Bottom Copper Layer Form Problem

Hey. So our team would like to edit a 15 pin terminal because we would like to make the distance between each pin to be 3.81 between the center of two pins. We edited the svg file of the PCB of Screw Terminal using Adobe Illustrator (below):

We were able to successfully edit the pinhole distances so that they are 3.81mm apart in each group. They are all under one layer, as well. (below):

However, after uploading the edited svg file of the board with the updated pinhole distances, it appears as though a grounded wire is also added to the Bottom Copper Layer.

Does anyone know how to resolve this issue? Or is there a better way to edit parts? Thank you!

To edit the terminal, we ungrouped the pinholes from their layers. We then deleted all pinholes, leaving only one. We would transform this one by moving it 3.81mm and making 14 copies. Those objects became individual arrays by clicking Object → Transform Appearance. Finally, we grouped these objects into a copper group. We repeated this process for each copper group individually.

This is the Generic 15 Pin Screw Terminal we chose to edit.


You look to have deleted all the connector definitions (which causes the red rectangle you are seeing.) It is best to upload (upload is the 7th icon from the left in the reply menu) the .fzpz file of your modified part so we can look at the svgs and fzp file to correct it. Alternately these two tutorials cover making parts (which is quite complex) on the current version of Fritzing.



FZPZ file would be better…
Use this svg file…
If there is still problem, maybe also problem in bb/schem file.

PS: just checked the pitch is 3.5mm, if the file work, please edit again…

terminalblock_15pin1.fzpz (12.6 KB)
Nevermind - here is the .fzpz file

Breadboard looks fine as is

schematic is missing terminalIds and thus the wire connects in the middle of the pin rather than the end:

the terminalId is present, just in the wrong place in the svg:

Change them like this and it will work.

on the ones other than the first one it was necessary to add a stroke and fill attribute of none and set the width to be 0.7 to match the height like this (in Inkscape, don’t know about Illustrator!)


Pcb is incorrectly configured which is why the red rectangle.

it needs to look like Blues’s svg with copper0 being a subgroup of copper1

I will just replace your pcb svg with Blue’s (rather than spending time to fix yours) and that should fix things. Running the resulting part through (detailed in my tutorial) indicates a problem with Blue’s pcb svg. The svg is dimensioned in px which can cause scaling problems in Fritzing. Your svg above is dimensioned in in which makes it dimensionally correct and may be the source of Blue’s different pitch. It is worth printing out the pcb footprint at 1:1 scale and comparing it to a real part before ordering boards though.

Warning 19: File
At line 3

Height 151.699px is defined in px
in or mm is a better option (px can cause scaling problems!)

Warning 19: File
At line 3

Width 18.432px is defined in px
in or mm is a better option (px can cause scaling problems!)

This actually appears to be an issue that Blue introduced as your original svg is correctly dimensioned in inches, so I will start from it and make the changes there. The corrected svg looks like this

with a silkscreen group (which you had) and nested copper1 and copper0 groups and hopefully the correct pitch. That produces this working part

terminalblock_15pin1-fixed.fzpz (8.9 KB)

In turn this part looks like this in Fritzing

(I didn’t change the moduleId or file names so you will need to delete your current part in Fritzing to load this one!)

As we see pcb now works correctly. Whether it is correct or not depends on your original breadboard svg. One thing that may be incorrect is the hole size of the pads. They are currently set to 0.04in (found by exporting the sketch to gerber files and looking in the drill.txt output file.) That may or may not fit the terminals you are using and should be checked before ordering boards. Hope this helps, and if you have questions feel free to ask!