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

[eTech]

Can you post your manufacturing plot files (unmodified) so I can download and take a look?

 

[ThomsCircuit]

Modified (Edited) NC.DRL plot

Un modified Plot

Note of all the available layers here the .DRL file is not available.
Understandably so because it is not a Gerber file (GBR) however there is a difference as shown so i can assume the .DRL file is utilized but not shown in the viewer.

 

[ThomsCircuit]

just a moment i did not do that right.

 

[eTech]

Modified (Edited) NC.DRL plot
View attachment 135482

Un modified Plot

View attachment 135483
Note of all the available layers here the .DRL file is not available.
Understandably so because it is not a Gerber file (GBR) however there is a difference as shown so i can assume the .DRL file is utilized but not shown in the viewer.

That looks like the drill identification drawing. That one IS gerber.

 

[ThomsCircuit]

-------------------------------------

 

[eTech]

View attachment 135488
-------------------------------------
View attachment 135489

So....nothing unusual here....

 

[ThomsCircuit]

Can you post your manufacturing plot files (unmodified) so I can download and take a look?

So....nothing unusual here....

i wouldnt know but without the .DRL file the plot is not right so i dont think it can be left out. however... in DesignSpark if you AutoGenerate plots your prompted with an option to include 3 plots or not. one is the NC.DRL file.

 

[eTech]

i wouldnt know but without the .DRL file the plot is not right so i dont think it can be left out. however... in DesignSpark if you AutoGenerate plots your prompted with an option to include 3 plots or not. one is the NC.DRL file.

If there are not any holes/cutouts/slots on the board, then you don't need drill data.

 

[eTech]

OK...

I just finished a chat with JLCPCB.
Don't use .XLN file extension for drill data. The JLCPCB viewer has a problem displaying it.
Use .drl

So...the bottom line:
It is not accurate for JLCPCB to say the file is unusable because it doesn't render.

This is why I use my own, separate, viewer...to verify the Manufacturing polts.

 

[eTech]

This is the "poolspinnerDual555-SMDr2 - NC Drill Data - [Through Hole].drl" file - This is the correct excellon drill data file.

And it should look like this(I turned on the board outline layer (red) for clarity):

I don't know what the "poolspinnerDual555-SMDr2 - Gerber Drill Data - [Through Hole].gbr" file is for and I don't think that is needed.

This is the "poolspinnerDual555-SMDr2 - Drill Ident Drawing - [Through Hole].gbr" drill Identification Drawing. It is also correct:

 

[ThomsCircuit]

I just finished a chat with JLCPCB.
Don't use .XLN file extension for drill data. The JLCPCB viewer has a problem displaying it.

ok I dont use .XLN Never have.

NC Drill Data - [Through Hole].drl" file - This is the correct excellon drill data file.

Oh i agree. Just by removing the remarks in the files header fixed it so there ya go.

I don't know what the "poolspinnerDual555-SMDr2 - Gerber Drill Data - [Through Hole].gbr" file is for and I don't think that is needed.

Ill play it safe and include it anyhow.

It is not accurate for JLCPCB to say the file is unusable because it doesn't render.

So what happens if i ignore that JLCPCB file rendering error I have to manually input the board dimensions. If i snip the header info from .DRL the form auto . populates. I like when the program does this because it lets me know that it understands what i have uploaded. It gives me absolute assurance that the boards will be made correctly.

Im still new at this but i have once again learned a great deal about plot files. Thank you eTech
Thank you so very much for helping me to figure this one out.

 

[ThomsCircuit]

Don't use .XLN file extension for drill data.

I just realized XLN is excellron. my program uses .DRL but i get it. so during the plot generation sel the NC data file to .GBR and not Excellron? correct?

 

[eTech]

So what happens if i ignore that JCBPCB file rendering error I have to manually input the board dimensions. If i snip the header info from .DRL the form auto . populates. I like when the program does this because it lets me know that it understands what i have uploaded. It gives me absolute assurance that the boards will be made correctly.

If you use a separate GBR viewer (DFMNow or other) then you can verify the integrity of the files your self.
Their viewer won't guarantee the boards will be made correctly. For example, if you leave out a drill file, the holes won't be drilled.

When I chatted with JLCPCB, one last comment from them was "If you can view it on your (PCB) software then you should be ok" .....yeah, right.

Anyway, some food for thought....

 

[eTech]

I just realized XLN is excellron. my program uses .DRL but i get it. so during the plot generation sel the NC data file to .GBR and not Excellron? correct?

No. The excellon file should be set to "Excellon" and named "yourfilename.drl".
In the past I followed JLCPCB suggested names. .XLN was for the drill data file. But after today, better to use .drl as the drill data file extension for JLCPCB. Either the .XLN or .drl can be used and will still work for board fabrication, but the .XLN just wont be viewable in the JLCPCB viewer.

 

[ThomsCircuit]

I made the following parameter changes to the NC.DRL output that i found on the DS support site. I uploaded the plot files to JLCPCB and it rendered in their online gerber viewer.
Ive attached the plot file for anyone wishes to verify it.
Format from 2 to 1
Checked "Remove Duplicate Drill Holes"
Changed Decimal from 5 to 3

UPDATE: THIS SCREEN SHOT IS FROM THE DS SUPPORT SITE.
It is 1 year old and does not include the new parameter options from 10.0 and 10.0.1. See post #37

The .DRL data file.
For some unknown reason this renders.

 

[ThomsCircuit]

When I chatted with JLCPCB, one last comment from them was "If you can view it on your (PCB) software then you should be ok" .....yeah, right.

Anyway, some food for thought....

Should be. Thank you for helping me. I only ordered 5 boards. I feel more confident after the modifications I made to the .DRL file parameters. I havent done any more tests but i believe it was the FORMAT setting change from 2 to 1 that was the problem. Im gonna call this one solved.
Well i couldnt resist. here is a comparison between the .DRL files before and after the parameter changes.
Here is a link to the most common header commands for drill communication for Excellon files.

UPDATE: .DRL
JLCPCB can read Format Type 2 just not with the header comments in the .drl file.
But, if it is Type 1 Format JLCPCB can read the file with the comments in the file.

 

[ThomsCircuit]

A rep from DS showed how to remove the header info from the .DRL file by setting another parameter change. He also recommends using Format 1 as it produces a pure drill file i.e. no milling profiles as are available in FMT 2.
Considering that selecting format 1 and leaving the comments in the header produces a file that renders in the online gerber viewer still leaves me to believe there is an illegal character in the header when other options are selected. In my software programming days it may have been a huge problem for me but ill leave this one to DS to figure out.
Cheers Mates!