I was wondering if it is possible to add a rectangular NPTH to a module (footprint). I see I can select that as an option for a NPTH, but there is still a drill size, and it shows up on the drawing. You see them both superimposed, I am not sure what that will mean to a board house. I guess what I want is really a slot that will be cut out with a router or something on the board, but will stay fixed with the part as I move it around.
The reason is to be able to mount and maybe change TO-220 parts on a PCB that is mounted above a heat sink. If you have several parts like this, and they must be in the middle of the board, it is difficult to mount them unless you can get through the board to put the shoulder washer, screw etc. into the part. I can just make the normal circular hole that would be there for a TO-220 much wider- say 8-10mm, but a rectangular hole (with rounded corners) would look a lot better. It might even be wide enough to change out the part through the slot, without having to dismount the entire board. (think of having 10-12 power devices, all with heat sink compound, that have to be unscrewed to get the board off).
A similar issue arises with some high power RF devices that must mount through rectangular holes, with tab or beam type leads. Sometimes the PCB goes on the heat sink first, then the device is placed so that the leads go straight onto microstrip etc. before the device is torqued down.
Hm… I’d not be worried much about it as the special footprint won’t be used all over the place and the bloke who made it is the one who uses it. There are a lot of instances where you have to do workarounds with KiCAD that cause grief if one is not careful
Just draw a closed loop (any combination of lines and arcs, as long as they form a continuous loop) on the Edge Cuts layer and it will be treated as a cutout. Since KiCad does not perform appropriate bounds checks you must make sure that the loop doesn’t overlap the board edges or as madworm wrote you’ll get into trouble.
Other issues to be careful with:
a. overlapping holes (since as I already said there are no appropriate bounds/geometry checks)
b. multiple bodies: if you have 2 or more non-intersecting loops on the edge cuts layer and these are not surrounded by one big loop (the board outline) then you will have multiple bodies which will lead to numerous problems later.
c. nesting more than 1 level: if for example you have a square (board outline) and in that you have a square which contains another square, what happens next is anyone’s guess (once again the problem of non-existent geometry checks)
d. If you forget to put a board outline and have only a single loop which was intended to be your cutout, it will be treated as the board outline.
Quite a few of the problems could be fixed by bringing in some geometry code and by having a board outline layer as well as a cutouts layer; at the moment all cutouts and the board outline go in the same layer - this scheme means we can not support multiple-bodied boards. Also, on the fabrication side, if a manufacturer prefers the cutouts separate from the board outline we have no way of separating them in our production files.
I have gone with a big (8mm) hole for now. I may go back and add to the edge cuts later, I just need to be careful I don’t route anything through that area! Thanks for the hints.
I am still trying this, I hope someone with more experience can give me some guidance. It falls somewhere between my understanding of Kicad and of how PCBs are made! The attached screen shot shows (I hope) what I am trying to achieve.
I did my layout with a TO-220 with a big hole (8mm) (this is like Q2). But I still have my doubts about assembling the board and power transistors onto the heat sink. So I created a footprint with no hole, and added a rectangular edge cut where I want the part to be. This is Q1. Is this going to cause a problem for a PCB house? The cut-out is shown with sharp corners- how is the cut-out done? Do I need to specify a radius, such as for a router bit? I realize this is going to increase the cost of my board, but the alternatives are also ugly- having the components all in the clear, and then long traces to where they need to go. Could even necessitate splitting into multiple PCBs. I am trying to keep lead inductance and resistance low by putting the parts where they need to go.
A couple of other things- my silk screen shows up as white (except when I move the part, when it is the normal blue color). Is Kicad showing it as another layer- maybe “Dwgs.User” or something- if so why?
I would like to copy my cut-out as a group, but it seems I can only grab each individual line. Any way to move it all at the same time?
Some board houses use a 2.54mm router bit (e.g. oshpark), others 1mm or 0.8mm. That will determine the radius of the cutout’s corners. Unless you want to add a huge safety margin there, I suggest you ask for that number.
You can specify a radius (draw arcs), but it only is worth the effort if it is larger than the actual routing bit. If you don’t specify anything, the fab will usually route to the center of the line and you’ll get a corner radius corresponding to the bit in use.
Your best bet for moving your cutout would be using the openGL mode.
You can put your cutouts onto something like Eco1.User or Dwgs.User and plot those as well, then just rename the file if needed for the manufacturer and you’re done… under the hood the gerber output files look all the same except for the drill file.
So far I didn’t had problems with multiboard cutouts/subdivisions/panelizations in a single file.
In the pic up there your silkscreen looks normal… are you referring to the values/references of the components?
They look ‘invisible’ to me…
Clean the mouse pointer from any tool selection, then draw a selection rectangle over everything you want to move… in the upcoming dialog deselect everything except ‘Include board outline layer’… then move this ‘group’ where you want it
Done by ELECROW without troubles, DIRTYPCBS board house had repeated troubles reading the outline/cutouts and in the end I canceled it (after 3 rejects they did try to do it manually by going with my files to the boardhouse, but I needed the parts sooner - was already late) and sucked up the higher cost for panelizing with ELECROW.
I eventually used edge cuts, created one by one, and the Gerbers were eventually accepted by Seeedstudio, They are nowhere that complex, just simple rectangles. From what I see, the boards will be along in a week or two, and I will see how they did!
