Least, nominal and most footprint layout options

I noticed that on my stencil for STM LD39100 I had too small clearance between the bigger middle pad and 6 smaller pads. Tried multiple times and solder paste gots always joined between those pads.
(regular 0402 resistors, etc are ok)

I think I had downloaded the footprint originally from ultralibrarian but now I noticed that the STM is offering footprint also via samacsys (https://www.st.com/en/power-management/ld39100.html#cad-resources) which offers 3 different sizes for footprints. Least, Nominal and Most, the difference being on the pad size. I was thinking does the Kicad have support for having little different footprint sizes for different purposes. I could for example think of producing the Stencil with footprints using the Least option, while the PCB would be produced by using the Nominal or Most option?

How are you holding the stencil down onto the PCB ? how are you applying the paste ?

I designed (modified someone else’s idea) and 3D printed a vacuum bed to hold the stencil firmly and flat onto the PCB, it’s made a huge difference for me.

1 Like

It wouldn’t work for me.
I tend to blow a lot of hot air, rather than suck it up! :wink: :rofl: :rofl:


There is a DFN6 in the standard KiCad library. It is probably relatively old as it hasn’t got rounded corners but how does it compare to your footprint?

I’m a bit cautious about some of these downloaded footprints - especially for fairly simple designs where it is more work to go searching for it than to design it yourself according to the manufacturers data sheet.You could start by modifying the standard design.

If you regularly want different tolerance land patterns generated programmatically you might like to take a look at Qeda.

You do not really need different footprints for achieving this as the layers the stencils are generated from (F.Paste and B.Paste) are different ones then the copper and mask layers relevant for the PCB. You just need to adjust the paste layers on the footprint to match the least option, independent from how the actual copper pads are dimensioned.

I do not believe the problem is on the my paste spreading technique as for 0402 components there is enough clearance that paste does not get mixed.

Anyway, I actually use a little similar construction. I created the openscad project for producing the container, lidboard, stencil frame and pcb holder in the middle of stencil frame. Parameters are quite easility modificable on project to produce different size of containers depending of the pcb size.
(I have printed 162, 142 and 122mm versions of the box and frames and now I usually just print the pcb holder part for new based on their size, everything else is reusable)

There seems to be actually 2 which seems to be pretty close to each others:

DFN-6-1EP_3x3mm_P0.95mm_EP1.7x2.6mm and

How exactly check which one of those 2 would be the right one for LD39100?
In the ultralibrarian version of footprint, the pad width has been 0.825 mm, while on this design you showed it’s only 0.5mm. I already reduced the pad size to 0,6 on my design and I believe this will help me to have enought clearance between small and big pads. Now I need to order new stencil.

Thanks, I did not realize this but I kind of thought for the possibility to have these “least and nominal” versions of same footprint and then possibility assign the nominal version of it to copper layer and least version to F-paste layer. It would be kind of nice to have possibility of kicad symbol to have possibility to have both of these assigned. With most of the components this is probably not needed but with components like LQFP-144 this could be very useful to have just a little smaller holes for pads on stencil compared to ones on copper layer on pcb.

First, if you start mixing footprints from different sources, then there is no way of predicting the result. Different sources use different sets of rules. As far as I know, KiCad’s own libraries are pretty consistent.

I also do not trust recommendations in datasheets much. Those may be 20 years old, for an unknown soldering setup and never revised. Without knowing it’s background, such recommendations do not mean much.

Next problem is that you do not always get what you order. Some PCB manufacturers even state on their website that they expand stencil apertures by some fixed amount by default. (Or was it shrink? (I forgot which)).

A very old EDA suite I used long ago (Ultiboard) had three sets of footprints, depending on the “production class”. Big pads and big courtyards for ease of manufacturing, and smaller geometry for denser PCB’s. But that was over 30 years ago. KiCad does not have this by default, but it is quite easy to modify footprints to personal preferences. A lot of the footprints in the KiCad libraries are generated by scripts (Available on gitlab), and you can even use these to make custom footprints. But I do doubt it is needed (for beginners / generic use).

And last, KiCad has: PCB Editor / File / Board Setup / Board Stackup / Solder Mask/Paste and here you can override the aperture sizes for the solder mask:

You can also set this for separate footprints on the Clearance Overrides and Settings tab of the Footprint Properties

I think your stencil jig has a problem, you have no central support, when you apply the vacuum the whole top plate can be pulled down, with support only at the edge the centre can bow.

My design has support under all of the top plate . . .

Same for mine . . .

This sounds promising. So if I specify -10% for example to “Solder paste relative clearance”, it would would make all pads, etc. 10% smaller than in original footprint?

It does not change the size of the (copper) pads, but only for the solder paste layer. (I guess) If you want to be sure, then:

  1. Create a set of gerber files.
  2. Change some settings.
  3. Generate gerbers for that too.
  4. Compare the files in the gerber viewer.

It doesn’t look like anyone has mentioned the standard industry practice of reducing the amount of solder paste applied to thermal pads.

I’ve seen 3 basic methods used:

  1. Reduce dimensions of the solder paste - paste dimensions can be up to 50% less than the copper thermal pad
  2. Window pane - use 4 or more rectangles of paste with a gap between them
  3. Dots - use several circles of solder paste

The window pane and dots methods allow venting of gasses generated during soldering without blowing solder out (potentially causing shorts).

Another thing which can help is to reduce the copper pads so that there is solder mask between areas which tend to short.

1 Like

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