Part creation for CAN module Niren


Can anyone suggest part file to import in fritzing for CAN More module. Please refer link


A google search on “fritzing part mcp2515” turns up a copy of the IC itself and a canbus shield but no obvious part for this particular module. It is easy enough to make such a part, but as usual there doesn’t appear to be a mechanical drawing which specifies the location of the header pins (needed to make an accurate pcb view in case someone wants to mount it on a board).

edit: Since the layout of the module makes it not useful to mount on a pcb, this part should do what you want. It has only breadboard and schematic views and the pins are probably not quite correct position wise (because I don’t have one to measure) but I expect it will be close enough.

Niren_can_bus_module.fzpz (21.7 KB)



Hello Peter,
I have one module and i have took measurement with Vernier prityclose and accurately to make PCB view. Can you please help and add the PCB view. I tried my self and tried finding videos on Youtube how to make PCB view in fritzing i found non good video. Please suggest if you know any material to learn. please refer attached PDF for module dimensions. if you need more information please let me know.

I don’t thing we should include the Jumper pins in the view as one can put the jumper from top on the module to use. The 7 pins are important to connect with PCB. In this case we can desolder the 7 Pin strip and put it from bottom side and solder again, in this way one can mount the module on PCB keeping Jumper and components upside and have access to use the Jumpers.


That should work and is easy enough to do. This fzpz is a new part so it will load along side the original. It has a pcb view with the 7 pins the outline and the mounting holes. You should print out a copy of the pcb and check that it actually matches the module correctly before ordering boards though.

Niren can bus module pcb.fzpz (24.1 KB)

Learning to make fritzing parts is a little more exciting. The only way I know of is to start doing it and ask questions here (preferably with a copy of the sketch that doesn’t work :slight_smile: ) and several of us will help. These two tutorials refer to the current fritzing version (many others on the net are for earlier versions) and thus may help:

To make this part here is (more or less) what I did this morning:

Edit current pcb svg using Inkscape

  1. Ungroup copper1 and copper0 to ungoup the 13 pads, then select and delete connector7pin to connector12pin as unneeded

  2. select all the pads (connector0pin to connector6pin), group them then rotate them 90 degrees twice to invert their positions (needed so the connections are correct)

  3. select group silkscreen and ungroup it. Change the color on all the lines from white to black (so they are visible in Inkscape)

  4. Create a 3 mm circle (for the mounting holes) and set the color to black and strokewidth none change the name to nonconn0

  5. duplicate it 3 times (for the other 3 holes) and name them nonconn1-3

  6. move the pad group and the 4 mounting holes in to position (I used thin lines in the correct places to align them)

  7. Ungroup the 7 pads that you grouped above (to remove transforms) then select the pads and the 4 mounting holes and group them twice.

  8. change the first group id to copper1 and the second group id to copper0.

  9. delete the thin alignment lines if you used them

  10. Delete the line marking pin 1 on the header and change the length of the 4 border lines to match your drawing (40mm by 28.2) and move them in to position to make a square. At this point doing a resize drawing to page is a good bet to make coords start at 0

  11. Add the text for the pins so it board alignment on the pcb is obvious.

  12. With xml editor move the text above the copper1 group.

  13. again in xml editor select the first line in silkscreen and group it, change the id to silkscreen

  14. In xml editor select (one by one) all the other lines and all the text and click indent node to move them in to group silkscreen.

  15. At this point you should have group silkscreen followed by copper1 (which has copper0 in it) so click edit select all and in document properties click resize page to drawing or selection and save it as plain svg.

  16. Now edit the fzp file to change the metadata to indicate the pcb now exists and add in the pcb defintions that I removed so supress the pcb and create the new part.

  17. in pcb svg manually remove the translates on connector0-6 that Inkscape has insisted on inserting.

  18. remove the px from the font sizes in the svg too.

You could start from the pcb svg of the original part and try and follow the above steps (you probably need to know a fair bit about Inkscape to follow them which is a complex task in itself), and see if you can come up with a working svg file that matches the one in the new part. The fzp file changes assume you know the file format, so I’d just copy the one from the new part for now. It is usually much easier when you have a working example to compare to.