How can I get 3D board view without vias?
Didan , 05-11-2022, 09:44 PM
Hello, Robert. Iam using Altium v21 and I would like to know how can I get a 3D view without visible vias like in your project. I attached a picture from the board I designed and another one from your 28 pin project. Cordially, Didan.
robertferanec , 05-13-2022, 08:30 AM
It may not work in your case as your vias are unmasked (not tented). If they were, you just change transparency of the solder mask.
Didan , 05-13-2022, 08:37 AM
So, how can I figure it out? Basically, I just change via settings according to your course hole 0.3mmand 0.6mm diameter but i didnt see any other option. Can you send me a screenshot please
robertferanec , 05-13-2022, 08:57 AM
when you select a via, in Solder Mask Expansion, change it to Manual and check tented
Didan , 05-13-2022, 03:47 PM
Amazing Robert! Thank you. I was reading about importance of tenting vias as well. I Would like to share the reason i found from an article from pcbgogo website about tenting vias if anyone else is checking this question here: https://www.pcbgogo.com/current-even...rication_.html
At least now, It clarified how to do it in Altium and why pcb designers should consider to use tenting vias.Until next time ^^
At least now, It clarified how to do it in Altium and why pcb designers should consider to use tenting vias.Until next time ^^
qdrives , 05-13-2022, 04:45 PM
Tenting via's does have disadvantages:
- They can 'exploded' during the reflow process
- Chemicals trapped inside the via can corrode it.
Via protection is either through:
- Surface finish
- Filling and covering it.
Fabricators often open the holes even if you selected tenting just to prevent the disadvantaged mentioned above.
See another blog: https://www.eurocircuits.com/blog/covering-vias/
I set the solder mask expansion for via's to be 50um from the hole edge.
This gets the best of both worlds:
- Reduces chemicals trapped in the via
- Prevents shorts between them
- Reduced (or eliminates) the ability for solder paste to go into the via
- Allows you to probe them (measure voltage etc.)
- They can 'exploded' during the reflow process
- Chemicals trapped inside the via can corrode it.
Via protection is either through:
- Surface finish
- Filling and covering it.
Fabricators often open the holes even if you selected tenting just to prevent the disadvantaged mentioned above.
See another blog: https://www.eurocircuits.com/blog/covering-vias/
I set the solder mask expansion for via's to be 50um from the hole edge.
This gets the best of both worlds:
- Reduces chemicals trapped in the via
- Prevents shorts between them
- Reduced (or eliminates) the ability for solder paste to go into the via
- Allows you to probe them (measure voltage etc.)
robertferanec , 05-14-2022, 12:51 AM
I often ask question about chemicals trapped inside of a via and if solder mask can trap air inside of a via. I was told, it's not really that bad. This is what I usually get as the answers: PCBs are washed very well between manufacturing processes - chemicals from previous process must not stay inside of vias for the next process, so there should not be any chemicals trapped inside if a good PCB manufacturer is used. And about solder mask trapping the air - I have never seen problems with exploding vias and I was told that the air is not usually trapped there (solder musk just flows through the via, I am not sure what happens if the hole is too small, I think some PCB manufacturers may automatically add a small hole in the mask if they think it is required). However, yes, if it is really required, filling up the vias is the safest option to go with.
PS: I am not 100% sure, but I think in the old days the mask was spread over the PCB, now it is done through photo sensitive materials ... maybe that is what could make a difference, but I am not sure about that: https://resources.altium.com/p/how-c...-mask-your-pcb
PS: I am not 100% sure, but I think in the old days the mask was spread over the PCB, now it is done through photo sensitive materials ... maybe that is what could make a difference, but I am not sure about that: https://resources.altium.com/p/how-c...-mask-your-pcb
qdrives , 05-16-2022, 02:17 PM
1) It (may) happen(s) during reflow soldering.
2) What do you, as customer, see? If the board fails due to this, you should not have received it.
That is with liquid solder mask, not with dry film.
Perhaps this could be more problematic when:
- Using the board for a long time (> 10 years)
- Using the boards in more challenging environments (humidity, salt, temperature, etc.)
Yes, absolutely.
2) What do you, as customer, see? If the board fails due to this, you should not have received it.
That is with liquid solder mask, not with dry film.
Perhaps this could be more problematic when:
- Using the board for a long time (> 10 years)
- Using the boards in more challenging environments (humidity, salt, temperature, etc.)
Yes, absolutely.
robertferanec , 05-17-2022, 08:08 AM
@qdrives thank you for all your answers. I found one of the videos where I was asking about this, I may do highlights from it: https://youtu.be/FM3pRM0CxGw
qdrives , 05-17-2022, 02:22 PM
I had a conversation today with a fabricator. He stated that via's smaller than about 0.3mm would completely close with solder mask if tented. That was new for me.
He also confirmed the trapping of chemical residue (for larger via's) and/or popping when using dry film (or when air pocket is created with liquid) during reflow.
I will watch the video again.
He also confirmed the trapping of chemical residue (for larger via's) and/or popping when using dry film (or when air pocket is created with liquid) during reflow.
I will watch the video again.
Use our interactive Discord forum to reply or ask new questions.