I would like to ask for one of those framed stencils made by JLCPCB. But I have found some problems:
I have decided to apply the clearance on the top paste layer by myself and send this layer, but the fiducials of the stencil are also reduced and I don’t think this is a good idea. I think the size of the fiducial must be the same size on the board and the stencil. Can I remove the clearance in these pads?
I want half etched marks as fiducials but I need that these marks are on the bottom side of the stencil (machine preferences). I found this on the web but it sounds complicated:
About the (top or bottom) selection, it depends on the solder paste that you will use to draw the fiducials, if you want them to be half etched at the top then draw them at the top solder paste layer, if you want them at the bottom side of the stencil then draw them at the bottom solder paste layer of you PCB design. Stencil Half Etched Fiducials
On the other hand, Bing said:
Add a remark in the stencil order specifying that the fiducials should be half-etched on the bottom side
It makes sense.
Have anyone asked to a framed stencil in JLCPCB and can help me?
Your question number 1 is about KiCad, but for number 2 you have to ask JLCPCB (we have to try to keep this forum focused on KiCad specific discussion lest it become a generic electronics forum).
For number 1, please give some more details – how you have implemented the fiducial in KiCad? KiCad’s own fiducial footprints don’t have paste layer, exactly because fiducials shouldn’t have paste on them.
As I said, this “half etched fiducial” is new to me, I doubt if you have understood it correctly. The PCB has top/bottom (front/back) sides, but stencil doesn’t from the viewpoint of the paste layer of KiCad. First you have to ask if your stencil maker (JLC) makes half-etched stencil holes at all, and if they do, how they want it represented. You don’t even tell us if you will order the stencil for yourself, or a 3rd party assembler, or is it just for JLC. The stencil needs half etched fiducials only if the assembly machine needs them. So, make sure you understand your whole process first and who actually uses the stencil and how.
I use fiducials in KiCad library for pick and place machine, but I define a new one adding a top paste layer for stencil because I need matching the position of pcb and stencil.
The stencil is for the company I work. Recently, the company purchased a new solder paste printer machine and it seems that it likes half etched fiducials.
My problem is I thought that these marks on stencil and fiducials on pcb must be the same size and I cannot do that in KiCad. You cannot skip a footprint if you add a general solder paste clearance.
Yes, you can edit this particular footprint clearance but you cannot remove the general clearance you added before, but maybe I am wrong and the size matching is not needed I must look at that again. Thanks eelik.
You can define a “Clearance Override” in the Pad Properties for your fiducials. If you set this to some small value (say 0.001), the size of your fid will be -almost- preserved.
That’s a practical good solution. If the graphics needs to be in the paste layer, the theoretically “right” way to do it is to use a separate paste-only pad. It won’t be modified by the clearance. Maybe you can also add graphics directly in the layout without a footprint. In any case you must communicate with the manufacturer.
If I Understand Correctly (big “if”), then stencil fiducials are a slightly different concept than PCB fiducials. They have the same name, and may look the same in Gerber data, but they are used differently, for different reasons, and perhaps KiCad was bringing over too much baggage (including solder mask clearance) from PCB fiducial pads.
A PCB fiducial pad is just a landmark, so that pick-and-place (or inspection, or …) machines can figure out precisely where on the (fixed-in-place) PCB something should go.
A stencil fiducial is used to position the stencil itself; it functions more like a tooling hole or fixture pin than a PCB fiducial. (Though the actual alignment might still be visual.)
By default, a stencil fiducial should be treated less like a pad (even a fiducial pad or other stencil pads), and more like a Non-Plated Through Hole.
I think the solder mask clearance is needed to get a better contrast with the camera of the machine.
But stencil fiducial has two parts: The pad in the PCB and the hole or the mark in stencil. In my case, I need a mark in the down side of the stencil. Here it is:
Finally I managed to get apertures without reduction using SMD apertures in the design of the footprint, taking the example of “SOIC-8-1EP_3.9x4.9mm_P1.27mm_EP2.29x3mm”:
