Could it be possible to remove PADs from paste stencil?

Layout Footprints
1

Hi

I 'am a beginner with Kicad. I designed a 6 layers PCB. An i have a question regarding the paste stencil.

I designed a PCB to be modular. it can accept one of three different communication modules: a SIM7000G, a SIM7020 and a Lora module from Murata. These modules are located in the same area on the PCB but the three module’s size are different. We designed the three different footprints that are included in each other (see print screen below).

image
image1600×900 221 KB

The stencil used include the three footprints whereas only one is used, the largest one. I suspect that a short-circuit could appeared between one of the smaller footprint with the largest one when we weld the largest one (SIM7000G).
My question :slight_smile:Is it possible to remove from the paste stencil the unused fooprints?
Could be possible do define a parameters for each components that define if this componenst will or will not present on the paste stencil. Of course the footrpint no used will be graved also but covered by the soldermak.

I thank everyone in advance for your remarks and propositions
Best regards
Serge

2

I think your best option is just to temporarily delete the footprint from your board when preparing to plot the paste layer.

3

The most flexible option is to put tape over the stencil area that should not be used. (Allows one stencil for all possible arrangements)
Otherwise make the footprint specific for your current case but then you will need 3 different stencils -> you can then already make 3 different pcbs as well as it will not really save you any cost anymore (stencils are quite expensive compared to pcbs)

4

(stencils are quite expensive compared to pcbs)

at hobbyist scale this isn’t really true, JLCPcb for example will make a stainless stencil for $6, and if you have them trim it to ~100x100mm, it ships for free in the same box as your PCBs.

at large scale I could also imagine it might make sense to have 3 stencils and a multipurpose board vs stocking 3 different board variants.

5

Hi Hlachal Hi Rene_Poshi,
I thank you for your answers .
In my case this PCB is for large scale production.

So, If I understood both of your Answeres, I should generate 3 variants, each one with one foortprint of the 3 modules. Thsi will allow the generation of just three different paste stencils.
I will produce one unique PCB (with the three foortprints) and requested de use only one of the three stencil.
Is that Possible when we provide Gerber files to the PCB manufacturer.
Sorry for my “naive” question. I don’t know much about PCB manufacturing.
Thanks
Serge

Is this scenorio possible when for a

6

…whatever “large” means. For some it may be 100 or 1000; for others it may be 1000000.

This is very important. If you do that, you have to make three different boards anyways, so it doesn’t necessarily make much sense to put all variants in the same board. Especially if these aren’t prototypes but for “large scale” production. On the other hand further changes are easier if you have only one project and one layout, but then you have to manage three different solder mask configurations somehow.

It’s also important to know how they will be assembled. In a factory or manually by you? If the former, you should make three stencils.

7

When I read soldermask I wondered about the thinking. If you know in advance which part will be covered by solder mask then copying the design to a new folder and modifying it so that you don’t have the extra footprint is the way to go.

It sounds like you’ll know which board to produce before a run anyhow?

8

You could make 3 design files, but that’s clumsy for upgrades.
What might work, is to make those PADS with a unique value, and then massage the Gerber file.
eg I just tried this

G04 APERTURE LIST*
%ADD10R,1.300000X0.251235*%
%ADD11R,1.300000X0.250000*%
%ADD12R,0.251235X1.300000*%
%ADD13R,0.685800X0.787400*%

Those long values of 0.251235 are designed to be unique and easy to find.
If I then edit those 2 lines, to zero-out those unique pads like this

G04 APERTURE LIST*
%ADD10R,000X0*%
%ADD11R,1.300000X0.250000*%
%ADD12R,0X00*%

Voila, the paste gerber has removed those pads.
A small script could automate this, or you could do it manually if you expect few revisions.

I think you can also enter a specific paste-pad stack of 0, for paste layer if you want a permanent change, short of a total part delete, and that should over-ride paste plots…
ie if you explicitly define a paste info, that info trumps pads shape info.

9

And what would be the extra cost of having 3 different designs ordered with each only a third the number of what you would order otherwise? (This is what you need to compare it against.)

In the end you could then really specialize the pcb and take advantage of the smaller parts (get decoupling caps nearer to it, better EMC by having fewer crossings, …)

10

you can manually turn off the paste area on each pad by opening the pads properties and unticking the Fpaste box, do this on each pad and it will not be cut on your stencil.

2 Likes
11

I wonder if a script can do that inside pcbnew, allowing a single design file ?
It would de-paste 2 of 3, maybe using ‘selected’ as the one to (re) paste ?

12

What about just saving off three different gerber sets in different directories?

13

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.