How to measure the maximum height of an assembly?

[Robert.Adams]

Hello everyone,

I'm playing around with FreeCAD (Mechanical) and figured I'd look at making a simple box for a project (using open source IMX6 which has Altium files already).  Unfortunately I do not know the maximum height of the PCB.

I've looked at the Board information report which gives the x & y dimensions.  I know I can click on components I think to be the highest and manually add up the height but this seems really inefficient.  Is there a better way to get this information (either in maximum total height or max component height per side)?

[T3sl4co1l]

I take it you don't have 3D info on all components, and thus can't simply eyeball the one that stands tallest?

Could probably do a query by Component Height and see where the cutoffs are (>1mm, >2mm, etc...).  Don't think there's a way to query the one tallest component; that would require an N x N comparison (or at least O(N lg N)), while Query is only applied to all N objects once.  For each side, just add "AND OnBottom" or whatever and do it again.

IMX6 is going to have a standard maximum profile, no?  So you could also specify component height design rules.  Probably one rule for OnTop, another for OnBottom, since they're probably different?

Tim

[marshallh]

2 ways --


1. Go to 3d view, and change the Projection to Orthgraphic. This turns off perpsective correction and allows you see the side as if it were a mechanical drawing.
2. Side view, eyeball the highest component. Easy


1. Create a dummy component with a huge 6 inch square simple 3d body, covering the entire board. Set the color to bright purple so any intersections will be visible.
2. Adjust the max height of the footprint (by editing the primitive) until it barely covers the highest component.

[Precipice]

Generate a BOM (from the PCB, not the project), and you've got height in mm, height in mils, as an option. Sort the resulting BOM by height (and side of PCB), and job done.

However, it's still tempting to export your case design as a STEP file, and import that onto the PCB as a final check, to see if anything lights up green. It's saved me some hassle with connectors lining up on holes before...