I want to duplicate one design on one board < 100x100 mm. I used pcbnew in standalone mode and did an Append Board, then drew the v-cut line on the Edge Cuts layer, and also lines on the silkscreens for good measure. DRC complained that the boundary wasn’t a polygon but I ignore that. 3D viewer was confused, couldn’t figure out the boundary but I can live with that since I view the single board version.
I want to retain the rounded corners, so the v-cut joins the ends of quarter circles in the centre, see picture and Gerber files. Is this accepted as edge to edge? Will this be a problem for manufacture? Should I extend the v-cut line to the original boundary of the board?
The milling tool will not give a sharp inner corner at the start and end of the V-cut. You will want to separate the boards 2 mm (or really the width of the milling bit), and have two V-cuts, one for each board.
Also, be advised that a V-cut does not give the clean edge that a milled edge provides. Therefore, the two long edges of each board will be different.
For your use case, you might prefer mouse bites that are filed or sanded down later in production.
I’ve done breaktabs and mouse bites before and they are fine. The problem is some fabs charge extra for these but will do V-cuts for free. I’m not concerned about the appearance of the board; it could be hidden by the housing. This is hobby project anyway.
Ok, so if I can obsess a bit over the numbers… A search shows that bit angles can be from 60° to 90°. So if I take the 90° figure, then the depth of the cut is 1/3 board thickness, and the width of the cut will be twice or 2/3 board thickness. For a 1.6 mm board this will be 1.06 mm. So I’ll put a 1.27 mm separation between the two halves since this is easy to align to. See how that goes.
I suppose using milling bits with 90° you can do what you designed between these PCBs but operating the bit not perpendicular to PCB but along PCB. I don’t suppose PCB manufacturers are prepared to do that. I think you should have rounded that two corners near each v-cut line end. The radius you use will determine the biggest milling bit can be used for these (my PCB manufacturer prefers to use 2mm diameter bit).
From my point of view. These PCBs can’t be just v-cuted as they have rounded corners. So milling is needed. If so there should be no problem with extra milling between two PCBs.
My PCB manufacturer charges per project and per dm². So here the price would be the same if I order two PCBs or one 2 times bigger.
I think you must contact your board manufacturer. I believe most of them won’t make that kind of board. V-cut requires a whole panel and cutting though it, they have minimum length for v-cut and it must go through the whole panel.
I just can’t see no sense in what you are doing. Are you going to panelize this construction or let the manufacturer panelize? In any case, why put the v-cut in edge.cut layer? Let the edge.cut be a closed line as it should be and draw the suggested v-cut in another layer, giving note to the manufacturer.
The outline is cut with a router with a milling bit that is often 2 mm diameter.
The V-Cut is cut with another router bit that has has a V as a tip. The routing does not in principle need to go from edge to edge. But to actually split the board after soldering (using a rotary V-cut knife), the V-cut needs to be edge to edge in a straight line to do this.
I have had boards panelized where the V-cut does not go from edge to edge until some boards have been split off, so there is a definite order between the different V-cuts. This must be negotiated with the manufacturer.
Also (again), in gerber X2 there is actually a way to have a specific file for VCut. I have a Python script that does the panelization and draws VScore in the layer Eco1_User. At gerber export the script also exports that layer but then proceeds to change the gerber file to VCut according to the gerber X2 spec. I suppose one could just change the FileFunction line in the gerber file with a text editor, but scripting does it right every time. My fab accepted this without question. The relevant code is
##### Generate gerbers for Vcut
pctl.OpenPlotfile("Vcut", pcbnew.PLOT_FORMAT_GERBER, "Vcut")
# Change Eco1.User to Vcut inside Gerber X2 file, see
with open(pctl.GetPlotFileName(), "r+") as f:
for i,line in enumerate(contents):
Ah, ok. So if I provide a 2 mm separation and draw the V-cut down the middle of that this means that the V-cut edge will protrude by ~0.5 mm from the original edge of the sub-board, according to my calculations. I know the fabs can do 2 mm slots from doing breaktabs and mouse bites.
I’ll put the V-cut info in the layer the fab says to.
I think we are speaking about different things.
I understood that 90° milling bit is flat at its top. I don’t know the nomenclature used with milling bits.
I think not. That is what I said - they are not prepared to do that.
But you designed those ‘negative’ corners with 90° sharp angle that I suppose you assume to use milling bit with flat top to do them. So I understood that you assume to run milling bit not perpendicular to the surface.
I am speaking about milling and not V-scoring. I have never seen how v-scoring is done but I suppose that they have two rotating discs and PCB goes between them through its all length. So I don’t know what you mean saying ‘V scoring bit’.
It is what I said “So milling is needed.” When searched in dictionary the word I found mill. The router seams to be the same.
But how that ‘negative’ corners are cut. It is what I was telling about.
No, I don’t expect them to produce the “negative corners”. I don’t think they expect that I expect them to. And I don’t expect that they will expect me to expect them to do it. I know they will come out rounded from my experience with breaktabs.
But maybe I’ll draw a semicircle there so that nobody has any undue expectations.
The v-cut is made with a tool which carves a groove in the board, it’s shaped like V, so the groove has width, typicall 0.5mm or something like that. You have to take that into consideration when deciding the space between the middle of the edge.cut line and the copper or other features of the board. You have to leave half of the width of the groove + tolerance. (EDIT: there are no standards for this, you should always find out what your manufacturer does.)
If you panelize so that you put two boards apart from each other, i.e. try to leave more space in panel instead of in the single board, the final physical edge of your board will be wider than the intented board width because the v-cut doesn’t actually remove any board material through the panel.
If you want to have e.g. exactly 50mm wide board (within tolerances), measured with a caliper, you have to make the width between the middles of the two edge.cut lines 50mm, not wider. But you have to leave enough room for the cut in the surface of the board because the usable surface width is something like 49mm.
The cross-section of the board, both sides with v-cut, will be like < >. So it depends on whether you want to use the farthest edge of the board or the the edge of the v-cut on the surface.
I think most manufactures give instructions to leave more room in the design of one board for the cut, and then panelize just side by side. (EDIT: there are no standards for this, you should always find out what your manufacturer does.)
I always expect things are done according to my project. If not possible, or especially difficult I expect be told of problem and not just to modify my project.
But I have never checked it by sending project not possible to be done.