Design Spark 10.1 NC Drill Data Gerber Plot not lining up with other plots

[ThomsCircuit]

This is from JLCPCB
When i uploaded a project for manufacture it had no preview.
In a chat the agent said this file was not lining up.
I re ran the process and left out the plot and it worked.
I still have version 9.04 of design spark and this plot is not part of the process.
I believe this new plot may have been added during an update from 10 to 10.1

Why was this added? What does it do? Why does it cause this problem?

 

[eTech]

I believe this new plot may have been added during an update from 10 to 10.1"

I just updated 10.0 to 10.0.1. Is this what you meant?
If so, the update did not add any new plots to my projects.

I read the changelog for 10.0.1 and there was a change to manufacturing plots but the log doesn't elaborate much.
"-Various improvements to manufacturing plots"

Why was this added? What does it do? Why does it cause this problem?

NC stands for "Numerical Control". Historically, its a file coded to be read by automatic drill machines and is still used today. Basically, they use the NC file to create any holes (or slots, if any) on the board. You already have an NC file and I believe its the "Gerber Drill Data" file. Its not actually Gerber but its in Excellon drill format. I don't know where the new plot came from, but its even more interesting that its doesn't align with the other plots. You can delete that plot file if you like.

 

[ThomsCircuit]

but its even more interesting that its doesn't align with the other plots.

Be nice to figure this out. lets take is slow so i dont bombard you with too much at once.
here are manufacture plot screens for ver 9 and ver 10.
See how ver 9 has no NC file option where ver 10 does.

now i will need to know when ver 10 was released so we can compare this next item. but i have plots created under ver 9 and when i examine the files generated the NC file is included. Seems interesting that there is no option for it during the file manufacturing creation but it is included in the output.

I can upload to you any files you need if it would help you solve this.
Or you can give instructions how to generate the output files again. maybe i missed something or forgot a step. but i do not see where i have any way to edit the PCB design to prevent this. Anyway here are the screenshots for ver 9 and 10

 

[ThomsCircuit]

You can delete that plot file if you like.

deleting the file solved the problem when i upload to JLCPCB.com but still curious what the deal is here.

 

[Nigel Goodwin]

deleting the file solved the problem when i upload to JLCPCB.com but still curious what the deal is here.

Presumably it's a file for other manufacturing methods, that JLCPCB doesn't use.

 

[eTech]

Be nice to figure this out. lets take is slow so i dont bombard you with too much at once.
here are manufacture plot screens for ver 9 and ver 10.
See how ver 9 has no NC file option where ver 10 does.

Actually--

Version 9 has one NC drill file:
Drill Data - [Through Hole]

Version 10 has two NC drill files:
Gerber Drill Data - [Through Hole]
NC Drill Data - [Through Hole]

Gerber format and Excellon drill format are two entirely different file types. So "Gerber Drill Data" is a somewhat misleading filename.
I recommend that you delete "NC Drill Data", then rename "Gerber Drill Data - [Through Hole]" to "Drill Data - [Through Hole]" for Version 10.

now i will need to know when ver 10 was released so we can compare this next item. but i have plots created under ver 9 and when i examine the files generated the NC file is included. Seems interesting that there is no option for it during the file manufacturing creation but it is included in the output.

The Manufacturing outputs have plots defined by default. So the plot definitions for V10 pre-existed before your update.
They have been correct for me before and after I've updated the software.

I can upload to you any files you need if it would help you solve this.
Or you can give instructions how to generate the output files again. maybe i missed something or forgot a step. but i do not see where i have any way to edit the PCB design to prevent this.

I wouldn't worry too much about the additional plot file, just delete it and move on. If it re-appears on its own, then we need to figure out why.
BTW- If you delete it from one project, it won't affect other projects, so if it exists in other projects, you may have to do each as needed.

Also-
Some advise...
If you update your PCB software, its best to move your designs to the newer software and not use the old software anymore to prevent "Versionitis".

(I wouldn't say this if you are trading files with a customer who may have an older PCB version)

 

[ThomsCircuit]

Also-
Some advise...
If you update your PCB software, its best to move your designs to the newer software and not use the old software anymore to prevent "Versionitis".

I dont use the older version. it did not delete during the last major update so i just let it be.
ill just exclude the NC file from the plot generator as you suggest. If its not an issue then i wont worry about it. Thank you eTech.

 

[ThomsCircuit]

As you suggested. Ill submit my plot files to JCBPCB this way

 

[ThomsCircuit]

Question: should the "Drill Data" file be type Exceleron or Gerber?
Here is a plot i created in feb of last year. See how the file name is called "Drill Data"? thats just how it was outputting the plots before the update. And its type is Excelleron.

 

[ThomsCircuit]

I tried both ways (DRL & GBR).
Only when the Drill Data is of type GBR that it renders correctly in the online viewer

JLCPCB Online Gerber Viewer

 

[eTech]

I tried both ways (DRL & GBR).
Only when the Drill Data is of type GBR that it renders correctly in the online viewer

JCBPCB Online Gerber Viewer

That is just the way their viewer is set up to work. JLCPCB doesn't care about the filename, just the file extension.
The Drill Data file is still Excellon format, not Gerber.

Here is an sample of a set of files that I renamed to satisfy JLCPCB's naming standard:

The filename reflects my own board numbering scheme. "D" stands for "Detail" and represents the FAB detail. The trailing "A" is a revision letter.
In addition, my Schematic files begin with "S", Projects begin with "P" (including the project folder).

 

[eTech]

Question: should the "Drill Data" file be type Exceleron or Gerber?
Here is a plot i created in feb of last year. See how the file name is called "Drill Data"? thats just how it was outputting the plots before the update. And its type is Excelleron.
View attachment 135467

When I talk about a drill data file, I'm referring to the file content format, not filenames or extension names.
The Drill Data file should always be Excellon format. JLCPCB has their file naming requirements but the file content for most of the files is Gerber EXCEPT for the Drill Data file.

 

[ThomsCircuit]

The Drill Data file is still Excellon format, not Gerber.

So i compared two Drill Data files. DRL and GBR extensions. When viewed with notepad the content is not the same.
When you say "file content" i assume you are referring to what im showing here.
I have no problem uploading the drill data file as an Excellon DRL type but their viewer cant read it properly. Only if I upload the GBR version does it render.

top Excellon
bottom Gerber

 

[ThomsCircuit]

Only if I upload the GBR version does it render.

and if it does not render i cannot place the order. Just so we are clear that this is not just about the gerber viewer at JLCPCB

 

[ThomsCircuit]

The Drill Data file should always be Excellon format. JLCPCB has their file naming requirements but the file content for most of the files is Gerber EXCEPT for the Drill Data file.

I want to be sure you know that i completely understand what you are saying. all files are GBR. Drill Data is DRL. Be happy to do it and be done with it. however...
Im adding this image so you can see that if i select Execllon for the export type it gives it the extension DRL.
If I upload that to JLCPCBit is not usable.
Now the update to Design Spark made slight improvements to this tool. It renamed Drill Data to Gerber Drill Data. Perhaps it must be exported as a Gerber and not Execllon in order to work.
I mean i feel kinda silly but back when i uploaded my first board to JLCPCB i had zero issues. I selected the files as you instructed , pressed run, then uploaded them. It worked. i got 20 boards and it all worked out. Since then ive uploaded 3 more projects again with zero issues. now we got this mess and you and i are left to make sense of it.
As Walter Kornbluth said in the movie in Splash (1984) - What a week I'm having!

DS ver 10.0.1 with suggested changes

 

[eTech]

Hello,

This is the naming scheme from JLCPCB's own website:

Now...I can't speak for JLCPCB. All I can say is that in the past I've submitted drill data files with either the .DRL extension or .XLN. The .DRL file extension renders in their viewer but I haven't located a .XLN file that has rendered in my past orders. But the point is that BOTH files contain excellon drill data so BOTH should render. This is why I stated its probably their viewer. Maybe their viewer requires the file extension to be .DRL or .GBR. You should ask JLCPCB.
To be honest, I never even paid any attention to whether or not the files appear in their viewer. I always view and verify my files with my own GBR viewer (DFMNow) before zipping them up an submitting them, and I've never had any problems.

By the way, if you have a thru hole board, there will be at least one, and maybe two, drill files. One for plated thru holes, and one for non-plated thru holes.

The image you show in #15 for the "Drill Data - [Through Hole]" file looks correct to me.

 

[ThomsCircuit]

The image you show in #15 for the "Drill Data - [Through Hole]" file looks correct to me.

Thank you .
I ran a test.
here are two NC.drl files. You can see what 10.0.1 added to the NC file. Some reference notes. they are supposed to be ignored by the viewer but they are not because i uploaded this file once with the additional info and again with the info removed. The manually modified file rendered in their gerber viewer.

These are from the same project that were compiled under version 10.0 in september and then under 10.0.1 in january

This is what i removed from the .DRL file
-------------------------
;#@! TF.GenerationSoftware,DesignSpark,DesignSpark PCB,10.0.5344
;#@! TF.CreationDate,2022-01-04T23:26:32+05:00*
;#@! TF.FileFunction,Plated,1,2,PTH
;FILE_FORMAT=3:5
;TYPE=PLATED
-------------------------

 

[eTech]

Thank you .
I ran a test.
here are two NC.drl files. You can see what 10.0.1 added to the NC file. Some reference notes. they are supposed to be ignored by the viewer but they are not because i uploaded this file once with the additional info and again with the info removed. The manually modified file rendered in their gerber viewer.

These are from the same project that were compiled under version 10.0 in september and then under 10.0.1 in january
View attachment 135476
This is what i removed from the .DRL file
-------------------------
;#@! TF.GenerationSoftware,DesignSpark,DesignSpark PCB,10.0.5344
;#@! TF.CreationDate,2022-01-04T23:26:32+05:00*
;#@! TF.FileFunction,Plated,1,2,PTH
;FILE_FORMAT=3:5
;TYPE=PLATED
-------------------------

That's good info...

You should report that to both DSPCB and JLCPCB.

Good work....

 

[ThomsCircuit]

Rendering in their gerber viewer with and without the NC drill.DRL file

 

[eTech]

Rendering in their gerber viewer with and without the NC drill.DRL file
View attachment 135478View attachment 135480

Turn off the other layers so we see only the NC file and show the result.