Led Driver Board 350ma pwm - updated with test part V3

Was only allowed to put one image in each post…

We won’t know until we get the svg’s or the finished part.

To upload here you change the extension, like .svg to .fzpz, because the forum only takes .fzz .fzpz, etc

There is a video tutorial in parts help.

Changed svg extension to fzpz

1w led driver 350ma pwm Breadboard.fzpz (18.8 KB)

1w led driver 350ma pwm Schematic.fzpz (2.7 KB)

1w led driver 350ma pwm_PCB.fzpz (2.2 KB)

The breadboard doesn’t have any nodes labeled connector, good drawing though.
The PCB will have to have major mods because it’s just supposed to be 6 pads and outline, but in specific groups.

It’s hard to say how it will come together until they are imported into the part.

OK, I’ll try again and will upload new files after I have redone them.

Looks like a good start. You probably want more detail on the pwm pins though, I assume one is likely ground and the other the active pwm signal and it would be good for the schematic to show which is which (a quick google search didn’t turn up much technical info on this board, just lots of people selling copies of it with no documentation). You may want to have a look at this tutorial in pars creation as well as Old_Grey’s videos:

You can export the part from Frtizing as an fzpz file which will contain the fpz file along with all of the svgs as well which makes it easier for us to make suggestions.


OK, thanks.
I’ll start the search for the documentation on this board.


It may be easiest to just post the part number of the chip it uses. That would give us the data sheet to tell you what the pins do. Typically these boards from china don’t have any documentation, I often have to get the chip part number and work from the data sheet (and sometimes trace pins) to see how to drive them.


Sorry for not answering you. Real life and work got hold of me.
Will try to find the part number of the chip.


Not a problem, there is no hurry :slight_smile:


I think i actually did it?
almost… I have some problems with the font OCRA, it gets substituted with a system font and I still need to find which chip is used to I can set ground on the PWM.

but here is the part so far
1w_led_driver_350ma_pmw.fzpz (12.8 KB)

Is there anything else that needs changing


updated schematics

1w_led_driver_350ma_pmw.fzpz (205.8 KB)

Found out that from a mac I need to use the SVG Tiny 1.1 to solve the font problem

Looking not bad, a few issues though:

Breadboard: the svg lacks a group named breadboard (as specified in the fpz file), the only thing I know this breaks is exporting the image as an svg in Fritzing. The terminals should be in the center of the hole for the pin so the wires in breadboard would connect as in real life (at the moment they connect to the edge of the pad).

Schematic: layer id is breadboard not schematic as it should be. Connector2terminal is missing from the svg and thus the connection snaps to the center of the pin (rather than the end of the pin as the others do correctly).

PCB: Its desirable to have an outline of the board on the silkscreen layer so if you were installing the driver on a larger pcb you would know how much space it needs to avoid overlapping other components. In the gerbers the hole sizes are a little odd (and a little large). My local fab house offers free drill sizes at .035 (IC pins), .038 (.025 square header pins and probably what you want here) .042 and .052. Your holes are currently .044


OK, tried to fix the the things below

id=breadboard, female and center connectors. The design of the board do that I can’t match the PWM holes to the breadboard, but VIN and LED does.

id=schematic, Female and connections to end of pins

Fixed: Silkscreen added and holes resized to 0.038

1w_led_driver_350ma_pmw.fzpz (14.9 KB)


Almost there :slight_smile: two last problems only one of which I know how to fix: your silkscreen doesn’t display (fixable) and your holes are now too small (don’t know how to fix that in Illustrator) so I copied a correct size one made in Inkscape in to your pcb. The silkscreen is easy (although finding it took me a while), the id in the svg is Silkscreen, it needs to be silkscreen (all lower case) to match the fpz file which is apparently case sensitive. While the Inkscape hole ( id connector1pin-6 which you need to delete when you get this fixed) in the pcb works correctly, setting the same parameters on the existing holes doesn’t work so I don’t know how to fix that (hopefully you will, via experimentation if nothing else :slight_smile: ). To see your hole sizes with the part loaded in Fritzing and pcb selected (and the board within the grey area as parts out side the grey area will be truncated which has tripped me up more than once.) click file->Export->For Production->Extended gerber and set an empty directory then click select folder. In that directory there will be a file called Untitled Sketch_drill.txt which is the text drill file. Mine for this part looks like this:


The first one is my hole from Inkscape at .038 (and a bit) the other is your 6 holes at .022 that you need to convince to be .038 like the first one somehow. Hope this helps.


First, thanks for all your help.

Silkscreen is now visible. The holes took a little bit of trial and error, but the values are now:


1w_led_driver_350ma_pmw.fzpz (17.7 KB)


No problem, the more people we have making parts the better for all of us. Hopefully if people see there is help available more of them will at least try to make parts. Your part now looks fine to me, we will see if one of the more experienced folks spots something I’ve missed :slight_smile: .