Bridge rectifier created


Simple bridge rectifier with round package and rubber-band legs in breadboard view.

PCB footprints:

  • round 200 mil
  • TO-269AA


bridge rectifier round.fzpz (10.4 KB)

bridge rectifier TO-269AA.fzpz (10.1 KB)

22.01.2019 / V1.2

  • Fixed serious bug in PCB round 200mil.

21.01.2019 / V1.1

  • Changed pad size from 0,12in (3mm) to 0,10in (2,5mm), hole size left with 0,04in (1mm)
  • Fixed the reported fzp and svg bugs.


But I think in PCB, the hole size is small, and the copper pad is too thick…!!


Actually the holes are fine. They are 0.040 same as the 1n40001 diode. Large pads are a good bet for potentially high current applications. In Inkscape hole size can be calculated as hole = diameter_of_pad - (2 * stroke-width). At the suggested scale (as this file is) that works out in thousands of an inch. In different scales you need to multilpy the scale factor in (I usally convert to the standard scale as being easier on me :slight_smile: ). Good parts, several of you are getting good at making parts which benefits all of us. A couple of minor nits though:

bridge rectifier round

Error 80: File
At line 53

Both terminalId and legId present, only one or the other is allowed.

this doesn’t appear to be bothering Fritzing (although Fritzing crashed when I deleted this part after moving one of the bendable legs to make sure it worked so maybe it is in some way.) You are getting very good if you can make bendable legs work, I usually still have trouble because there are undocumented rules (different parts of the legs must be specific graphic constructs and the legId portion must be outside the viewbox).

Error 18: File

Connector connector0terminal is in the fzp file but not the svg file. (typo?)

svg svg.breadboard.bridge_rectifier_round_200mil_d4b37b7d708ee9291c0aa1b4b3048108_3_breadboard.svg.bak

Again Fritzing ignores the missing terminalId (which typically isn’t in breadboard anyway) and uses the center of the svgId instead. This is typically a problem in schematic as the terminal will be in the wrong place.

Warning 25: File
At line 17

Silkscreen layer should be above the copper layers for easier selection
in pcb view

This is a warning because it doesn’t hinder function. It is however desirable the have silkscreen as the first group in pcb because it will select the silkscreen before it will select copper if slikscreen is last which usually isn’t what you want.

bridge rectifier TO-269AA

much the same complaints with only this new one:

Error 47: File
At line 87

LayerId copper0 doesn’t match any in View pcbView layerIds [‘silkscreen’, ‘copper1’]

which indicates you have copper0 definitions somewhere in the fzp file but it isn’t in the layerId definitions (which means the later instances will be ignored). As I said overall a good job.



Yes, the holes are okay, they are 1mm…
But, about thickness, it’s maybe good for high voltage, I was just worried about the 48mm copper trace between legs gets close…

Anyway, what I checked that, in the datasheet of W series bridge rectifier (w04, w10), the Spacing between legs is 5.6mm.
Here, in this pcb, the spacing is 5.08mm…

I don’t know, maybe my mistake…
I’m about to order some of them, and designing PCB for project, so I’m just curious…


Perhaps the W series isn’t what this part describes? I don’t see a part number in the part, and it specifies 200 mil spacing which would be 5.08 mm. You could clone this part and change the spacing for the W series.



Oh Yes, 200mil…
I’m just done with my new svg for it…


Peter, thanks for reviewing the parts.
I have fixed the reported issues and hope that they are ok now.



Unfortunately Inkscape has bitten you.

Error 65: File
At line 11

Connector connector0pin is an ellipse not a circle, (gerber generation will break.)

Error 74: File
At line 11

Connector connector0pin has no radius no hole will be generated

(repeats for connectors 1 - 3)

in XML editor:

id connector0pin
rx 35
ry 35.000004

rather than the correct

r 35

The result is that the gerber generator won’t generate a hole for the pad. This is round off error in floating point calculations in Inkscape (or which ever svg editor you are using). The easy fix is to use xml editor to set both rx and ry to 35 at which point it will revert to a r 35 and gerber generation will be happy.


As well you need to do an

edit->select all


file ->document properties->custom size-> resize page to content


Resize page to drawing or selection

to adjust the viewbox to the drawing dimensions (it is also complaining about incorrect scale currently, although scale is set correctly). Because the offset is positive nothing bad happens, if the offest were negative, the edges of the drawing outside the view box would be truncated in Fritzing.



Peter, thanks again for the detailed feedback.
I did the described corrections & hope not to stress your patience to much ;o).


Blue, I am not sure about how to read the W-series bridge rectifier datasheet …
Is the pin spacing really 5,6 mm or is it between min: 0,180in (4,6mm) and max: 0,220in (5,6mm)?



Looks good now. This really isn’t your fault, it’s a quirk of Inkscape’s, (or possibly python). For some reason it decided to recalculate the radius and floating point roundoff issues changed the circle to an ellipse which screws up gerber processing on our side, because it is looking for a circle to generate the hole. Similarly Inkscape inserts px on the end of font-size statements to be CSS compliant but Fritzing will set the font size to 0 if you edit a part with px in the font size. Neither is wrong, they are just doing different things. My parts check script looks for (and corrects when it can) these issues.



Your right it is unclear, but I think what they are trying to convey is that 5.6mm is the spacing to the outer diameter and 4.6mm is the spacing to the inner diameter of the pin making the pin 1mm wide and the center somewhere around 5.08 mm and should therefore match you part. If he has one of these printing out the footprint and trying it would confirm if that is correct.



Ugh!! That’s confusing… 1mm difference is huge… If I’ve to bend legs to place it, there will be space between part and PCB…
I should wait till I get one of those…

That’s why my all new & edited parts are referenced from actual parts…!!


I think that you will find that it is .2in center to center with a 1mm pin (the center point that we want being 1mm (2 * the difference between the larger and smaller numbers) + the smaller measurement, which puts it around 5.08mm and thus the original footprint should work fine, assuming I am reading the data sheet correctly.



Yes… Both datasheets just stated the spacing without & with pins…!!!
After your explanation, I got that… So, the 200mil must be correct… Thanks…