Hello Everyone,
This post is to update people on my PCBA experience with using Galp's v1.0 board.
It was posted on endless-sphere here:
https://endless-sphere.com/forums/viewtopic.php?f=2&t=109266&start=75#p1656363
The silk for that OLD file was labeled "V2.0, May 2021, OW"
Those boards were assembled, but some things were changed thanks to PCBway finding some errors. The notes below show a combination of what was done to create may2021, AND how you had to fix the board that board to work.
I am now posting the Nov2021 version, that represents an update of everything. Updated files are included in the zip file. The attached file when unzipped includes a readme with a subset of these instructions. Found in: README.txt
The resulting zip file may be found
HERE
The silk for that NEW file is labeled "V2.1, Nov 2021, OW"
What was done to create these files:
This board started with Galp's v1.0
Total set of known changesModifications to schematic and eeschema:
-updated the silk to "V2.1, Nov 2021"
-changed pins of the crystal (to connect circuit to 1 & 3)
-tied pin 2 of crystal to ground
-changed crystal to (ECS-80-18-30B-AGN-TR)
-trace to pin 2 of crystal to ground
-changed footprint of crystal
-removed U7, fixed traces
-minor changes to silk
-added "MANUFACTURER", "PART", "SMD/TH" into symbol editor, populated all those fields
dumped all the parts into single column, cut and pasted into mouser BOM maker
cut and pasted all the part manufacturers from mouser spreadsheet into the symbol editor
edited the SMD/TH column
-the original part for USBLC6-2P6 was wrong
-the foot print for:
C34-C39, C54, C62, C64, C76, C78, C83, C89, C95, C99, C102, C103, C106, C109
should be 0603, changed the part to: 810-C1608X8L0J225K08
-the part number assigned to C4,C5,C6,C7,C8,C9,C13,C14,C15,C65,C66,C67,C104 were wrong, and needed to be 270p
used: Mouser #:80-C0603C271J5G
-added part numbers for the LEDs
-TAJD107M016RNJ was too large (note "D" in TAJD)
Changed to TAJC107M016RNJ (note "C" in TAJC)
-PCBway wondered if R77,R78 part RC0603FR-1324R9L, value is 24.9R ok. it is okay.
-TH1 (the termister) of may2021 was wrong.
changed to mouser #81-NCU18XH103F6SRB
The directory: "T-K124W15822A pictures" shows some pictures that were part of the emails from PCBWay
The spreadsheet "t-k124w15822a_response.xlsx" was sent by PCBway to confirm some parts. It also contains prices.
Hey, speaking of price, how much did this cost?
$116 for 10 PCBs
$1196 for 5 assembled boards
that does not include the cost of throughput parts.
==============================
==============================
MAKING THE BOM FROM KICAD EESCHEMA
For MacOS,
copy my_BOM2csv.xsl plugin to here:
/Applications/KiCad/kicad.app/Contents/SharedSupport/plugins
Got to Tools->Generate Bill of Materials
Load up your custom script
Be sure to change:
"%O"
to
"%O.csv"
Manually:
-touch up the column headings if needed (in my case there were extras)
-sort on SMD/TH to find rows to remove
-save as excel file
-remove csv old files
total parts: 226
------------------------------
MAKING THE CENTROID FILE FROM PCBNEW:
File --> fabrication outputs --> footprint position file
Select: CSV, millimeters, single file for board
Select: "Include footprints with SMD pad even if not marked Surface Mount"
(gets R31, R32, R33)
Open the resulting file, do these steps manually
-You have to remove some stray parts
remove all refs beginning with J, FED
-Rearrange columns so the fits the headings in the next step:
- add:
"*RefDes<TAB>MidX (mm)<TAB>MidY (mm)<TAB>Package<TAB>Rotation<TAB>Top/Bottom<TAB>Val"
to the top
- save as excel file
- remove csv file
total parts: 226
------------------------------=
PCBway wants all the components could be clustered on to one line
Use bom2grouped_csv from eeschema
set output to %O.csv"
Import into excel
Look at column SMD/TH --> Sort on SMD/TH
Remove all non-SMD parts
Total lines: 53
Perform a sum on column B:
Total parts: 226
------------------------------=
create gerber files.
in PCBnew:
File --> plot
Use the gerber settings as shown in PCBA/GERBER_SETTINGS.png
Hit Generate Drill Files...
Use the gerber settings as shown in PCBA/GERBER_SETTINGS.png
==============================
==============================
NOTE: when I report in the notes above that something was "wrong" that does not mean Galp's original design had a problem. It may very well have been introduced when I made modifications to his file in order to create a BOM. I am not saying his original schematic or PCB had errors.
