I’m a new user of KiCad, I have done a very simple schematic, 2 layers, a few components.
The board in Layout is very little e simple. I would like replicate the same board in a pannel of 10 board for example. How can do that? some suggestions? thank you very much.
Hi @sarmassi, welcome to the forum!
You can open PCBNEW in standalone mode and then File > Append Board (or something along these lines).
You can then use Move Exactly (while the whole board is selected) to create your panel. Not sure if Create Array works with this (but I expect it does).
There is no real support for making panels in KiCad.
There are some people who do so anyway, and add things as mousebites, strips on the sides and extra routing to put multiple instances of a PCB on a panel, but this has some limitations.
For example. Nets get merged because the net names are the same. There are multiple footprints with the same RefDes, so DRC does not work and there may be more problems.
It is also quite a lot of post processing on a PCB to turn it into a panel, and if anything is changed on the PCB itself, there is no easy way to update the panel with this new revision.
Besides the information and software you will find from the links provided, a couple of things you might want to note:
If you panelise then you also have to consider how to break up into individual boards. Aside from sawing (highly not recommended, hard work and dust not good for you), this might entail a further charge by the factory for V-cuts or slots and mousebites.
Many factories will combine shipping on multiple orders so you can amortise that cost, which usually dominates the per board cost. This might make putting one design per board more palatable.
I assume you mean that you will populate and solder the boards before breaking them up. Remember that bending the board will stress the components. In a similar vein, PCBA (PCB assembly) factories generally do not accept V-cuts, only slots, with assembly because of the risk of damaging the components when cutting because that step happens after assembly, whereas the slots are done before.
Panels made by CAD are usually problematic in the fabricator CAM, for the netlist issue already mentioned here, more in general because the data is ‘flattened’, and the information that it is a set of identical PCBs is lost. Imagine you would receive the design of a panel with 10 copies of a PCB, and were asked to make changes on the PCB.
If you send the fabricator the individual PCB, and a clear drawing how to panelize it, he may prefer to panelize it himself rather than receive the panelized data. Or maybe not. You can ask him what he prefers.
On top of all this.
The size of the panel can be an important factor.
Just think about a PCB manufacturer having base material of 400x400mm
and you design a panel with dimensions of 205*205mm. In this (extreme) case, almost 3/4 of the base material would be waste, or have to be filled with other projects.
I knew of a company producing very high reliability assemblies for space and armament use. They supposed that even sawing the board to panel web would be an issue. So they used a laser to cut them.
Well the edge of the board was very (too) close to the circuitry and the laser would partially melt the inner layers resulting in intermittent shorts.
I just found it interesting that trying to be ultra conservative resulted in a worse failure mode.
Perhaps of no helpful use but, wanted to mention it…
Much has changed in 20 yrs but, back then I wanted PCB panel’s with Main board and four small ones.
Vendor’s (several of them) said Extra money. I said, ‘how about I define the actual cutting path rather than V-cuts or having you folks doing it?”
They said great. The cost was same price as if one PCB (of same overall size). I added notes on drawing to Ignore DRC errors.
Image below is the PCB as delivered. I cut off the smaller boards with a blade from Hacksaw.
This kind of approach may still work with fab houses. (And, I currently do it on PCB’s that I mill and do the cut path on the Edge-Cut’s layer)