A few components on my board must be placed somewhat precisely with respect to the edges of the board. I’m a new KiCad user and I’m confused about how to do this. I know I can alter the X and Y values in the Edit window, but I assume that only applies to the top-left of the footprint, but it’s the bottom edge of the footprint (or the pins in the footprint) that I want to align to. I would be able to get this “close enough” by eyeballing if I could just turn on a ruler or measure tool like I’d find in most normal design software, but I can’t find that in KiCad. Does it exist?
Is there some way to import a sort of semitransparent overlay into the PCB editor that would allow me to create a “traceable” board layout in a more precise graphic design program and then use that to place the components?
There is the measuring tool… bottom RH button beside the Appearance Manager.
There is Dx/Dy… bottom middle of your screen. Place cursor in position, press “Space bar” to zero, pick up a footprint with the cursor and watch the distance in x & Y or rad & angle with respect to the first cursor position.
There is Right click footprint to access "select " menu and half way down the list is “Positioning Tools” with four alternative methods.
Here are some instructions on two of the “Positioning Tools” methods:
Select and highlight circle to move
Right click, select “Positioning Tool” then “Position relative to” or hotkey “Shift + p”.
From newly opened window click “Select Item”
Select and highlight second circle (where circle to move will finish)
Window re-opens then select OK
Active and non-active layers are inconsequential with this function.
There is a bit of experimenting needed with this new function.
The full procedure for Move with Reference is:
Find the location you wish to locate (eg. the corner of a connector).
Place cursor on that position.
Press space bar. (this will zero dx & dy at that position)
Left click connector to move then right click.
Select Move with Reference.
Place cursor at the exact corner of connector and left click.
Move connector now attached to cursor using dx & dy readings until both zero.
Left click connector and the corner is now in the exact position.
Effectively, this has now, temporarily, moved the anchor for exact placement.
No. X,Y are the position of footprint reference point (anchor) as defined when footprint is edited. For SMD symmetric footprints standard is footprint center and for THT frequently the reference is its pin1. If you edit your own footprints you can set reference point as you want.
Relative position of all elements of footprint are set in footprint definition.
For me typically only one reference point per footprint is enough. For holes and LEDs it is their center. For SMD USB connector I like to set where the PCB edge under connector is expected to be. For terminal blocks I set reference at the pin 1 screw center rather than at pin 1 pad center (there is some offset sometimes). That helps to align it to holes in the case.
To make positioning easier I am working around absolute 0,0 position (after editing frame to have no frame). In most my PCBs it is in their center so if I have symmetrical holes they got + and - coordinates with the same numeric value.
I decided to work that way when I was investigating the KiCad 4.0.7 before my first use. Now in V7 there are more tools to positioning footprint relatively so may be help of having 0,0 in the center is not so important than those time but I see no reason to change it.
Thank you both! This is super helpful. Multiple good ways of working with this. I’m used to more conventional graphic design tools and I keep tripping over myself with the basics but getting better… Thanks!
