Is there any way, to draw a component in low relief? The goals is to build an socket to solder(or help) smd components, and if possible avoid solder it. Is for 72-QFN components and 128/144 tqfp . As an aside and for another case (the case of wanting to make an adapter for the three sockets, for dip(example, qfn/128tqfp/144 tqfp for dip)) preferably all in the same position.
Hi, I’m afraid I don’t understand the question, could you provide more info as to what Kicad is or is not doing please ?
In a general sense, ‘Relief’ is an Inset (a pocket at different depth than the surrounding surface). This is not possible in Kicad (though, could put hole/shape in the Mask layer).
But, OP may have a different concept of ‘Relief’…
Indeed, I can think of a form of ‘Relief’ I would not choose to discuss here.
I was referring exactly to what you wrote. But to BE more clear i want to do it using diferente layer
The only choice is between Top/Bottom or both layers.
You can set the Mask thickness in the Board-Setup. BUT!! just because you can set it does not make it ‘doable’ for a PCB supplier…
Default Mask thickness is 0.01mm. You could ask your supplier if they can Mill a pocket to specific depth and get out your checkbook…
Can also make a Jig as an Aid for placing it…
This is called z-axis milling (as search phrase for google) and not natively supported from kicad. This is also a non-standard feature for pcb-manufacturing and therefore different pcb manufacturers could have different approaches/requirements for this task. So contact your pcb manufacturer (or look on their website for a description).
For example my standard pcb manufacturer wants a separate drawing on a separate layer for the z-axis milling. The drawing should should show the exact milling contour (drawn with 1mil linewidth) and include a textual description of the milling depth. In kicad this drawing could be made for instance on the USER1…USER9 layer and exported as gerber file together with the standard layers.
1 Like
It’s not directly supported by KiCad. Currently KiCad is limited to a single Edge.Cuts layer, and this is used as the size for all layers. This also means that Rigid/flex or semi-flexible PCB’s are not supported.
I am also not sure whether definitions for this is Gerber files (I have not checked). KiCad is also getting some support for other fabrication output formats though.
If you want to attempt it anyway, some hints:
In KiCad’s footprint editor, SMT pads are only placed on the outer layers, but it is possible to edit the footprints in a text editor and place the pads on an internal layer, and then the pads stay on that internal layer (or at least, they did a few KiCad versions ago).
For the depth milling layer, you can draw graphics on one of the user layers, similar to now Edge.Cuts is used, but you will have to communicate with your PCB manufacturer.
Another option you could try is to make two thinner PCB’s, and find a way to combine them together in some way. For example, you can use THT pads in the same locations for both PCB’s to solder them together. But this is all highly experimental, I have never done this myself.
I like this aproach.
If you have a Mill or know someone/Fab-house willing to do it, make a Drawing as suggested (and/or a 3D-Model/Step file for them to use…)
You could further your effort by loading the PCB in FreeCAD with StepUp-workbench then, create a Body (actually several other ways to do it) and make a Pocket.
Example - see the light blue pocket
Thays my goal. Build an pocket with right shape and dizer as The component
Whats the easiest way to draw The Holes (on this layer)? From the original footprint or symbol?
I would put any non standard layer in Kicad on a user layer, and instruct the fab house what to do with the layer.
You’d need to do this anyway for any package. In Altium I might do some wierd sh1t on MECH8 layer and then on the PCB gerbers on all layers but not within the board region, I will have instructions for the fab like
“MECH8 : Z axis mill -1mm”
“MECH6 : Tab route”
“MECH5 : board outline route”
This way it is completely obvious the the shop floor that there are extra instructions, even if sales didnt hand it down correctly to mfr.
If you need something like this, you will need to be having a conversation with the fab house, it cannot just be a tick boxes and upload the file and wait " sort of purchase.
You can accomplish your task with various steps/approches and making pretty pictures is irrelevant to making the PCB. Though, good images can help a Fab-House understand in conjuntion with Drawings/sketch.
That said, and mostly for Pretty Picture… and to answer your question about Drawing…
There is plenty of info on this forum about drawing and many of the posts include using FreeCAD and StepUp - homework is your task(s).
The screenshot below shows:
• Red-Lines on Edge.Cuts layer
• Blue-Lines on F.Silk layer
• Grey-Lines on User.Drawings layer
This screenshot shows the PCB loaded into FreeCAD (from StepUp)
And, my manipulations/work and results
Your next Task is to try and duplicate what I did by Trial and Error
I will hint at having partially Plugged/Filled the Circular Hole by using it’s bottom-edge for Extruding (Padding)…
The User.Drawings layer was Exported by Kicad as DXF and imported into FreeCAD - it self-named as Junk_Test_User_Drawings.
To make it usable, I used the Shape-Builder tool>Face_From_Edges and Drag&Dropped into the Body…
It may take you some time and frustration but, you’ll learn to use these tools…
I did Not re-color anything…etc
1 Like
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.