Hi, so I am having an issue with using the create circular array tool, I have looked at other posts and researched online but still couldnt figure it out.
My issue is that I have 28 SMD LEDs in my schematic that I want to use the circular array tool to put them in a 22mm radius circle. I can make a circle of the right size and amount of LEDs but instead of repositioning my existing LEDs it generates new LEDs which means that 1.) there is too many LEDs in the schematic 2.) if I delete the LEDs original LEDs (not in a circle) then the rats nest isnt correct on the new generated LEDs, even if I go through and change the designators to match the schematic.
So my question is how from an existing schematic containing 28 LEDs, that in the PCB layout will position the LEDs correctly and with the correct rats nest.
Any help with this would be great, I have been banging my head on this for hours,
Never used any array tool but if it adds new LEDs than my idea is to:
- delete your LEDs,
- use array so you get LEDs with the ref numbers like you have at schematic,
- update PCB from schematic (not sure that function name) but according to references and not default time based (hidden) IDs.
I’ve been experimenting a bit in the last 10 minutes. It’s something I also never properly understood, but I got it to work with the following procedure:
- Draw schematic, with LED’s (no footprint assignment needed yet).
- PCB editor / Drill/Place File Origin and put it in the center of the circle.
- a to add a led with the footprint you want and place anywhere on the PCB.
- Edit properties of the LED:
- Set RefDes to D1 (or whatever your led’s start with)
- Set Postition to X: 22mm and Y: 0mm.
- Set other parameters…
- Create the array [Ctrl + t] and set:
- Horizontal and vertical center to 0 (Which is apparently relative to it’s current position).
- Radius is now set to 22 (Because of step 4.).
- Set Count for number of LED’s.
- Assign unique RefDes.
- You have now drawn a circular array of (not yet connected) LED’s.
- PCB Editor / Tools / Update Schematic from PCB
- Make sure the Re-link footprints to schematic symbols option is on:
And last, select a few LED’s on either the PCB or the schematic. KiCad’s cross probing function will see the associations between the symbols and the footprints.
Great thank you so much for this, it worked great. I can’t help but feel like this feature should be made more user friendly, such as being able to highlight all of your LEDs in the PCB layout and then reposition the existing LEDs would make this much easier.
But anyway, thanks a bunch.
For the next time, there is a new feature on this forum. At the bottom of each post there is a checkbox to mark a post as the solution, and marking it will help others findingen the solution quicker.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.