To try if the routing was doable, I have transfered the coordinate of the components of the panel from illustrator to kicad, with the help of taking one encoder and every smd led + led pipe and copy paste them with offset, with the snap functionality of kicad, I first placed the encoder with coordinates then snaped the whole ring (smd led + led pipe), so I did not had to enter each coordinate from illustrator for every components.
Now, I made a schematics, and I want to know what would be the best practice to avoid the time consuming task of replacing every components placed with the correct footprint and copy paste each coordinates from illustrator.
From what I see, I can’t copy paste a whole bloc of footprint because they will be unlinked.
How would you proceed to do import from schematics to a board that already have component placed ?
Looks like you’re rowing uphill through a dried up riverbed and enjoying it for all the exercise it gives you.
A project of this size is a very bad choice for learning KiCad. The reason is that there are a lot of different ways to do things in KiCad, and some of those ways are huge time sinks. KiCad works quite well with a “forward” workflow, but a backward workflow is very limited. If you make mistakes in a project of this size, mistakes you make also get multiplied by the amount of footprints you have.
The quickest way to fix this is:
Start by deleting all the LED’s except for one LED ring (Yes really delete them)
I assume you you also have placed 17 rotary encoders and all those leds in the schematic. Delete them too, except for one encoder + led ring.
Put the encoder + LED ring on a hierarchical sheet.
Make as many references to that sheet as you need in a hierarchical schematic.
Manually match the RefDes of all the encoder schematic symbols to the encoders on the PCB.
Manually match the RefDes of the symbols of one LED ring with the footprints of the single LED ring you left.
Update the PCB.
Run the Replicate Layout plugin.
The Replicate Layout plugin is a wonderful tool for projects like this in KiCad. But you do need some practice before you can use it effectively. It is probably better if you first experiment here with a few dummy projects, or at least make sure you have backups of the real project. But experimenting with a smaller project is better, as it lets you concentrate more on the workflow. The Replicate Layout plugin can also be used to replicate the track layout of all those tracks for the LED’s.
And once you’ve created the PCB, you can export it to Blender in a few minutes. So either rowing uphill or downhill, once you get there you have done almost everything twice.
But I do admit, your Blender Renders look nice
On a sidenote, are you aware that similar LED rings with more LED’s for higher resolution are available commercially? Unfortunately, they are relatively expensive, but I’ve also seen a project on Hackaday of a recreation with regular small LED’s and a 3D printed frame to reduce light bleeding.
In this case there is no easy way, since you don’t have any reference designators. IN reality if you would just get on with the program youd be done in 20 minutes, if you started from scratch. Yeah, i too vote on deleting all but one led ring
However, why do you need kicad in the first place? Your not using any of its features. All you really need is to export the results into gerbers for manufacturing you could mostly do this in illustrator if you wished all you need a a pdf to gerber converter.
PS: you can draw crosses in illustrator and export a dxf and import that so you dont have to type values for positions.
PPS: Consider which software houses your master model, then script that application to spit out a kicad file
All those LED’s are going to need quite some amount of tracks to connect to those “multiplexer IC’s” (whatever they are) and the arduino board. And that is enough to want to make a normal KiCad project out of this.
Yes and no. Sure if you are doing documentation based workflow then yes. But I am more generally pointing out that if one is not going to bother using the software at all as intended then why use it at all. The workflow makes an assumption that all the traces would fit into the layout. This is not at all a given thing.
Yes, it would be beneficial to have this in kicad, no placing the damn things again is not all that much work. especially since 15 of them are just an array. Besides one may need to do massaging of component placement anyway, design is iteration after all.
PS: THis one would definitely benefit from the kicad nightly as it now has the shap to intersections tool
