How to check footprint correctness?


Using Freecad with KiCad stepup and the drawing dimension workbenches.


Import the footprint into freecad

Open freecad and create a new project.
Switch to the stepup workbench using the workbench selection drop down menu or view->workbench->kicad stepup
Use the import footprint button. This will start a file browser dialog. Navigate to your footprint and click open.

After clicking ok you should see the footprint within freecad. You will see the different layers as a body in the compo viewer.

Create dimensioned drawing to compare against datasheet

If the datasheet defines a landing pattern you can simply dimension the footprint directly and compare it’s values against that drawing.

Get the footprint into the drawing workbench

  1. Switch to the drawing dimensioning workbench
  2. Create a new page (Insert new drawing)
  3. Select the footprint layers you want to check by crtl+left clicking in the combo view.
  4. Insert the selected parts as a new view.
  5. Move all views somewhere within the page and maybe also scale them. (Make sure you place all views at the same place and scale them the same value.)

Dimension the drawing

The dimensioning tools will take a bit of getting used to. (There are other workbenches that have a better user interface but they do not really allow dimensioning between different “layers”)

Look at the datasheet and “copy” the dimensioning system. (Use the same relative measurements)

Example: Checking the Connector_Molex:Molex_Micro-Fit_3.0_43045-1215_2x06_P3.00mm_Vertical from the v5 repo.
Simplified datasheet (removed unnecessary stuff to reduce clutter for this tutorial) with highlighted dimensions.

Dimensioning system duplicated in freecad. (Highlighted the dimensions in the same colors i used in the datasheet.)

Using a sketch of the datasheet given values for the pin contact area

Freecad sketcher tutorial

If the datasheet does not give a landing pattern but only dimensions for the package it might be helpful to use a sketch that represents the pin contact are and measure the footprint relative to this.

Create a sketch using the part design workbench reflecting the contact area of the pin as given in the datasheet. Use the maximum area to be sure.
(If you have access to IPC standards, you can use the formulas and values for heel, toe and side given there.)

You also need to create a solid out of this sketch to be able to use it in the drawings dimensions workbench.

The sketcher might take a bit of time to understand. Use any freecad sketcher or part design tutorial to see how it is done. (Workflow: draw approximate outline, add constrains until fully constrained = dimension the sketch, extrude sketch)

Example: Checking footprint for TI-INAx180 against Housings_SSOP:TSSOP-8_3x3mm_Pitch0.65mm (or Package_SSOP:TSSOP-8_3x3mm_P0.65mm in the version 5 repo)

[Solved] How to link the pads with each other?
ATMEGA16U2-MU(R) / resistor packages
Serving Suggestions
Global Pads Coordinates check/table
Lesson in drawing schematics grinds to halt
Tutorial: How to make a footprint (From scratch)?
Anybody know how to get Sim900A footprint package
Measurement tool on creating a new footprint
[solved] Problem with "read the netlist" in newPCB
Tutorial: How to make a footprint (From scratch)?
Cvpcb picking footprint for scart and pin connectors
Diodes Inc SO-8 Footprint
Looking for footprint of an SMD oscillator
FAQ Index Thread