How to delete solder mask opening?

[asadi.siyavash]

Hi,
I set 8 layer PCB to manufacturer but he sent me question file and said:
question: the soldermask opening of many vias are same size with holes and they are located in BGA areas,pls confirm
Recommendation /suggestion :
delete their soldermask opening
What I did:
Vias under BGA parts has 23mil Diameter and 12mil Hole Size. I changed Via's Solder Mask Expansion to specify expansion value = -6mil but my problem doesn't solve, please help me it is urgent.
(I use Altium Designer)
any help would be greatly appreciated.

 

[FvM]

I fear the question isn't completely clear.

Firstly you didn't tell what you wanted to achieve. A screenshot from a gerber viewer would be helpful to understand the situation.

Usually you don't want vias with full soldermask opening in the BGA area to avoid solder shorts and possible solder drain into via holes. You can either use tented vias, as apparently suggested by the PCB house, or reduced soldermask opening, which is my personal favour. In the latter case, the opening must be larger than the via hole to get clean soldermask structures despite of positioning inaccuracy, e.g. 100 µm all round after all solder mask corrections have been applied.

This will result in an opening that is still smaller than the via copper feature and thus achieve safe distance to BGA balls.

 

[asadi.siyavash]

Hi FvM Thank you,
I changed solder Mask opening with changing VIA solder mask Expansion to specify expansion value = -30 as you see in picture '0' .
I think with this work some problem solved but manufacturer sent me again these two questions:
1:there are still some vias whose soldermask opening is same size with hole size,pls confirm (recommendation: increase their soldermask opening to drill+6mil and do not plug them)

2:As the fig2 shown,many vias are located in smd pads,it is better to plug them by resin for ensuring good solderability,pls confirm(recommendation: plug via-in-pads by resin)

is it possible how I can solve these problem in Altium?
Any help would be greatly appreciated.

 

[FvM]

I don't understand the parameters in the via dialog. You initially told about -6mil expansion, now you have absurd -30. A reasonable value might be -3 or -4.

Vias in pads is a new problem. I don't think that it's acceptable except for large thermal pads. Simple resin plugging without metallization can affect the solderability.

 

[ArticCynda]

Make it a good habit to apply tenting on all vias that are located under components, especially ICs, unless they serve a thermal conductance purpose (i.e. exposed center pad). Leaving via's untented will only increase the chance of shorts, and if they're located underneath a component you won't be able to use them for probing anyways.

Never place a via on a pad, while this may seem like a good idea to save space on the board, the solder will drain through the via, causing a poorly soldered joint (reduced mechanical endurance) and increasing the chance of tombstoning.

 

[asadi.siyavash]

THANKS ARTICCYNDA. For tenting via I should do any change to PCB or just tell to manufacturer?
also how I can Plug Via in altium?

 

[ArticCynda]

In the via settings window you posted a screenshot of above, tick the checkbox "Force via tenting on top" (or bottom, depending on the side of the board your component is on). Altium will then remove the solder mask cutout from the top/bottom solder layer.

 

[FvM]

Some PCB manufacturers discourage customers from tenting vias on one side only, because they can't be properly rinsed in their process. Therefore I use untented vias with reduced opening regularly, they are compatible with all processes, safe against solder shorts and can be optionally used as test points.