When will the flex PCB be supported in KiCAD,
1 Like
What sort of extra support from KiCad do you think you need for a flex PCB?
Hi, I have done the design for the flex pcb, and a sample has been manufactured.
Current KiCAD can support flex PCB very well, there is no difference between FR-4 PCB and flex PCB in KiCAD side. Maybe you need to have some more information on the PCB drawing to explain what do you want before you deliver your manufacture file to PCB/PCBA supplier.
2 Likes
Pure flexi works fine now.
It is flexi-rigids that KiCad cannot deal with properly
What is KiCad lacking that you need for rigid-flex boards? Iāve designed one such board in KiCad without the assembly house and pcb manufacturer complaining.
Could you upload example files (gerber or pdf) which is not possible to create in KiCad?
Only thing I can think of is that the 3D viewer and step export wonāt be 100% accurate. But there are probably a few more functions that would be nice to have when designing those boards.
2 Likes
Some discussion here:
Stiffeners are one need
Stiffeners can easily be drawn in any general purpose layer, of which there are plenty to choose from in pcbnew.
That thread didnāt clarify what must be added to Pcbnew for rigid-flex. If anything it clarified that itās absolutely possible to create rigid-flex pcbs.
Zebonaut wrote:
A flexible PCB is just a one- or two-layer device with a different material specification (polyimide instead of some sort of FR4). The Gerber files are no different.
Flex-rigid-combinations are similar: Youāll give them a pretty regular Gerber stack, as with rigid PCBs.
In addition, you send them a specification for the layer stack and tell them which layers are to be fabricated on polyimide. Flex in the middle or your stack? Flex on an outside layer? An additional Gerber layer with the dimensions for the entire PCB and the parts that are flexible might help.
With that said, Iām sure that there are functions which could prove useful if implemented. Iām just not sure what those functions are?
I donāt think that there is a standard on how rigid-flex pcbs are defined/represented in standard gerber files? Maybe thereās something added to the X2 Gerber format?
In altium designer, it supports flex-rigi board like this:
1.Define the soft part of the pcb
2.Define bending place and bending radius
3.Display the bended board on 3D view, and the bending angle can be adjusted.
4.Export the bending process as a movie
6.Export bended pcb in a 3D file.
I donāt think KiCAD needs those features at all, because KiCAD has a lot of important features which needs to be achieved, and these features are not important.
1 Like
Thatās sounds really cool! 
But I do agree, thatās nothing that I need in order to design flex-rigid boards. āDefiningā the soft parts and hard parts in a comments/graphic layer has proven sufficient so far.
I just had a short look through:
The Gerber file format does have some extra capabilities that are not supported by KiCad. For example there is a V-cut layer, while more common practice is to try to communictate this to a PCB manufacturer by some other method.
There also is a āpeelablemaskā layer. I think this should be used for thinks like masking off gold plated edge connectors if wave soldering is used (and similar purposes).
For simple flex PCBās there is not much need for anything special needed for KiCad. The only real change is that the PCB manufacturer does not use FR4, but some flexible substrate.
Ridgit / Flex is a different story. These do not have a āsimple outlineā. some parts of the PCB have more layers then other, and if footprints can be placed on both the ridgit and the flex part, then the footprints (and their pads) must therefore be defined on different copper layers. KiCad does not support this (yet). KiCad can only place footprints on the two outer copper layers.
KiCad has been steadily improving over the last bunch of years.
When I started with KiCad, it had some serious flaws, such as library management not working properly, but those have all been solved some years ago. Plenty of new features are getting added, and old features are improved. The development pace of KiCad is also improving.
If you want some new feature in Kicad you can always generate a feature request on Gitlab. There is no guarantee of such a request getting implemented of course. It all depends on how useful the request is, if it fits within KiCadās philosophy, how useful it is for others who use KiCad and probably a bunch of other factors.
Sure, thatās a real example of one thing that cannot be done as of now. But that to me seems extremely special. Why in the world would anyone want to do that? If you are already paying for a flex-rigid (part flex, part FR4) board, why would you place components on the flex? With or without a stiffener, I donāt see a reason for that. Itās much better to place the components on the FR-4 part, and you will pay for FR-4 for the entire area of the pcb regardless.
Also, if you would place the flex on the top layer instead of in the middle, this should be possible. The component layer is then the same regardless if the components are placed on FR-4 or on flex. Although Iām not sure if thatās a manufacturable option. In your example where the flex is placed in the middle of the FR-4 stack, the components will be placed on different height depending on if they are placed on FR-4 or flex. How will the paste stencil for this look? It would be the most stepped stencil Iāve ever heard of. 
Regarding the outline of a flex-rigid pcb: What Iāve done is to draw a conventional outline in the Edge cuts layer, which shows the outline of the complete pcb. Iāve then drawn the outline of the FR-4 parts on a different layer and clearly marked which is which in the gerbers.
Several flexi-rigids that I have used have had a THT FR4 end with SMD capacitors, soldered onto a circular connector.
The other end was either gold flashed to plug into a cam lock socket or soldered to a THT plug
all these processes could be done in FreeCAD
here some experiments:
3 Likes
thanks, itās very cool.
I have successfully made flex PCBs with KiCad. The main thing that is missing for me is the ability to easily do curved traces which are recommended instead of the usual 45 degree bends.
Curved copper tracks are supported by the new, almost ready KiCad V6.0. Support is still a bit limited though, and there are not yet many build in ways to draw and manipulate them.
I know itās an open request. I have been following this for a while.
would anyone whoās done a rigid-flex board be willing to share some of the drawings they used to define the board, stackup, flex portion, etc.
I know (now) that V6 has many more user layers than V5 did, but what extra layers did you use to do dimensions, bends, etc.?
1 Like