Download Microchip PIC18F27Q43 VQFN Footprint C

Can some check the Microchip generated footprint for the 4x4 VQFN28

I’m having trouble trying to route just about with any PCB thickness
I think the keep outs are wrong.

Footprint be downloaded from here
https://www.microchip.com/en-us/product/pic18f27q43
or here

Regs Joe

I hereby certify that I am not simply asking someone else to design a footprint for me.

This is an auto-generated message that is in place on the “footprints” section of the KiCad.info forum. If I remove it and ask for a footprint to be designed anyway, I understand that I will be subject to forum members telling me to go design my own footprint or referring me to a 3rd party footprint site.

I don’t know this MCU but why futz around with 3rd party footprints when there appears to be a suitable one in the KiCad library: VQFN-28-1EP_4x4mm_P0.45mm_EP2.4x2.4mm

Thanks,
“why futz around with 3rd party footprints”

-1 I was hoping some could test this footprint (in case it was my error and not Ultralibrarian)

  1. I could not find a exact match in any of the KiCad Libraries
  2. The pad pitch is 0.4mm not 0.45
  3. The exposed pad is 2.65mm x 2.65mm not 2.4mm x 2.4mm

The source of the information comes from the data sheet page 946, 947, 948 of the data sheet here

3rd party footprints often have errors. If you can’t find an exact match, you can often make a footprint using the Wizard in the footprint editor.

Here’s a footprint generated by the QFN wizard. I’ll leave it to you to tweak (or twerk :crazy_face: ).

I have never seen footprints at Microchip, but that might by my fault. So please, where can I find them at the link you have.

Plus, ultralibrarian requires registration.
And they say “Please refer to the latest revision of the manufacturer’s datasheet to confirm product specifications (Symbol, Footprint, and 3D Model). Note that it is the user’s responsibility to verify all specifications before using the provided content.”

It looks like the KiCad libraries do not include the Microchip package with 0.40mm lead pitch

ul_PIC18F27Q43-I-STX (3).zip (11.5 KB)

Ohhh I have posting upload privileges now - see KiCAD Library attached.

Hoping some can test the clearances.

“We must accept finite disappointment, but never lose infinite hope” I think you should check it yourself and rise a kicad question if you’re in troubles.

1 Like

OK I have already tried when I try to route a trace of any thickness from one of the pads of the PIC18F27Q43 I get two green highlighted PAD either side and KiCAD can not route trace.

Hence I am asking some one to quickly prove me wrong an able to route tracning from this footprint.

Can you do it?

Green?! On what layer are you working?

F.Cu. See attached

The exposed pad is too close to the other pads.

Here’s how this can be solved:

  • Reduce minimum clearance constraints
  • Make the exposed pad smaller
  • Move other pads further away from the exposed pad

Thanks dsa-t!
Do these 3 items suggest the download foot print is not correct?
Given these 3 are set up by the foot print?

What is your reason for wanting to use this part?

0.4mm is a quite narrow pitch. It’s easy to route in KiCad, but you have to adjust the design rules in KiCad to set them to smaller track width and clearance as dsa-t already mentioned.

The problem here, is that when features on PCB’s become to small, you have to select a PCB manufacturer which has it’s process tuned to a fine enough accuracy, and that is a more expensive process. So the tradeoff is a slightly smaller PCB for a higher cost.

I see nothing wrong with the footprint. It just is (probably) not compatible with the default design rules in KiCad. KiCad works with nanometer resolution, and that is far more then any PCB can be manufactured.

Constraints are set up in Board setup, not in footprints.

Looks like this footprint is designed for clearances around 0.1 - 0.125 mm, not 0.2 mm like you have in your Board setup.

Thanks dsa-t

Thanks the design has very small PCB size requirement

Thanks Everyone!

I understand a wish / need for a small PCB. I see you have found how to change KiCad’s default design rules so this IC can be routed. But that you had to search for it, means you don’t have much with KiCad yet, or maybe even with PCB design. I advise that before you continue with routing, you select a PCB manufacturer and make sure that the design rules you set up in KiCad is actually compatible with what your PCB manufacturer can manufacture reliably.

In general, the advise is to set the rules in KiCad a bit coarser as the minimum that a PCB manufacturer states. Many PCB manufacturers have different processes for PCB’s. 4 layer PCB’s are more expensive then two layers, but this is only partially for the extra copper layers. 4 layer PCB’s often also have a higher resolution. Are you planning for a multi layer PCB?

1 Like

Also note that if you use 4 mil ≈ 0.1 mm clearance/track width, it can cost more with some manufacturers.

1 Like