ESP32 DevKitc V4.fzpz (90.1 KB)
You can download espressif esp32 devkitc v4 from here. I draw it from image on Inkspace. Find shemes, hope it is right. I wrote some notes on pins you cans ee while mouseover. Have fun 
If you need more info about board use this pinout ESP32-DevKitC V4 Getting Started Guide - ESP32 - — ESP-IDF Programming Guide latest documentation
Not a bad job, but a number of errors. This tutorial set should tell you how to correct them:
Starting in breadboard
The scale is slightly wrong. Note the bottom left wire is not straight. The pins should be exactly on a 0.1in boundary and they are not. You likely need to rescale the image slightly to correct this. The bottom two right connectors are not correctly defined and thus don’t connect. The ratsnest line comes from this connection in schematic (which is almost correct other than the terminalIds)
The wires are connecting to the center of the pin because the terminalIds are not correct (missing completely in some cases.) The fzp file should look like this:
<breadboardView>
<p layer="breadboard" legId="connector1leg" svgId="connector1pin"/>
</breadboardView>
<schematicView>
<p terminalId="connector1terminal" layer="schematic" svgId="connector1pin"/>
</schematicView>
<pcbView>
<p layer="copper0" svgId="connector1pin"/>
<p layer="copper1" svgId="connector1pin"/>
</pcbView>
where each connector has a terminalId called connectorxterminal which is also in the schematic svg. In the current fzp file many of the pins lack the terminalId definition causing the above problem.
<breadboardView>
<p layer="breadboard" svgId="connector3pin"/>
</breadboardView>
<schematicView>
<p layer="schematic" svgId="connector3pin"/>
</schematicView>
<pcbView>
<p layer="copper0" svgId="connector3pin"/>
<p layer="copper1" svgId="connector3pin"/>
</pcbView>
there should be a terminalId=“connector3terminal” added to the schematic connector entry above. The pcb svg is the wrong scale. The pins on the board should be in the same place as the header beside it as one is supposed to connect to the other.
the traces should be horizontal not at an angle. If you have troubles fixing this feel free to ask for help!
Peter
ESP32 DevKitc V4.fzpz (137.7 KB)
Me and my friend redesigned the pins for Breadboard and Pcb. I think all is done. I hope Fritzing add this to their parts. Thank you for your help @vanepp
Still problems. This is the output from FritzingCheckPart.py
Error 69: File
‘svg.breadboard.ESP32 DevKitc V4_ce08f31c35c5981bbe852cf0263a676b_3_breadboard.svg.bak’
At line 516
Found a drawing element before a layerId (or no layerId)
Error 74: File
‘svg.pcb.ESP32 DevKitc V4_ce08f31c35c5981bbe852cf0263a676b_3_pcb.svg.bak’
At line 1267
Connector connector19pin has no radius no hole will be generated
Error 74: File
‘svg.pcb.ESP32 DevKitc V4_ce08f31c35c5981bbe852cf0263a676b_3_pcb.svg.bak’
At line 1268
Connector connector20pin has no radius no hole will be generated
Error 74: File
‘svg.pcb.ESP32 DevKitc V4_ce08f31c35c5981bbe852cf0263a676b_3_pcb.svg.bak’
At line 1269
Connector connector21pin has no radius no hole will be generated
The no layerId error will cause the part to not be exported as an image. It is fixed by adding a group called breadboard to the breadboard svg like this:
to this
In pcb the pads need to look like this to cause Fritzing to drill a 0.038in hole in pcb. As well the silkscreen stuff should be deleted as it typically isn’t used (it will however work as is unlike the pads!)
You need to replace all the red dots with the pad outlined in green here.
Peter
This screwed me up a little. Got a pcb from JLCPCB with holes missing. Okay I think it’s fixed now. Try this…
ESP32 DevKitc V4.fzpz (141.8 KB)
If the original poster made the changes I suggested above they didn’t post a new version of the part. That said, your new version still has a number of problems, mostly cosmetic but the pcb hole size is only 0.036in and they need to be 0.038in to fit 0.1 header pins so your new board probably won’t work either. The breadboard svg is still missing its layerId and thus won’t export as an image.
In schematic the problems are cosmetic. The font sizes are wrong, the one circled in red should be 35px and be the pin number and the one beside the pin should be 49px and the pin name. In pcb
all the stuff and pin numbers should be deleted, the outside edge of the board should be 10 thou wide and be the outline of the complete part and as noted the holes in the pads should be 0.038in like this (taken from the gerber output drill.txt file)
; NON-PLATED HOLES START AT T1
; THROUGH (PLATED) HOLES START AT T100
M48
INCH
T100C0.036000
T101C0.038000
%
T100
X010125Y007051
X025126Y007051
X007125Y017055
…
T101
X015126Y020051
X011126Y020051
X007126Y020051
the line T100C0.036000 indicates that the holes defined as T100 are plated through, and 0.036in in diameter. The T101C0.038000 indicates that the T101 holes are plated through and 0.038in diameter (and are the 0.1in headers I added to the sketch!) Here is a corrected part that meets the graphics standards and is ready to be added to core parts.
ESP32_DevKitc_V4.fzpz (37.9 KB)
Peter
Thanks Peter and sorry about the hole size being wrong. I actually just copied and pasted the holes from the svg of the arduino nano part. Anyway great news that the community now has the esp32 devkit part.
