Meanwell - IRM-05-05 - 230V to 5V

parts submit
4

Over all pretty good but a few problems. The hole size in pcb is too small:

Hole size in gerber drill.txt file:

; NON-PLATED HOLES START AT T1
; THROUGH (PLATED) HOLES START AT T100
M48
INCH
T100C0.020505

indicating the hole will be 0.020 in when the pin is 1.04mm (about 0.047in) so the module won’t fit. The layerIds are missing in breadboard and schematic svgs. This means the part won’t export as an image (it will be omitted from the image.) I went through and cleaned up the part like this:

pcb

rescale (to get the part to the standard scale)

Removed the text. The reason for this is that the user can add the text to pcb in the sketch if they want it, but must modify the part to remove the text if they don’t want it. So in general don’t include text in the pcb view. Adjusted the hole sizes to be 0.047in. In Inkscape (it is different for the other svg editors) pcb hole size is set by

hole-size = pad-diameter + (2 * stroke-width)

so I set stroke width to 20 (20 thou) and the diameter to 0.087in which will create a hole size of 0.047in which should fit the pin.

schematic

I recreated schematic with the Inskcape Fritzing schematic extension which creates schematics at the correct scale and with the correct colors and font sizes (normally schematic pins are set to grey, color can be set but usually is not.)

breadboard

rescaled and set the layerId to breadboard.

fzp file

Change label to M (for module)

Replace icon svg with breadboard

remove terminalIds from breadboard (it isn’t in the svg and isn’t needed!)

<connector type="male" name="AC/L" id="connector0">
  <description>AC/L</description>
  <views>
    <breadboardView>
      <p svgId="connector0pin" layer="breadboard" terminalId="connector0terminal"/>
    </breadboardView>

to

<connector type="male" name="AC/L" id="connector0">
  <description>AC/L</description>
  <views>
    <breadboardView>
      <p svgId="connector0pin" layer="breadboard"/>
    </breadboardView>

Then ran the part through FritzingCheckPart.py to make sure all is ok (this is what flagged the missing layerIds on the original part.)

export as gerber to check the new hole size is correct.

; NON-PLATED HOLES START AT T1
; THROUGH (PLATED) HOLES START AT T100
M48
INCH
T100C0.038000
T101C0.047000
%

The bottom one 0.047in is the one for the module, the 0.038in holes are for .1in header connectors. All this is in this part

MW-IRM-05-5-improved.fzpz (18.4 KB)

How I did this is documented in this tutorial series

Peter