53 AM
In such situations I often change the shape of the 4 corner pads to round instead of perfect (square) rectangle. That gives more clearance between the corners of the corner pads. I do that in the PCB library, since it will probably be an issue with every board.
robertferanec , 06-01-2016, 04:55 AM
I like @mairomaster solution!
Use our interactive Discord forum to reply or ask new questions.
Discord invite
Discord forum link (after invitation)

Didn't find what you were looking for?