Add exposed copper layer

Projects
1

I made a PCB for a customer but it came with a design flaw. I am not sure how to fix the flaw. He wanted to ‘take the risc’ and now I have a 100 useless PCBs instead of 5 (like I recommended to prevents these kinds of issues)

First, I am trying to recreate something which looks like this.

afbeelding

My design looked okay in pcbNew’s 3D viewer

afbeelding
afbeelding1189×759 38.5 KB

It was however not okay at all. I examined the used layers of an SMD pad. And I made zone with those layers enabled.

afbeelding

The thing I missed…it is a non-copper zone. I had zero copper or any other layer at all at the silver colored areas. I am looking directly on the epoxy of the pcb.

I am now not sure entirely how to fix this. I added another zone, a copper zone, on top of the other.
afbeelding

I am not sure what to expect this time (besided no more than 5 possible ruined ones instead of 100 ).

Now I have copper, front paste and front mask. Can I expect the desired tinned plating?

Kind regards,

Bas

2

Front paste is the layer used to manufacture paste stencil (thin (like 0.2mm) metal sheet with openings for paste). If you don’t plan to order paste stencil (what I suppose) then you not need paste layer.
When you order PCB you should be able to specify if you want copper to be finished by gold plating or PbFree HAL. The second looks like at your 3D view.

You should know that copper is not very strong fixed to PCB. If there will be some force I would be not sure it will not be tear off.
It will be much more robust if you have a serie of plated vias connecting your top copper with copper on the bottom side. Until you not order tens of square meters of PCB the cost of 2 layer PCB should be the same as single sided, I think.

Did they done so sharp corners in your rectangle opening as at your 3D?
If yes - I wonder how did they done that?
If no - did they asked you for acceptance for doing it not according to your design?

3

Did they done so sharp corners in your rectangle opening as at your 3D?
If yes - I wonder how did they done that?
If no - did they asked you for acceptance for doing it not according to your design?

After I get home, I’ll post a photo of one of them. Besides the lacking metal the shape looks pretty much okay to me. Just a tiny bit too much backlash when you insert 2 PCB’s in eachother but that’s a manufactor tollerence vs design thingy. But I am content with the sharpness. I was not asked for acceptance.

You should know that copper is not very strong fixed to PCB. If there will be some force I would be not sure it will not be tear off.

The original design does not have vias either, but it surely is a good tip to use them. I can fit them underneath where the rails will be.

Regards,

4

Picture of les miserabeles :sweat_smile: FUBAR

afbeelding
afbeelding1080×1920 211 KB

5

It ALWAYS pays to check the Gerber files before submitting a board to be manufactured.

1 Like
6

OPs problem is that even looking through gerbers he would not notice the problem. I hope it is already past.

7

…he would not notice the problem.

OP’s problem is that he still has things to learn :wink:

I was simply not in the habbit to examine gerber files not that I don’t know how to. Until yesterday I never had to. I merely do DRC on schematic and PCB, than do a visual check on schematic and board and lastly I check the 3D viewer if it looks okay. I even let a coworker sometimes review me hobby projects.

Atleast now I know the 3D viewer can give a little bit misleading information. I will ofcourse keep this lesson in mind and add gerber examination to my checklist :white_check_mark:.

I am currently examining the old and new gerber files.

The old with the obvious problem.

afbeelding
afbeelding1553×857 49.7 KB

And the new

copper layer

afbeelding
afbeelding1658×814 50 KB

Solder mask

afbeelding
afbeelding1628×440 19.6 KB

So if I understand correctly. If I have a copper layer and solder mask I can expect a plated copper layer to which I can solder the rails to?

Bas :coffee: :+1:t2:

8

A thought?

If these rail connectors/locators are being made originally with double sided board, it would pay to place the same copper on the other side and attach the top and bottom with vias. This way, wires could be attached on the underside without being obtrusive.

9

It would also add to the adhesion of the copper to the substrate, as has already been mentioned . . .

10

added! I may double the amount though. The stresses arent that extreme. I think it will suffice

afbeelding
afbeelding1192×362 65.7 KB

11

When the stars are aligned. I managed to find me another problem :smiling_face_with_tear:

I added vias. I also made a new net. The copper plane has no net

afbeelding
afbeelding1416×590 16.9 KB

Than I assign the same net to the copper field

afbeelding
afbeelding1008×738 21.1 KB

And the plane dissapears

afbeelding
afbeelding1168×522 19.5 KB

The outlines of the fields are there, it just isn’t drawn. This seems a bug to me, but I don’t any better…

Regards,

Bas

12

Be sure that it is not problem to have both rails at bottom (can be a problem if used at metal surface).

13

It will be gold plated or HAL depending of specification when ordering. Gold is gold, HAL is tin.

14

I’m thinking ‘Simple-Minded’ and if I were doing it, I would simply make the Shape and place a Cu Track on it with Via’s.

I would create a Drawing or place Text on the PCB that indicates ‘Exactly’ what I want… Quick example below (“TYP” means ‘Typical’ in Drawings)

Screen Shot 2023-04-19 at 09.04.14
Screen Shot 2023-04-19 at 09.04.141600×702 160 KB

15

Can somebody tell me why my copper planes dissapear as soon as I add a net to them?

16

Have you already filled zones (for example, hit B key)?

17

Many times. If I add a net and I press B, they vanish. The outlining of the zone is there, it just is not filled. I cannot see the copper in gerber viewer as well

18

Imagine a zone placed on all the PCB with many footprints and tracks on it. When zone is filled it can be divided into many islands. If island is connected to any pad with the same net then it is filled. If not it is not filled as unconnected copper is not what electronics like.

Edit:
As you said that they dissapear I can suppose then may be zones with no net specified are filled.
If so then left them without net.
If my understanding of what you said is wrong then you have to add a pad having the same net. Pad can be smaller than your track so it will have no effect at PCB you get. At PCB Copper at copper is still only one copper.

19

I just noticed the same thing: a zone with a net needs a pad, too. A netless zone is filled by default if its “Remove islands” property is “Never”.

20

Instead of using a net and adding a footprint, you can also add this to Board Setup → Custom Rules:

(version 1)
(rule x
(condition "A.Type == 'Zone' && B.Type == 'Via'")
(constraint clearance (min 0mm))
(constraint hole_clearance (min 0mm))
)

Then the vias and zone can be without a net.

You can also set the Default netclass clearance to 0, zone clearance to 0, Board Setup → Constraints → Minimum clearance to 0 and Copper to hole clearance to 0.

It’s up to you to to decide which solution is the most professional for your complex and demanding design.

1 Like