I’m having trouble trying to verify the placement of certain footprints against my 2D UI design drawing which dictates their exact location. In my 2D drawing, the origin is the bottom left corner of the enclosure.
In order to place the footprints, I used the Grid Origin tool in PCB New to place the origin somewhere inside the default page layout, then zoomed in right on the center of that with my mouse pointer, and pressed spacebar to set that point to 0,0.
From there I used the Position Relative To command and put the footprints in the appropriate place in relation to my user defined origin. So this is all fine and good and allowed me to place my footprints.
The problem now though, is I need to verify that the locations are correct before sending away for manufacturing. I can’t seem to find any way to do this that isn’t very clunky and makes me think I’m doing something fundamentally wrong.
How do I see it’s location relative to my user defined grid origin? When I select a footprint and view its properties, it shows me the location relative to the absolute origin point. I mean, I can zoom in really close and make sure my mouse pointer is perfectly on the footprint origin, and then look in the bottom right corner at the cursor position, but that seems super clunky and error prone. There must be a simpler way. What’s the correct workflow here? Thanks!
For some reason that report is not showing me any components on “back side” which is the side I need. But regardless, all the Top side components show their location relative to the absolute origin, which doesn’t help me.
Ahhh ok, thank you. That info about the Place Auxiliary Axis is crucial! Ok so now my pick and place and drill files will be correct, thankfully.
The footprint position window seems to only give SMT footprint positions, but I’m looking for the positions of my through hole (UI) components. So I’m still looking for a way to verify their positions relative to my user defined origin. Surely there must be a simple way to do this.
Is this a new preference that’s been added into 5.99? If so that’s great!
I’m kinda new with Kicad…where do I find 5.99? I guess this is a beta (nightly) build because I see 5.1.9 as the latest download on their site. Should I be concerned about using a nightly build or are they fairly stable for the most part? Thanks
I only see one solution here: edit every single THT component properties and mark them as SMD.
Be careful with the positions. In the official libraries the anchor of a THT footprint is placed at pad1 in most of the footprints (if not in all of them) while the SMD footprints have the anchor at the centre of the footprint.
That is why I place my PCB relative to the absolute origin. I frequently have symmetrical cases (DIN rail) so I place my PCB such that its center is at absolute origin.
In your case I would place my PCB to have the absolute origin at the same point that it is at your drawing.
Thanks for all the help everyone. Ok, I see there is no simple way to do this with my current version, which still seems odd to me. I agree that using the absolute origin from now on seems like the way to go. Just seems strange that the absolute origin is outside of the page boundaries by default.
Can anyone confirm that the 5.99 build has an option to use the auxiliary axis as the reference point used when looking at a footprints location properties, before I update to that version? @RRPollack mentioned this might be the case.
The internal origin is actually at the upper left corner of the “page”. The worksheet you see on the screen allows margins around the printed border because printers can’t print to the edge of the paper.
I can confirm it’s in there, as I am the author of that change. It was merged into the 5.99 development branch last fall. I’m working to extend this to the footprint editor, but I missed the cut-off for such changes for the upcoming 6.0 release.
The only thing this change does is to alter the displayed coordinates. These are user options, so if you have multiple people working on the same file, or use multiple systems for your work, you’ll have to change the options for each user or system. Changing these options does not change the board file at all, so you can play around with the various options without risk to your work.
another option which i didn’t see mentioned is to make a reference drawing (i do this kind of thing in librecad) and import it as DXF either into pcbnew directly, or make it a footprint
