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

[Giugiu]

Hello,

I’m new on fritzing and i was searching for a project a Meanwell part for IRM-05-05.

As I couldn’t find any, I made this first file :

I haven’t tested it on a PCB yet, so if some experts can verify it that would be great.

I hope it will be useful to the community.

Have a nice day

PS: How can i upload the fritzing part on the forum?

[vanepp]

@Giugiu

PS: How can i upload the fritzing part on the forum?

Upload the .fzpz file for the part. Upload is 7th icon from the left in the reply toolbar.

Peter

[Giugiu]

Thanks Peter!

Here is the Fritzing file.

MW-IRM-05-5.fzpz (27.6 KB)

It would be great if someone could look at it to see if I’ve done this part right.

PS: The upload problem comes from google chrome (I didn’t have access to all the file extensions). It works fine on Firefox.

[vanepp]

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

Part creation howto part 1 breadboard and pcb

Someone in this forum post requested help to fix up a part. So while doing that I decided to record what I needed to do in order to fix the part to provide a tutorial to create new / fix broken parts. If you start from the Tarjeta S4A EDU.fzpz file posted in the above thread, you should be able to recreate my improved part posted in the same thread. I started by loading the original part in to Fritzing, that indicates breadboard is (at first look anyway) pretty good, but schematic and pcb are…

Peter

[Giugiu]

Thank’s a lot!

I will try to do better next time.

I begin to read your tutorial.

Thank you again!

[Marlock]

Hello,

Thank’s for this part !
It is possible to have IRM-02-5 too ?

I will try to create it if is not possible =)

[vanepp]

@Marlock

It is possible to have IRM-02-5 too ?

Sure it is a relatively simple change (for me, perhaps less so for you )

This set of tutorials describe parts making (which is not simple!)

Fritzing PART CREATION Video Tutorial Series

NEW FASTER PART MAKING VIDEOS AT THE BOTTOM-Fritzing Parts Fast ADVANCED FRITZING USER TIPS & TRICKS VIDEOS AT THE BOTTOM-Fritzing Adv Tips & Tricks A series of part creation videos - I’m not an expert, but there was nothing else around at the time. Use 1080p HD fullscreen to see details clearly - use gear symbol bottom right -. Recorded slowly for older people, so select a higher speed if it’s too slow. P.S. - Sorry about the voice/sound Fritzing Part Creation - Chapter1 - New Part …

Part creation howto part 1 breadboard and pcb

Someone in this forum post requested help to fix up a part. So while doing that I decided to record what I needed to do in order to fix the part to provide a tutorial to create new / fix broken parts. If you start from the Tarjeta S4A EDU.fzpz file posted in the above thread, you should be able to recreate my improved part posted in the same thread. I started by loading the original part in to Fritzing, that indicates breadboard is (at first look anyway) pretty good, but schematic and pcb are…

and here is the new part

meanwell-IRM-02-5.fzpz (5.5 KB)

Peter

[Marlock]

Thank’s you for the part and the tutorials !
I’m a begginer with fritzing and I will learn these tutorials

[real-bombinho]

I was looking for the IRM-03, as I had not found anything I made this from the provided IRM-05:

[file removed to avoid confusion]
revised version here

For the PCB I used a scale of 100 dots per millimetre instead of the usual 1000 dots per inch. Could this become a potential problem? The printout of the PCB on a bit of paper worked well so far.

Also I noted that the part somehow offers me variants, which is okay for the IRM-05 but it does as well offer some variants of the Hilink power supplies? How does this happen, is it linked to the family?

Is there an easy way to rather have editable voltage or voltage variants?

[vanepp]

@real-bombinho

For the PCB I used a scale of 100 dots per millimetre instead of the usual 1000 dots per inch. Could this become a potential problem?

No. It is desirable that the viewbox be 1/1000 as specified in the graphics standards but in practice it will work just fine as the svg scaling automatically compensates. Dimensioning the svg in px rather than in or mm can be a problem but you haven’t done that. FritzingCheckPart.py only issues warnings for the scale no errors so the part appears fine:

Warning 32: File
‘svg.breadboard.MW-IRM-03-05_02d58bc319d1e0b5412c1291a19f7c29_13_breadboard.svg.bak’
At line 2

Scale is not the desirable 1/1000 ratio from width/height to
viewBox width/height.

Warning 32: File
‘svg.pcb.MW-IRM-03-05_02d58bc319d1e0b5412c1291a19f7c29_13_pcb.svg.bak’
At line 2

Scale is not the desirable 1/1000 ratio from width/height to
viewBox width/height.

it is only a warning because it doesn’t affect correct operation (but doesn’t meet the graphics standards.) There is potentially a problem in pcb in that the hole size is 0.031445in, for a 0.1in header (if you chose to mount the part on a header) the size should be 0.038in. The pin size may or may not be correct for the part I didn’t check.

@real-bombinho

Also I noted that the part somehow offers me variants, which is okay for the IRM-05 but it does as well offer some variants of the Hilink power supplies? How does this happen, is it linked to the family?

The multiple options in Inspector are indeed a function of the family name. Any part with the same family name will be listed as an option in Inspector. There aren’t currently any guidelines on family names (although discussions are happening very slowly on github) on that or a variety of other parts policy issues.

@real-bombinho

Is there an easy way to rather have editable voltage or voltage variants?

If the text labels in breadboard or schematic are of the name “label” they will be substituted from the property name chip label in the fzp file

    <property name="part number">74x125</property>

which can be used to change the voltage on a part. This tutorial covers various of these issues

Part creation howto part 1 breadboard and pcb

Someone in this forum post http://forum.fritzing.org/t/tarjeta-s4a-edu-pieza-en-proceso-solamente-falta-la-imagen-en-pcb-y-en-esquematico/7487 requested help to fix up a part. So while doing that I decided to record what I needed to do in order to fix the part to provide a tutorial to create new / fix broken parts. If you start from the Tarjeta S4A EDU.fzpz file posted in the above thread, you should be able to recreate my improved part posted in the same thread. I started by loading the origi…

Peter

[real-bombinho]

The pins are specified at 0.6mm and measure precisely 0.6mm. I had aimed at 0.8mm vias, hence the 0.031445" seem very close.

Though right enough, from a replacement point of view 1mm might be more comfortable to extract.

[vanepp]

And it provides the option of installing 0.1in headers to plug in the module. Either should work fine though.

Peter

[real-bombinho]

revised version:
MW-IRM-03-5-improved2.fzpz (32.2 KB)

[vanepp]

That looks better. It is now 0.039in (from exporting the gerbers and then checking Untitled Sketch_drill.txt):

INCH
T100C0.039147
-------------

which should take a 0.1header as well as the device.

Peter

[real-bombinho]

Thank you for your help, Peter.