I am new to Kicad (the project I am working on is only my 3rd board). My current project involves designing a custom PCB for use with very small GMR (giant magnetoresistance) sensors, and in my specific case I require a trench (or hole between specific layers) in a 4 layer PCB. The sensors are placed on the back of the PCB (4th layer), while there is also a current trace passing beneath them on the same layer.
I require a trench or hole between the front layer and the 3rd one (such as only the back layer and corresponding insulation layer) remains. From my understanding, my problem will be solved easily If I can define a custom shape blind via (square or rectangular) or NPTH passing between those specific layers but I haven’t been able to find how you can define that in Kicad (in the footprint editor or PCB layout).
Can you guide me through a step by step process on how I would be able to do so?
Thank you in advance.
P.S. Let me know if more details are required.
P.P.S. I am using the latest version of Kicad (5.1.5.)
I am also half guessing to what you want to do.
From what I understand you need custom milling of the PCB, but you want it only between the inner layers? That is: not visible from the outside?
Or does this “trench” start on the top of the PCB and goes to the 3rd layer???
I do not think this is supported by KiCad, I would not know how to do it.
Even if it could be drawn in KiCad, how do you want to manufacture it?
Maybe it is an option for you to make gerbers for 2 separate boards, and then order boards with a 0.8mm thickness and then glue or solder them together, or a PCB with a slot and a separate flex that goes over the hole.
Try to think of ways in which your design can be modified to fit in with regular production methods.
I’ve seen some microwave multilayer pcb with odd cut outs, but never an internal void.
Have you ever done this before? It may be impossible as the prepreg would want to fill a milled out area. It would be highly dependent on the pcb mfgr process and likely big $$$
The impression that I got from the OP is he wants a hole or slot cutting through layer 1, 2, 3, but not 4. I’ve never heard of a board house making non plated blind vias…
I’m wondering if a milling operation with a small end mill would work as a post-process step. Not sure if the board vendor would (want to) do it, or if it should be an in-house modification once the boards are received.
The only technology exists. I have seen it marketed as 2.5d for cases where you do a deph controlled milling from the outside. (One usecase is to reduce the height of a pcb by sinking components into it.)
Cutouts on the inside are used to place copper inserts or heatpipes.
@Compuser101 might want to talk to their manufacturer how they want this communicated. I suspect a drawing of the outline of milled areas on a separate layer.
From memory they are called “blind slots”, they are charged out similar to fancy flex+rigid PCB’s, where they mill certain layers before sandwiching them. done it in the past for a flush sensor array, Contact your board house and see what they can do for you.
If it hasn’t been made clear enough already - you have to communicate with your board manufacturer and use the normal features of KiCad and gerbers. There are no specific tools, standards or communcation mechanism for what you need. Especially the gerber format is so old and generic that if you want to do something special, you have to find out what the manufacturer wants from you and tell informally what you want from them. Then you either use some extra gerber layer and normal text + graphics, or some other means to give specifications to the manufacturer.
Thank you very much for your responses!
In this reply I am going to answer all of your questions as best I can.
For a better explanation for what I would like to do, the hole or groove [(what I called trench)- I think the correct term is “blind slots”] start on the top of the PCB and goes up to the 3rd layer (so it is not located inside the PCB). I haven’t thought about the possibility of making two boards and essentially gluing them together, but I would have to explore if this is practical for my design as it would have to be watertight (in the groove, a microfluidic chamber or channel needs to be built- this would be a separate process done elsewhere).
An extra step involving a depth controlled milling as Rene_Poschl suggested I think would solve my issue.
I would communicate with the manufacturer if this is possible for them.
Thank you for all your answers. I will get back with a detailed update (probably after some time).
You mentioned sinking components onto the PCB. I think this can prove useful for my design.
Do you have some suggestions about how I can define components sinked into the PCB in Kicad?
The link for the utilized sensors:
I will use the bare die model.
Below you have a caption of the backside 3D model of the PCB sensor area. The grooves would be located right in the middle of the GMR sensors begining at the 1st layer and passing through the third layer (so not located inside the PCB). This section of the board is 12mm across, while each sensor has a width of ~1.5mm. So a very fine blind slot would be neccessary. Because I need to maintain the current traces passing through each sensor, the slot cannot be through hole (the design is initial and will be improved).
Due to the complexion of the design, I think it would be more viable to sink the sensors in the PCB. So can anyone guide my on how I would be able able to do that in Kicad?
They explaine you which options do you have (all of them look pretty expensive) but at design time, you’ll need to contact them (or your manufacturer of choice) to ask, which information do they need exactly. Maybe you will need to deliver a Gerber file with the cutouts, maybe a DXF mechanical drawing or something else.
In KiCAD you will need to use keepout areas for the layers that are going to be milled away.
Have you considered to some CNC milling yourself?
Cheap chinese routers which look like they are usable start at around EUR1000. For a bit more you can have a decent German version such as the Sorotec. There are also other manufactureres around the world of comparable stuff.
Prototypes for custom stuff like this are probably relative expensive, and your exact wishes hard to convey to manufacturers.
With a small CNC machine you can build a lot of custom groove prototypes (from the same standard 4-layer board) yourself.
For DIY CNC, hackaday.com has a collection of home built machines.
I’ve built a decent CNC machine myself, and in parts it also probably cost around EUR800. I built it as a hobby, and it’s of much better quality then complete machines of twice that price, but if you count the hours, it’s not worth it. But it’s a hobby for me.
You might need a more powerful tool than KiCad for such a task. KiCad can not place pads on an inside layer which would be required for this. (I fear you will really need to use one of the high end tools like altium)
This is possible using a trick… create a footprint with pads on to or bottom layer and save it; then edit it with a text editor and change the layer to an internal layer.
Here a sample board with a RF coupler designed in In2 internal layer. https://github.com/PeraZver/Microwave-Transmitter Transmitter.kicad_pcb Transmitter.kicad_pcb (511.7 KB)
As a side note the footprint is DRC compliant… I wonder why the footprint editor doesn’t allow to design in internal layers…
As far as i remember there is the question “How should KiCad handle such a footprint on a board without said layer?”
And i doubt the correct way is to have the layer specified in the footprint. I would expect this to be solved by having more placement options than front and back.
Humm Even if the option to move a footprint in internal layers would be a nice feature, in this footprint there are top and inner pads connected and inner geometry pads … so moving the footprint internally is not the right solution for this case.
The footprint uses two layers next to each other. I doubt you want to need to have such a footprint made for every possible layer combination.
I imagine the best option would be to have pads (or copper features generally) on relative layers and then the option to move the whole footprint to the layer pairing that you want during PCB design.
I mean i don’t expect this to happen soon but this solution would i think be the most flexible solution filling the most usecases (would solve ridgit flex construction, 2.5d systems, inlaid parts, and your RF features)
