The 3D viewer does not work properly with pads composed of multiple geometric shapes.
It’s his preview:
Does anyone else encounter the same error?
It’s his preview:
Does anyone else encounter the same error?
I don’t know what I’m looking at from a simple screenshot.
Have you combined the pads with the (presumably) graphic shapes with the pad edit mode?
Can you create a simple test project that uses this footprint and post it here?
That allow us to look at this footprint and troubles with it in KiCad itself, and this makes analysis much easier.
Please post your KiCad version and OS details too
Also in addition, just to be clear. What do you perceive to be the problem? Is it the C like and the two dots in the pads? Or something with those blue areas around the pads? (What are those?)
Here is the file with the fingerprint in question. As reported in the file, the same pad in question copied from another pcbnew window is displayed correctly.
a.kicad_pcb (33.0 KB)
KiCad 8.0.4
Windows 11
Generating Gerbers creates the same D-codes for the left side pads. (Different D-codes for different rotations, so the copper layer is OK.)
A bit later, the problem is with the solder mask layer. It displays (probably) normal in the PCB editor, but has the C and extra dots in the 3D viewer.
These are quite weird pads. Pulling one apart in the footprint editor with the pad edit mode shows an SMT pad, two filled rectangles and two lines for each pad.
On the PCB, solder mask expansion is used for this footprint.
If I set this from -0.06mm to 0mm then the artifacts in the 3D viewer are gone.
Solder mask expansion does look all right both on the PCB and in the gerber viewer, so this seems to be a drawing artifact that only shows in the 3D viewer.
I think this can be classified as a bug, but overall I’m more surprised that solder mask expansion works at all with such a weird pad like this. A workaround can be to disable the soldermask altogether for the pads in this footprint, and then use aperture pads for the solder mask layer. You can also use the same aperture pad for the solder stencil, as I suspect that there probably will be too much solder on these pads.
I guess that this solder mask expansion was an attempt to reduce the amount of solder paste on the pad, and not the solder mask (solder resist) layer. Is this correct?
Yes, it only occurs with the KiCad 3D viewer, the production files are correct. Regardless of the shape, the viewer should still display them correctly, should we open a bug report on gitlab?
The strange shape is my modification to facilitate soldering when not using the stencil to apply the paste. The bottleneck creates a small capillary force that pushes the IC into the correct position.
I always apply a negative solder mask, don’t you?
Yes, probably worth a bug report. The PCB editor, artwork output and 3D viewer should generate the same layers.
No, but I make far less PCB’s then my presence on this forum may suggest. A big part of my KiCad knowledge is from figuring out details of how things work for answering questions on this forum. In general SMD (Solder Mask Defined) pads are not the default an NSMD (Non -SMD) is prefered. I think SMD is mostly used for BGA’s and other high density board when it is the only option to keep adjacent tracks covered by solder mask. You can search a bit for those abbreviations for more background info.
By far the most used (by hobbyists / beginners, which is the biggest chunk of forum users here) is to use no solder mask expansion at all. Pad having the same size as the soldermask is a very bad practice in itself, because there will always be some (and varying) misalignment between copper and soldermask, and with no clearance, the exposed amount of solderable copper will also vary. Best I know however, PCB manufacturers use this as an implicit freecard to use whatever solder mask expansion which is needed for their production process. It’s a bit shady because you do not get what you order, but it also avoids problems with misalignment, and thus improves the PCB you get. So it cuts both ways.
Solder mask expansion settings also depends on the tolerances with which a PCB is being manufactured, so it makes sense to leave this setting for the PCB manufacturer to decide.
At first I thought your footprint was to accommodate two footprint sizes, but I can understand it for hand soldering too. Is this QFP or QFN? I don’t have problems with hand soldering QFP, I have not done QFN and am a bit apprehensive of it.
Another workaround for you that probably works is to combine the SMT pad with a single graphical polygon. A graphical polygon also has a line width you can set in it’s properties, and with that you can make the rounded corners.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.