JLCPCB and KiCAD?

[phil from seattle]

I recently switched from Eagle  to KiCAD and yesterday sent off a my first board designed with KiCAD to be made.  I checked the gerbers with gerbv and all the layers lined up. But I got a fairly cryptic note back from their tech

Hi Sir,

Well got your order with many thanks~

Sorry to bother you, but there is an issue that we want to confirm with you before proceeding.

As shown below, please kindly doubt check whether the tl layer is normal or not ? it is ok to fabricate the board follow your current file ?

We can cancel order without refund to let u fix it and then replace files if that is a mistake.

Your early reply will be highly appreciated!

Thank you so much!

with the attached image. It looks like there might be an origin issue but I'm not seeing it in gerbv (or other viewers). OSHPark is ok with the gerbers as well. I cancelled the build but am a bit at a loss to understand what the problem really is/was.  Also, I do not understand their instructions as there seems to be no way to change the gerbers without just submitting a new job. 

Any insight would be appreciated.

[phil from seattle]

Here is gerv showing top/bottom/inner1/inner2. They all line up. [edit]Inner2 is the ground plane so I omitted it. It "lines up" because it goes everywhere[/edit]

[retiredfeline]

Submitting a new set of files is done by emailing them a zip archive. Yes, with these fabs often there is no method to change the submission online so it's done manually.

Sorry I don't understand the message either, but it looks like a stray trace maybe created while moving the origin? Any chance you can post the file for that layer? Also the filename shown in their message doesn't match what is usually generated by KiCad, it's usually of the form projectname-F_Cu.gtl, when you have checked the box Use Protel filenames. Did you rename the files yourself? Did you include a stray file in the zip by accident?

[janoc]

JLCPCB has this:

https://support.jlcpcb.com/article/44-how-to-export-kicad-pcb-to-gerber-files

Make sure that you export the files using their settings - gerbv will load and show a lot of things correctly, their system may not. There are plenty of variants and conventions around gerber files, so it pays to follow the fab's instructions.

I have sent KiCAD generated files to JLCPCB without issues before, so KiCAD isn't really a problem.

[phil from seattle]

No stray file.  I pulled the zip file from them so it is exactly what they used.

I submitted the same zip file to OSHpark and their renderings all look perfect.

I did get a lot of error messages in gerbv but I get them with eagle too.  The resulting renderings have always looked ok.

Here's the 4 layers in a zip file.

[phil from seattle]

Yes, I followed their instructions.

[S. Petrukhin]

Submitting a new set of files is done by emailing them a zip archive. Yes, with these fabs often there is no method to change the submission online so it's done manually.

When I was faced with the need to replace Gerber, the "upload Gerber" button appeared in the suspended order, I did not send it by e-mail.

[retiredfeline]

One thing I noticed it that your Gerbers seem to have been generated with Use X2 extensions. This can cause problems with some fabs. Here's what the start of one of my projects looks like:

Code: [Select]

G04 #@! TF.GenerationSoftware,KiCad,Pcbnew,5.1.5-5.1.5*
G04 #@! TF.CreationDate,2019-12-29T19:55:11+11:00*
G04 #@! TF.ProjectId,inchdigits,696e6368-6469-4676-9974-732e6b696361,rev?*
G04 #@! TF.SameCoordinates,Original*
G04 #@! TF.FileFunction,Copper,L1,Top*
G04 #@! TF.FilePolarity,Positive*
%FSLAX46Y46*%
G04 Gerber Fmt 4.6, Leading zero omitted, Abs format (unit mm)*
G04 Created by KiCad (PCBNEW 5.1.5-5.1.5) date 2019-12-29 19:55:11*
%MOMM*%
%LPD*%
When X2 is not selected, the metadata has been turned into comments in G04 codes.

There seem to be two tutorials, one for Kicad 4 and a newer one for Kicad 5.1.5. The one for Kicad 5.1.5 leaves the X2 unchecked.

[phil from seattle]

Submitting a new set of files is done by emailing them a zip archive. Yes, with these fabs often there is no method to change the submission online so it's done manually.

When I was faced with the need to replace Gerber, the "upload Gerber" button appeared in the suspended order, I did not send it by e-mail.

Hmmm, no button showed up for me. and the tech said she couldn't substitute my new gerbers.  sigh...

[phil from seattle]

As I recall, X2 was unchecked but I could easily be wrong.  I will walk through the process again.  I have a smaller board ready to go - probably should have done it first.

The whole v4 vs v5.1 is kind of a problem for Kicad - so many things changed.  But I digress...

[retiredfeline]

Kicad 4 has been obsolete for a while, but unfortunately a lot of tutorials and webpages refer to it, confusing new players. Also causes problems with people who upgrade and have stray files from 4.

[retiredfeline]

Another interpretation of that cryptic message is the tech drew that red line to draw attention to the origin far away from the board area which shouldn't really be an issue but they thought it might be.

[phil from seattle]

Yeah, I wondered if that was the issue - maybe she was new on the job?  The whole Kicad origin not being at the corner of the PCB has been nagging at me for a while now.  Everything I read says it isn't a problem, though.

[S. Petrukhin]

Submitting a new set of files is done by emailing them a zip archive. Yes, with these fabs often there is no method to change the submission online so it's done manually.

When I was faced with the need to replace Gerber, the "upload Gerber" button appeared in the suspended order, I did not send it by e-mail.

Hmmm, no button showed up for me. and the tech said she couldn't substitute my new gerbers.  sigh...

Your order has probably already been sent to production by the system. But the manager was able to catch it before the machines started working and asked to send it by e-mail to manually replace it.

I can't show this button now, it's no longer there, but it was there (see the picture).

[S. Petrukhin]

Maybe the arrow points to some lost element, a hole, a piece of track outside the PCB?
Did you do a DRC check?

[phil from seattle]

Maybe the arrow points to some lost element, a hole, a piece of track outside the PCB?
Did you do a DRC check?

I thought of that but nothing shows up in kicad or gerbv.

Yes, I do DRC frequently when I'm down to the last few traces, tweaking things to look better or make even the simplest change. Learned that the hard way years ago. I have put quite a few boards through 5 different PCB Fabs, definitely not my first rodeo...   I have done 12 different boards through JLCPCB so I am somewhat familiar with their process.  Though, they continue to surprise me.  I think their processes are evolving pretty quickly. 

[S. Petrukhin]

Maybe the arrow points to some lost element, a hole, a piece of track outside the PCB?
Did you do a DRC check?

I thought of that but nothing shows up in kicad or gerbv.

Yes, I do DRC frequently when I'm down to the last few traces, tweaking things to look better or make even the simplest change. Learned that the hard way years ago. I have put quite a few boards through 5 different PCB Fabs, definitely not my first rodeo...   I have done 12 different boards through JLCPCB so I am somewhat familiar with their process.  Though, they continue to surprise me.  I think their processes are evolving pretty quickly.

Ask them to help you figure it out. There are responsive people and smart guys. Maybe this is some mistake on their side, they will find and correct it - other people will not have to suffer with it.

[atommann]

Hi Phil,

Your file is in X2 Gerber format and the CAM software JLCPCB is using cannot handle it. (Or a software compatibility issue)
Please try to generate the new file without the option "Use extended X2 format" being checked.
(I checked your file in JLCPCB's CAM software and see the same issue)

--
Atommann from JLCPCB

[retiredfeline]

Phil, well there you go.

There's a plugin that may help you in future: https://github.com/g200kg/kicad-gerberzipper to get the right settings for each fab. It has presets for major fabs or you can add your own.

[48X24X48X]

More often than not, it is not the CAD software issue with gerber file generation but people don't take the time to understand the standard properly and what is needed for the factory to process. I guess people expect 1 button press generation without any check boxes or options.

[phil from seattle]

More often than not, it is not the CAD software issue with gerber file generation but people don't take the time to understand the standard properly and what is needed for the factory to process. I guess people expect 1 button press generation without any check boxes or options.

Or perhaps there are so many options and conflicting instructions that it is hard to know what is correct.

[S. Petrukhin]

More often than not, it is not the CAD software issue with gerber file generation but people don't take the time to understand the standard properly and what is needed for the factory to process. I guess people expect 1 button press generation without any check boxes or options.

Or perhaps there are so many options and conflicting instructions that it is hard to know what is correct.

Or use EasyEDA to order boards and components at a reasonable price in a couple of clicks without checking the boxes. 

And agree: guys at JLCPCB are great-they always help and take care of users in the forum. 

[yaqwsx]

You can make your life easier with a tool I recently created: KiKit. You can automatically export manufacturing data for a given fab house with KiKit. KiKit will use the correct settings.  Read more about the fab command of KiKit. PS: It can also export data for PCB assembly.

[Harjit]

Does anyone have the design rules for JLCPCB for two and four layer boards that can be imported into KiCad?

[janoc]

Does KiCAD even allow importing the rules from outside? I believe they are stored in the project.

EDIT: there is, indeed, an Import button allowing to import the settings from another project. Never saw that before.


You can probably use this information and just set up the project yourself:

https://github.com/ayberkozgur/jlcpcb-design-rules-stackups

Then save it as an empty project so that you can have a template to copy next time.