FEDEVEL
Platform forum

rubenB , 08-23-2024, 07:35 AM

I followed Robert's tutorial for making ESP32 and when I uploaded my gerber files, I noticed an additional drl layer in jlcpcb. Robert's video does not have these vias showing in top and bottom layer as well as the drl layer.
What could possibly my error?

Robert Feranec , 08-23-2024, 01:38 PM

your is correct, i didnt show the drill layer in the video ... I thought no one will notice 🙂

Robert Feranec , 08-23-2024, 01:39 PM

be sure the vias are masked / tented

Robert Feranec , 08-23-2024, 01:41 PM

when I am checking the materials after ordering the PCB it shows the drilling ... you can jump there (but I only show it in gerbers)

Robert Feranec , 08-23-2024, 01:43 PM

rubenB , 08-23-2024, 02:28 PM

I see, I was just worried since some of the top overlays were cut off by the vias since they were overlapping. Thank you for your help!

QDrives , 08-23-2024, 07:29 PM

Why would the vias need to be tented?

Sniper2 , 08-24-2024, 08:53 AM

safety?

Sniper2 , 08-24-2024, 08:54 AM

harder to short out 2 vias

Sniper2 , 08-24-2024, 08:54 AM

+ looks better

Robert Feranec , 08-24-2024, 09:25 AM

one problem is under BGA. But mostly I had to be super sure there is absolutely no dirt on PCB, especially when I was debugging the board and I had to move it a lot between soldering table and my table or when I was just holding it in my hands and there could be very small pieces of solder or copper wire or something ...or even low conductive materials e.g. flux could influence signals. So I had to often inspect the boards and clean them - especially very high density boards - it is just via everywhere.

Mini , 08-24-2024, 10:16 AM

Also don't forget about when putting your device outside. Harder to corrode. But indeed you have to have a coating on anyways. I always use tented via's and mainly it's because it's harder to short them and of course during soldering no worries about solder sticking on them.

QDrives , 08-24-2024, 12:00 PM

Ok, but this board is not high density.
You can also do "encroached" vias, or negative solder mask expansion.

QDrives , 08-24-2024, 12:16 PM

There are many problems with "tenting" vias.
1) It is not defined how. This mainly comes from the various methods of applying the solder mask. Dry film, liquid photo resist, etc. and also if the fabricator changes the 'gerbers' to open the via's.
2) Chemical residue can be trapped inside the via causing corrosion
3) The vias can pop (open) during reflow.
4) It is harder to do (debugging) measurements as the vias are covered.
https://www.eurocircuits.com/blog/covering-vias/

It is true that is harder to have shorts between vias. I had that happen with a wave soldered board.
However, I now use the negative solder mask expansion and that work great too. See the picture in my previous comment.
Solder will not (or at least seldom) enter the via.

Sure, you 'see' the vias more clearly in this picture. But I had liquid photo resist solder mask on boards "tented" and there too you could see the via's.
If you absolutely want to hide the via's, you need to go to filled vias. If you plate over them, you can also place them in pads (VIPPO - Via In Pad, Plated Over).

As for outside use and corrosion: the inside of the vias will have the surface finish when open. With tenting, this is more undefined (see points 2 and 3 above).
Better is to use conformal coating or potting. For conformal coating, it is best to have the vias filled too.

QDrives , 08-24-2024, 12:24 PM

See the vias here. Some are open some covered. All of them were specified as "tented".
Not all 'invisible'.

Robert Feranec , 08-24-2024, 12:51 PM

We took some pictures of resist in vias, I was surprised it actually flows through even for small diameters. I will talk about it when I make video from the materials.

Robert Feranec , 08-24-2024, 12:51 PM

it completelly filled up the via inside

QDrives , 08-24-2024, 12:52 PM

Again, it depends on the material and process.

Robert Feranec , 08-24-2024, 12:56 PM

also, about chemicals trapped inside of VIAs - I talked about this with some PCB manufacturers and I was told a good PCB manufacturer should be able to clean PCBs very well as anything left from previous process could influence the next process. but I guess it may depend on PCB manufacturer.

QDrives , 08-24-2024, 01:04 PM

Naturally a fabricator will tell you that their process is perfect.
My data comes from Eurocircuits - a fabricator and EMS (link provided in earlier comment), and from TBP an EMS that makes boards also for ESA, ASML and military.

Sniper2 , 08-24-2024, 07:31 PM

newer had that problem , maybe those via are simply to large for that type of mask

QDrives , 08-25-2024, 03:07 PM

What kind of solder mask was used? Dry film, liquid photo resist, other?
And yes, what size vias did you use?

Sniper2 , 08-25-2024, 03:42 PM

mask: green didnt specify so dont know but i guess liquid by the look
via size 0.5/0.2mm

Sniper2 , 08-25-2024, 03:42 PM

@QDrives

Sniper2 , 08-25-2024, 03:46 PM

other via types were untended for some other reasons

QDrives , 08-25-2024, 08:39 PM

All the vias in the picture with the black solder mask were specified being tented.
My vias were 0.9mm pad size and 0.4mm (finished) hole size.

For the green board, it was 50um (0.05mm) from hole edge.
Vias there 0.6mm pad, 0.3 finished hole.