You can use gerbv for gerber previews, much more lightweight.
Right, it was not about the viewbox. The holes were just defined outside any layer.
I moved the holes to the copper layer (id=“nonconn0”) and also added black silkscreen for the visual in Fritzing. From top to bottom: Fritzing, Aisler, GerbV
Can you upload the fzpz file here?
I have another issue with the id=silkscreen. I might need to open a new topic for that.
When I have the id=silkscreen at the bottom, it covers the pads and pins in the part editor, but I’ll look into that some more, or I’ll create a separate topic.
Thanks and regards, Harald!
Sure 
USB_type_C_rund2.fzpz (23.7 KB)
Thank you,
You added the drill holes to the layer id=silkscreen. Is that for better visibility, or does it have an impact on the production process?
gerbv works great, thanks for that too!
Best regards, Harald!
When using your previous file with very thin copper rings, the Fab showed a warning that these would be removed. Which would be correct, but is also irritating.
So, I made acutally made the copper circles (drills)
fill="none" stroke="none" stroke-width="0" id="nonconn0"
This won’t cause any warning about removed copper. The since the circles in the copper are now invisible, the silkscreen is required for display.
The Fab again removes the silkscreen, because its on top of the hole, this time without a warning.
Ah yes, I hadn’t even noticed that the warning was gone.
One last question: if the four mounting holes (connector16pad-connector19pad) for the USB socket are supposed to be on both sides, do I need to insert the same graphic element into the copper1 layer?
They should essentially be implemented as THT so that the socket can also be soldered from the bottom.
Best regards and many thanks!
Harald!
They already are THT, but the FZP file defines no copper0 layer:
<pcbView>
<layers image="pcb/USB_C_molex_217182-0001_round_7cf4663b7fff81789bfe5bdff984885c_5_pcb.svg">
<layer layerId="silkscreen"/>
<layer layerId="copper1"/>
</layers>
</pcbView>
When you add it there, it should work. You might have to remove the other pads from pcb svg copper0 though. Right now, the definiton is ambiguous: Then connector pads in fzp use copper1 only, in the svg the are in copper0 and copper1.
If you add copper0 in the pcbview definition, the ambiguity might be resolved differently.
Our the fzp_checker.py script in Fritzing part should warn about this already.
Great, a final thank you and good night. I’ll do the check tomorrow and add the missing layer then too.
Good evening,
I have now defined the four pads for soldering the connector as THT on both sides and got the component to pass the fzp_checker.py test.
You could now have a test board made. There are no more error messages during the Gerber export and the Gerber preview looks good too.
Ailser has also stopped complaining.
USB-C-molex-217182-0001.fzpz (23.1 KB)
Regards, Harald!
Hi Harald,
that looks really good. I have a good feeling about the dimensions and the fit. I placed the USB socket on a paper printout and it looks great.
Could you check one more thing though: I’m considering ordering a stencil along with the test PCB. Unfortunately I have no experience with stencils — this would be my first time. In the preview on Aisler, the stencil cut-outs (SMD) are shown in light grey. The pads for THT remain dark grey. But for the new USB-C socket, it’s the other way around. Something might not be quite right with the layers there.
Could you please send me the Fritzing file for this? I can take a look and see if I can find the cause in the fzp file or the corresponding svg file, though I can’t say for sure.
Regards, Harald!
Atmega2560.fzz (75.4 KB)
Sure, here’s the complete Fritzing file. Don’t be surprised — the circuit isn’t finished yet and the components have been thrown onto the board randomly.
Good morning,
I took a look at the files. For the processor, there’s no visible difference in the fzp file.
But in the PCB file there are differences — the pad has the following additional values:
stroke:none
stroke-width:0
stroke-linecap:round
Hi @KjellM,
are the above-mentioned pad properties necessary for SMD stencil cut-outs?
Regards, Harald!
I’m currently expanding my circuit. I’m thinking about connecting the housing of the USB-C connector or the shield plate to GND or PE via a decoupling network (capacitor and resistor).
Hence my question: Can one or all 4 outer solder tabs be made “connectable”?
@KjellM
Can you help us with the stencil questions as well?
Hi Ralf,
yes, that’s definitely possible. I’ll take a look at it tomorrow!
Cheers, Harald!
Hi Ralf,
I’ve now connected the mounting pads to GND. To avoid an error message, I’ve also added the missing connections to the schematic and the breadboard. Could you check whether that works?
Unfortunately, not all GND connections are in one bus, but I’ll try to change that.
I would change this fzp code:
<buses>
<bus id="internal1">
<nodeMember connectorId="connector16"/>
<nodeMember connectorId="connector15"/>
</bus>
<bus id="internal2">
<nodeMember connectorId="connector17"/>
<nodeMember connectorId="connector0"/>
</bus>
<bus id="internal3">
<nodeMember connectorId="connector18"/>
<nodeMember connectorId="connector7"/>
</bus>
<bus id="internal4">
<nodeMember connectorId="connector8"/>
<nodeMember connectorId="connector19"/>
</bus>
</buses>
</code>
…as follows:
<buses>
<bus id="GND">
<nodeMember connectorId="connector16"/>
<nodeMember connectorId="connector15"/>
<nodeMember connectorId="connector17"/>
<nodeMember connectorId="connector0"/>
<nodeMember connectorId="connector18"/>
<nodeMember connectorId="connector7"/>
<nodeMember connectorId="connector8"/>
<nodeMember connectorId="connector19"/>
</bus>
</buses>
That way, these 8 connectors would always be tied to GND.
Let’s see if that works.
USB_molex_2171820001_GND_BUSS.fzpz (33.5 KB)
Beispiel.fzz (38.7 KB)
Best regards, Harald.
Hi Harald,
the shield plate now appears to be electrically connected to GND. I can’t see a connection as such, but when I click on it, GND and the shield plate light up at the same time.
I currently favour connecting the shield plate to PE via a capacitor (1206 C0G 2.2nF 1kV). It would therefore be better if the shield plate had its own net — e.g. shield1, shield2, shield3, and shield4.
That way, each user can decide for themselves what to connect the shield plate to.
Even when connecting to GND, there should be some decoupling. On Arduino boards (where there is no PE, so GND has to do the job), this is decoupled via a ferrite bead of type BLM21.
Ah, so it shouldn’t be connected to the other GND pads. I understand that. I once had serious ground problems with a preamp for a cassette recorder.
So I’ll leave pads A1, A12, B1, B12 as separate GND and combine the 4 mounting pads into one GND net.
Best regards, Harald!
The paste mask (stencil cutout) is currently determined by existence of layers:
This is again not sufficient enough for the USB-C connector, like the oblong cutouts, this is a new feature.
I think the currently best workaround to combine SMD and THT is to split it in two part composites:
One with only the pads, that uses copper1. And another one with the mounting holes, that uses both copper0 and copper1.
Edit: I reopened this issue about solder mask: more control over solder mask · Issue #2488 · fritzing/fritzing-app · GitHub
Hi Ralf,
I tried to find a compromise. I’ve set the PADs so that they appear grey in the stencil view. However, the mounting holes are no longer implemented as THT. So you can only solder the socket from the top. One option would be to place the four holes as a THT component exactly on the socket, so that you can solder the socket from both the top and bottom. Please check that first — only then would I check the socket with the script.
Component:
USB-C-molex-217182-0001.fzpz (28.5 KB)
Example:
PAD.fzz (34.6 KB)
Best, Harald!
