Drill size does not match the copper hole size (Solved)

I am fairly new to Fritzing but have successfully made custom Board SVG’s and two custom parts but all of a sudden my latest part is having issues and after two days of variations and googling I can not find the answer.

The copper rings turn out the correct size but the drill hole is tiny.

I have attached the part as exported from Fritzing.
IN-16 Nixie Tube.fzpz (13.3 KB)

( I tried uploading the pictures separately but as a new user I am not allowed).
(pic 1) You can see the copper holes are fairly large (0.75mm hole with a 0.275mm ring)
(pic2) They show up correctly in Fritzing PCB view.
(pic3) But once you export it as Gerbers the holes are tiny. Even smaller than the via’s.
(pic 4) As you can see on the bottom right board the drill holes (in the circle pattern)

Hole sizes are in the svg so you need to upload the ,fzpz file, or the complete sketch .fzz. Just use the 7th button above.

Opps I thought that is what I had uploaded. Here is the correct one I think.
IN-16 Nixie Tube.fzpz (13.3 KB)

Yeah drill.txt shows 0.007" holes.

Peter had that problem so he probably knows the fix - maybe because they are paths not circles -, but I would redraw a “circle” connector using the circle button, duplicate, snap them on the originals, and then delete the originals.

You also don’t need all those paths in copper1 if copper0 is inside copper1 and has everything. The bottom layer copper0 gets duplicated in copper1 if it’s inside it. You also don’t need that terminal5 as far as I can see.

Thank you for letting me know I do not need to duplicate all the paths from copper0 in copper1. When I created the SVG I only had three main groups. copper1, silkscreen. I then had copper0 group inside the copper1 group. Once I open it with Fritzing part editor and save it again I end up with the groups inside of groups inside of groups etc and it also changes the id’s from connectorXpad or connectorXpin some times. Is this normal behaviour or is it a sign of the problem I’m having?

Yeah FZ adds stuff. If you look at your export part everything is now 7 groups deep.

Ok I remade the rings using the circle tool and it works now. Thanks so much. It exports perfect Gerbers now so I’m not too concerned.

Is there a way to replace a part in a sketch without deleting it and starting over? I have a lot of complex routes on both sides that I do not want to have to redo.

For anyone else that comes across this thread I should say the original SVG was created as an export from Blender of a part I had made there. I then used Inkscape to simplify the rings which made them look correct but Fritzing obviously wants a specific type of path.

Turns out that once I connect the pads to their respective nets the connection points move really far away. So I still don’t have a working part.

So I think I have it figured out. I removed all the extra groups, saved the svg over the last updated fritzing svg. Opened the part in the editor and reassigned the the pins and now it works.

Here is the updated part. It in not ready for publishing because it uses an IC schematic currently but for normal use it works.IN-16 Nixie Tube.fzpz (14.0 KB)

If anyone could try it out with a few connections and make sure it looks correct that would be most appreciated.

13 holes 0.031", seams to be fine. We use Gerbv to view the gerbers, and add 1 layer at a time to check what each does. You can also add the drill file the same way to see the holes.

You can draw the SCH svg, right-click on the part in the bin, Edit Part/Schematic/File/Load image for view, if you just want to change just 1 drawing.

Thanks again. I also use Gerbview but I used Aisler’s renders for my picture upload because they are pretty.

The Schematic just isn’t on my list of important things. I did check and you can find generic Nixie Schematic SVG’s online so I may convert one of those, although most of them are only for 0-9 and do not include the decimal point connections so I would have to add those.

.031 may be a little small (that is the standard size hole for an IC leg) from what I remember of nixie tubes (I haven’t seen one in 15 or 20 years) the pins are more likely to be around .1 post size or .038 in I think. You probably want to measure a pin with vernier calipers before committing to a board I expect. In Inkscape hole size is pad dianeter less stroke-length*2, so for a .038 pad with the normal 20 strokw width the pad diameter needs to be .078 in (which when you subtract 40 for the stroke with leaves you with .038 for the hole size). Your board looks to be in something like mm but the calculation should be the same.


Thanks for the reply. The legs are only 0.6mm or less on very small tubes that fit in a watch ( I have three different kinds). The hole size was chosen to fit the legs while still having room between the pads for 8mil traces with a 8mil clearance between them. It won’t be the easiest to get the legs through but should be possible (fingers crossed). I could make the hole larger but I figured 0.25mm copper was already small and I didn’t want to go down to 6mil traces and spaces even though they would be fine for the 2.5ma going through them.

I just remeasured and the smallest tubes have 0.4mm leads so I shouldn’t have any problems.

I like Gerbv more than Gerbview because it has a ruler to check distances.

You could put a oblong or rectangle on the pads and angle them towards the center if you need more mechanical grip to the PCB.

Gee 0.4mm is a thin pin, at least for us old guys.

Good idea on the non-elliptical pads. A tear drop shape should work. Although in this usage I am not to worried about stress on the pins.

Thanks for the tip on Gerbv. I went to check if gerbv was available for Linux and it turns out that is what I have installed. I just thought it was gerbview since the title bar says Gerber viewer. I’ll will be sure to check out the measurement tool.