Hello to all,
I am from France and i want to made this projet:
https://ubitx.net/2018/07/02/homebrew-ubitx-with-through-hole-components/
With this link, you can see it, and you have a link to download files.
On the zip, you have 5 files with Gerber extension to create à PCB board.
But, it seem to be type 274D files.
I contacted a company that makes printed circuits, but it tells me that the files are useless.
If you look at this same site, others have had the same problem
Do you have a solution to have file in a usable format
Sorry for my English.
Cdt
These files are indeed not compliant with GERBER standard. IMO your best bet would be to contact the author of this board.
1 Like
It seems these gerber files are missing the newline characters. Normally there should be one command per line but these files look like they are a single line (or white space chars in general).
Hello,
Some help here
http://gerbv.geda-project.org/
Normally you have an option in Kicad to convert file gerber. i look at that, but you said “missing the newline characters.” infile, so it will not work
Cdt
I am not even sure these files were created by KiCad in the first place to be honest. The PDFs of the schematic and of the layout do not look like PDFs i would expect to come from KiCad.
So i am not sure how we should help here. As @fred4u already indicated you will need to ask the creator of this project if they can do a fresh export or if they can give details what gerber version they used.
It might also be that the problem comes from the zipping process. Maybe a particular program must be used to extract the files (I of course use the unzip Linux program so there could be a problem introduced by it)
Ok
I’ll see if there’s a file converter 274D to 274x or and old version, but in évaluation mode you can’t print!! (Ex: gerber 2.6) Lol
it’s clear here:
There are two standards defining Gerber files: An old one called RS-274D, and a newer one called RS-274X. Gerber files generated in the old format (RS-274D) lack aperture information, which must be supplied separately. The new standard (RS-274X) embeds aperture information into the file. Note: Gerbv displays RS-274X files! Gerbv will not display RS-274D files! When you create Gerber files using your PCB tool make sure you export RS-274X files if you want to view the files with gerbv.
Others have not been so successful
here a message from manufacturer:
Hi Peter,
I got the answer from the same company about making PCBs for the uBitx including the arduino. I sent the ZIP file and here’s what they ask? Please Help.
Best regards from YU1KM,Miki (Kostadin).
Hi Kostadin,
Good day. This is Vicky, we’re glad to hear from you.
We checked the Gerber, but the format is not we need. Can you please output in RS-274X format? Thanks.
Best regards,
Vicky
——
WONDERFUL PCB (HK) LIMITED
Room A, 6th. Floor, Nanyuan Fengye Mansion
Nanshan Avenue, Nanshan District
Shenzhen City 518054, China
I never came across the 274D standard. It being in that standard could explain the extra DCODES.txt file as well as the gerbv and even kicad gerber viewer behaviour.
The author gives the manufacturer they use so maybe just order with them? (My guess is that they still support that gerber standard)
By the way KiCad also uses the newer format but its gerber viewer at least can open the original format in some fashion (I have not found a way for it to use the DCODES.txt file. So the result is not really useable.)
Or contact your manufacturer if they have the capability to convert the old gerber format to the new one. Might cost you a bit.
euro circuits also has a page for the old format https://www.eurocircuits.com/rs274d-standard-gerber-with-separate-aperture-tables/
But this looks more like an encyclopedia than a list of supported formats. It is however for sure worth a try to get your board manufactured with them.
I would not say that the files are “useless” or that it would be hard to fix.
KiCad seems to be fine with the missing newlines.
If I open Layer2.gbr in GerbView it looks like:
All lines have a width of 0, so it seems all coordinates are read fine, but the apertures are missing, and these are apparently in one of the other files.
RS-274 used to be a big mess, with tens or mayby 100’s of slightly different dialects. But it looks like it’s doable to convert the data, maybe it’s as simple as copying the contents of DCODES.txt into the .gbr files, with maybe a bit of added fiddling.
It also seems possible to just backport these gerbers into KiCad, and then re-trace the coordinates with the normal KiCad track drawing functions. If you want to go this way, then start with an 8 layer board or so, to keep this old data on separate layers from the new tracks you draw.
Hello,
try the method descripted on electronic stackexchange:
open the zip whith option GBR of kicad
after export it with pcbnew option
it’s seem working, but i can’t post file when you are a new user
it’s will create a new file type kicad
if i have all understood, all will be good, but no drill (?)
if you confirm that it can do both sides of epoxy board with this method, even without making the holes and serigraphy, I don’t care.
I’ve already made hundreds of holes on epoxy. It’s a proto for my use. Too bad, there will be no metalized holes, we will weld both sides.
If ok, i will send the file to manufacter here in France, i can say to me, if it’s ok for im
cdt
I also did this, and as I suspected, you can make a KiCad PCB out of it, but the width of the tracks is missing. There is also something going wrong with the coordinates. KiCad thinks the whole PCB is 15 mm wide. The easiest way to fix this is probably to add the right code for the units to the “.gbr” files before opening them in GerbView.
Drill data (Excellon) seems to be in the file “DRILLDATA.txt”, but it’s not very important.
To make this a complete KiCad project. I would start by checking if someone else has done this before you. If so, then simply use that project.
If not, then you have to do it yourself and then I would do it in this order:
- Convert & import the .gbr files to the right scale and make a KiCad project out of it.
- re-create the schematic from the .pdf files by printing the .pdf files on paper and then putting all components one by one in Eeschema.
- Do normal Footprint association in the new schematic.
- Import the netlist and components with [F8] from Eeschema to Pcbnew.
- Place the components in (approximately) the same place as the on the old converted format. (This also puts all holes on the right locations).
- Use the thin lines as a guide to re-create the tracks.
- Throw away the old data, which is easiest if it’s on “unused” layers.
[Edit]
Using this method makes the probability of human error very small, because you have 2 separate paths. You have the schematic, and you have the PCB. If you can not re-reate the PCB by tracing over the old thin tracks, then you know there is some error and you have to double check your previous work.
It is a lot oft of dull and repetitive work, but not very difficult.
It’s also much less work than designing the whole project from scratch.
A design like this probably takes a month or more to design. Recreating it is less than a day’s work. I think I’d rather pay EUR150 for a complete kit to build this thing then spend a full day to re-do the project, and then still have to have the PCB manufactured, buy components, etc.
I am sure it is possible to use KiCad to convert the gerbers one way or another. But be aware that KiCad is not really designed for this task. Which means there is not really tool support here.
Any manual rework one does is always connected to the risk of human error. Plus it will take quite some time. (There is always the option of a complete redesign from the pdfs as @paulvdh explains, but that is even more work)
So maybe really first check if the original author is prepared to either share their design files or make a new export in the modern gerber format.
Also contact a few manufacturers to check if they are able to use the old gerber format. Even the manufacturer you used originally might be able to read these files. It is however likely that their automated systems do not support it. So send them a mail explaining what your problem is and ask if they have some options available.
I did a little bit of searching on github and found:
https://github.com/jgiercyk/uBITx/blob/master/uBitx_CircuitDescription_v5.pdf
In this pdf there is a schematic of the thing made with KiCad. This suggests that you may be able to find a (hopefully) complete KiCad project of this thing.
Hello
I give you news
I can open the layer files with the Viewplot application 1.5
The track is good and the circuit size is 15.5 cms.
On the other hand all the pastilles for welding are very small and all the same.
so the pb must come from the DCODES file
The traces do not look correct to me and the filled areas are not fille. Looks the same as in kicad.
Here the dcode file:
Beginning:
Dcodes for job …ax\r2win\Cad Jobs\uBITX2.5 Arduino.r2
Units :- Inches
Round Dcodes
Size Dcode Size Dcode
0.070 10 0.000 10
0.080 11 0.000 10
0.160 12 0.000 10
0.010 13 0.000 10
0.012 14 0.000 10
0.050 15 0.000 10
0.045 16 0.000 10
0.055 17 0.000 10
0.060 18 0.000 10
0.065 19 0.000 10
0.024 20 0.000 10
0.001 21 0.000 10
0.000 10 0.000 10
0.000 10 0.000 10
0.000 10 0.000 10
0.000 10 0.000 10
Square Dcodes
Size Dcode Size Dcode
0.030 10 0.000 10
0.000 10 0.000 10
0.000 10 0.000 10
0.000 10 0.000 10
0.000 10 0.000 10
0.000 10 0.000 10
0.000 10 0.000 10
0.000 10 0.000 10
0.000 10 0.000 10
0.000 10 0.000 10
0.000 10 0.000 10
0.000 10 0.000 10
0.000 10 0.000 10
0.000 10 0.000 10
0.000 10 0.000 10
0.000 10 0.000 10
Target marker dcode
37
Profile dcode
21
End
Plotview can’t read the file
Message 0 aperture have been found
I tried to eliminate all the useless information from this file. It’s the same. I would need an example of this type of Dcodes file
I’m surprised at your answer.
Everything overlaps well, and the pitch of the integrated circuits is well at 2.54mm
The size of the circuit looks good. 15.5 cms
For me the route looks good.
It is true that the mass seems more made of lines than a full set.
But it is an HF circuit, it may be so (?)
I think all pellets remain in a standard state since the aperture file is not read correctly.
ddt
