FEDEVEL
Platform forum

aaqibqureshi , 05-18-2024, 01:05 PM

I have gotten the following observation when ordering the PCB that "As per given data we found solder mask opening pads are missing in both side". Can anyone suggest what i have done wrong?

aaqibqureshi , 05-18-2024, 01:33 PM

This is the 3d view of second file

SirJames , 05-18-2024, 02:55 PM

From 3d view it seems like soldermask openings are there. Except C_PV and H7 have non-plated holes for some reason.

aaqibqureshi , 05-18-2024, 03:09 PM

These are the top and bottom view

SirJames , 05-18-2024, 03:10 PM

If first image shows etch in gray and soldermask in blue then there is clearly some soldermask missing. Maybe you forgot to add some layer into soldermask file when setting up gerbers?

aaqibqureshi , 05-18-2024, 03:11 PM

H7 is a mounting hole, so i kept it non plated. C_pv is plated.

SirJames , 05-18-2024, 03:13 PM

can you post only soldermask layer?

aaqibqureshi , 05-18-2024, 03:14 PM

aaqibqureshi , 05-18-2024, 03:15 PM

this is the second PCB

aaqibqureshi , 05-18-2024, 03:17 PM

Thank you for the reply sir. How can I enable only the soldermask layer?

SirJames , 05-18-2024, 03:26 PM

if viewer that you are using dont have any filters, you can use some other online gerber viewer or try downloading ViewMate. Standard license is free

aaqibqureshi , 05-18-2024, 03:39 PM

Cant i do it in altium

SirJames , 05-18-2024, 03:42 PM

oh, i didnt know you are using altium. Yes, there is gerber viewer with filters

SirJames , 05-18-2024, 03:45 PM

select only soldermask and see if it matches positions of all pads and holes that should be uncovered

aaqibqureshi , 05-18-2024, 03:49 PM

aaqibqureshi , 05-18-2024, 03:49 PM

these are top and bottom solder mask gerber files

aaqibqureshi , 05-18-2024, 03:50 PM

aaqibqureshi , 05-18-2024, 03:52 PM

this is the 3d view

SirJames , 05-18-2024, 03:54 PM

so it looks line only mounting holes, C1, C2 and R8 have soldermask generated correctly, right?

aaqibqureshi , 05-18-2024, 03:54 PM

aaqibqureshi , 05-18-2024, 03:55 PM

I think these are the ones for which solder mask hasnt generated correctly

SirJames , 05-18-2024, 03:59 PM

I dont use Altium but try to look into Gerber setup -> Layers. Maybe if you click on soldermask settings it will show which layers are used when generating files https://youtu.be/p310rOUhMTw?feature=shared&t=65

aaqibqureshi , 05-18-2024, 03:59 PM

I made these components myself. I placed pads at appropraite distances, selected hole size andcopper size only.

aaqibqureshi , 05-18-2024, 04:00 PM

maybe here i have made some mistake

SirJames , 05-18-2024, 04:01 PM

this image shows pad that is generated correctly, right?

SirJames , 05-18-2024, 04:02 PM

is there any difference if you click on one of pads of for example Q5?

aaqibqureshi , 05-18-2024, 04:04 PM

yes there is

aaqibqureshi , 05-18-2024, 04:05 PM

aaqibqureshi , 05-18-2024, 04:05 PM

This is for Q5

SirJames , 05-18-2024, 04:06 PM

and C1 is also component that you created, right?

aaqibqureshi , 05-18-2024, 04:06 PM

I created C1

aaqibqureshi , 05-18-2024, 04:07 PM

and got q5 from altiums library

aaqibqureshi , 05-18-2024, 04:08 PM

i mean manufacturer part search

aaqibqureshi , 05-18-2024, 04:09 PM

I havent entered value for solder and paste options in components i created

SirJames , 05-18-2024, 04:09 PM

well yes, but your components are fine

SirJames , 05-18-2024, 04:10 PM

the ones from library doesnt have soldermask in gerber files

SirJames , 05-18-2024, 04:11 PM

I think it is a problem regarding layers. I had same problem first time I draw PCB in Allegro. Parts that I created where fine but the ones I downloaded had their soldermasks excluded when generating Gerbers. Sadly, my manufacturer wasnt that mindfull 😄

SirJames , 05-18-2024, 04:12 PM

I'm sorry but I dont have enough experience with Altium but I think that problem is in this settings

aaqibqureshi , 05-18-2024, 04:13 PM

Thank you with the help

SirJames , 05-18-2024, 04:18 PM

Oh, don't mention it. Maybe someone will help more. If you resolve this issue, please let me know. I'm kinda curious what was the problem.

aaqibqureshi , 05-18-2024, 04:18 PM

I definitely will update

QDrives , 05-18-2024, 07:57 PM

The pad setup is wrong. Pad (copper) is ~150x90mil, hole is 70mil, but solder mask opening is 68mil. That means there is no solder mask.
Unless you have good reasons to deviate, set the solder mask expansion for all pads to "Rule expansion".
You can do so for all pads on the board by just selecting pads.
Do not forget to have your library correct too. Actually, it is even more important to have the library correct.
For the library there is the PCBLibList panel.

aaqibqureshi , 05-20-2024, 05:18 AM

Thank you for the help. Should i also keep the Paste option --rule based

QDrives , 05-20-2024, 02:50 PM

Generally you do not want solder paste on through hole pads, unless they are THR/PIP (Through Hole Reflow/Pin In Paste) compatible. This means that the TH parts can be soldered in the reflow oven.
Most TH parts are not THR, so the paste mask should not have an opening. This is by setting the size to 0 (zero) and shape to i.e. round.