I want to have a V-scored snapable edge on my pcb with signals across to test in factory, the pcb is a 4 layer pcb. In which layer shall I put the connections? Which layer should have the V-Scoring line? I thought of mouse bits first, but those usually require some keepout so I guess is not an option for routing signals or is it ?. What is the best way to do it in KiCAD ?
V-score lines are usually put in the edge cuts layer, same as the outline, but check with the factory. They must be edge to edge. Be aware that after you have added a V-score, the 3D previewer will complain about not finding a closed outline.
Does it matter which copper layer you will put the traces to be broken on? Won’t it be separated already at the score? You cannot guarantee that the V cutter will or will not reach the inner layers.
It can be whatever layer as long as it doesn’t get destroyed in the V-Scoring process.
Are you sure about this:
If you put the V-scores on Edge.Cuts have to be removed from Edge.Cuts before that layer can be used for it’s intended purpose.
PCB manufacturers may accept this, but I’m guessing this is an extra complication.
You are probably better of with putting the V-scores on a separate layer and include a text note that this layer is for the V-scores.
Some time ago I had a look at the latest Gerber standard from Ucamco and this has a special layer in which V-scores can and should be defined, but as far as I know this is not used much. KiCad also does not have direct support for this.
But in the end this does not matter much.
I had a look at a number of Chinese breakout boards and the V-scoring is quite deep. It reaches over half the thickness of the PCB and is done on both sides, so it probably cuts through all 4 layers of your PCB.
Routing in between mousebites does work. Routing over the mousebites (If you use plated holes for them) probably also works. If you use the outer layers, then there is a chance that you peel the tracks off from the PCB when you break them apart. You can prevent this by placing vias through the tracks near to the mousebites. The tracks will then not peel off beyond those vias.
Another option is to use neither V-scoring nor mousebites, but just leave short sections of PCB intact, and then use a PCB de-paneling tool:
The picture above is from the simplest hand-held tool, more “professional” pneumatic tools also exist. Some are mounted on a table, etc. For some pictures:
Yet another option is to buy a small CNC router, and use that to separate your PCB’s from each other.
these are not “clean” processes. If you put the tracks too close together there is a chance that your test tracks may get shorted during separation of your PCB. With mousebites (and extra via’s) small sections of tracks may peel of and break in unexpected places, and those loose hanging parts may create shorts. With routing, copper is a soft material, and copper chips may get embedded into the side of the PCB and “smeared out” a bit, and for this reason using castellated holes are relatively expensive, because it takes extra work to prevent or remove such shorts.
A lot of Chinese manufacturers specify the Edge Cut layer for V-scores, but it’s always good to check with them.
JLCPCB: This is what a user reported: V-cut and rounded corners
PCBWAY: I can’t find a page saying that but I had a panel of breakout boards for TSSOP/SSOP chips made and they said to use the Edge Cuts layer.
Ocean Smile, formerly LocoPCB: https://hackaday.io/page/6724-a-review-of-ocean-smile-formerly-locopcb-pcb-service also Edge Cuts layer.
They may charge extra so one should always check.
I have not done this myself, I’m mostly repeating things and Ideas I’ve read.
It’s hard to predict what your via’s will do when the mousebites break. I would not be surprised if they get partly ripped out of the PCB and loose parts may cause shorts with other parts. Making the part of the track that has to stay on the PCB the same width as a via may help with keeping them on the PCB.
I’m assuming the final goal is to save on testing or programming time during larger production runs, and reliability is an important issue for that.
It may be a good idea to design a small test panel which has different sorts of mouse bites, and then simply try what works best, or use the first iterations of prototypes or small production runs to try what works best.
So better like this ? Signals still go in the inner layers to avoid peeling off. I have doubled the tracks for getting more current. and there are no different signals onto each other for avoiding possible shorts ?
Yellow and pink. Are those inner layers?
That would prevent them from peeling off.
I’m guessing the holes are a bit small, but at the same time I do not know why I think such a thing. It is a compromise between the ease of separating the PCB’s and the strength of the panel.
SMT resistors and capacitors are made of ceramic material and are very brittle. They may break if they are in an area with high bending forces. There are some guidelines about the distances for these from V-scoring and mouse bites. They also break much easier when bent over the long axis, compared with the short axis.
I would think they should be a drill drawing line, describing where to do the cutting. Otherwise you don’t have a poligon board.
also certainly it’s good practice to pull back the copper pour from the score.
The instructions I were given were to put the V-cut lines in the Edge Cuts layer. The semantics don’t collide as it is possible to tell which is which. Too bad about the 3D viewer, perhaps it could be taught how to distinguish them. BTW the machine is a V-cutter, not a drill. You can see illustrations here: https://www.pcbway.com/blog/PCB_Design_Layout/The_depth_and_width_of_the_v_cuts_grooves.html and here’s a 16 second video showing a machine in operation: https://www.youtube.com/watch?v=cs2lWyH84Nw
I used the gerber X2 Vcut spec to order from a manufacturer here in Sweden. (Yes, not a cheap Chinese place.) The script I use to panelize and output gerbers uses the Eco1.User layer to hold the Vcut lines and then changes that after producing gerbers like so:
# Change Eco1.User to Vcut inside Gerber X2 file, see # https://www.ucamco.com/files/downloads/file/81/the_gerber_file_format_specification.pdf with open(pctl.GetPlotFileName(), "r+") as f: contents=f.readlines() for i,line in enumerate(contents): if line=="%TF.FileFunction,Other,ECO1*%\n": contents[i]="%TF.FileFunction,Vcut*%\n" f.seek(0) f.truncate() f.write("".join(contents))
What’s the name of the swedish manufacturer? is it based in Skåne ?
Hejdu, de heter MULTI-TEKNIK mönsterkort AB
Ah yes, I know them. Tack så mycket!