Community
Fusion Electronics
Working an electronics project and need help with the schematic, the PCB, or making your components? Join the discussion as our community of electronic design specialists and industry experts provide you their insight and best practices.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

ODB output data contain wrong silkscreen

6 REPLIES 6
Reply
Message 1 of 7
mechamania
320 Views, 6 Replies

ODB output data contain wrong silkscreen

Hi,

When uploading the output zip file to Eurocircuits to manufacture PCBs it seems that Eurocircuits looks at the ODB files for ths silkscreen. And this ODB contains wrong data! It contains the layers as indicated in the layers table. But also the tDoc layer while this is not specified! The gerber file for the silkscreen on the other hand is correct.

 

6 REPLIES 6
Message 2 of 7

Hi mechamania,

Firstly thanks for using the ODB++ output.

Regarding the silkscreen issue you are seeing I have to say that I am not sure why that would be the case without seeing the design. Regarding the tDocu layer this is added as default in the CAMJOB template file that is used if you didn't create your own CAMJOB. The way to remove this layer is by opening the CAM Processor UI dialog and after the CAMJOB template is loaded you can select the silkscreen_+_top layer and from the Layers tree remove the tDocu layer then save the customized CAMJOB. Then you can generate the ODB++ output by using the Export command (from the ODB++ tip level tree node) or by choosing the Process Job button (if you want to generate all outputs).

Moreover we have tested the ODB++ output comprehensively using the ODB++ Viewer application and I haven't seen any issues regarding the silkscreen.

I could have a quick look into your design and see what can be done if you wish. My email address if you want to send the design is constantin.popescu@autodesk.com

 

Kind Regards,

Constantin Popescu

 



Constantin Popescu
Principal Software Engineer
Message 3 of 7

This is how the silkscreen is generated:

 

CaptureS.JPG

The problem is that when processing this, The gerber files contain the correct silkscreens, while the ODB files have the additional tDoc layes.

 

 

 

 

Message 4 of 7

Hi mechamania,

Thanks for your response.

Firstly the difference happens because the ODB++ CAMJOB template (loaded when the CAM Processor UI opens) contains tDocu layer apart from tPalce and tNames. The ODB++ template SilkScreen layers are not identical with the Gerber ones in terms of the layers selected for output. I can see this to be a mistake on my part when I implemented the ODB++ output so in the mean-time the way to make the ODB++ and Gerber identical you'll need to remove the tDocu layer manually from the silkscreen_+_top layer and bDocu layer from silkscreen_+_bottom layer and save the CAMJOB configuration to a new .cam file that you can use anytime.

Please see the attached picture (ODB-Silkscreen-UpdateLayers.png) for more details. I will remove the tDocu and bDocu from the default templates for SilkScreen and the fix will be available in the next minor update.

I hope this helps.

Please let me know if you have any other questions.

 

Kind Regards,

Constantin Popescu



Constantin Popescu
Principal Software Engineer
Message 5 of 7

Hi mechamania,

One more thing I forgot to mention after saving the CAMJOB containing the changes to the ODB++ silkscreen layers next time you open the CAMProcessor UI you need to use this new .cam file instead of using the default template that is loaded automatically. In order to do that you need to use the Load job file button in the upper left corner on the right side of the CAM Job Name edit-box and from the pop-up select the Open CAM File... command or the Recent CAM jobs command (this contains the most recently used .cam files and the .cam that you created should be there) and your .cam file will be loaded containing the changes you made to ODB++ Silkscreen layers.

 

constantinpopescuXD3CL_0-1630114822213.png

 

Kind Regards,

Constantin Popescu



Constantin Popescu
Principal Software Engineer
Message 6 of 7

Thx for the explanation.
To be sure the gerber files are the same as the ODB files to I always have to edit the ODB layer specifications seperately?
The zip file which is the result of the processing, contains both the gerber and ODB files. I send this to the manufacturer and I do not know in advance which they will use (gerber or ODB, or both?). In fact it turned out they used the ODB files for the silkscreens and I got wrong silkscreens. Suppose there are differences in the copper layers. That would be very bad.
The manufacture preview in Fusion shows the silkscreen without tDoc layers.  I assumed that is shows what will be generateted for the zip file.
So how can I absolutely be sure that the zip file contains correct information and that this is exactly as shown in the manufacter preview window?

 

Message 7 of 7

Hi mechamania,

Regarding your questions here it is:

"To be sure the Gerber files are the same as the ODB files to I always have to edit the ODB layer specifications seperately?" - the answer is you only need to edit the ODB++ layers configuration ones, for the Silkscreen layers remove the tDocu (Top side) and bDocu (Bottom side) layers then save the ODB++ .cam configuration and then anytime you want to generate your CAM outputs use the saved .cam configuration file instead of the default template (you should have one .cam configuration file for each design that you work on, this is the way I always work, the default templates supplied with Fusion Electronics are just starting points and they cover the most basic configurations and cannot be used always out of the box, an example is blind, buried via boards). I would also strongly suggest that you never send out CAM data that you haven't thoroughly checked so you can be 100% sure it is correct and it matches you intent. For Gerber, NC Drill you can use any free CAM Viewer like: GCPrevue, GerbTool, ViewMate or any other CAM tool that offers a free viewer. For ODB++ you'll need to use the ODB++ Viewer application available on Windows only, you can get it from here http://odbplusplus.com/design/downloads/odb-d-viewer/ (this is the de-facto ODB++ Viewer built by Valor now a part of Siemens). If you work on a Mac then your best choice is Cuprum but the ODB++ support is not free.

"Suppose there are differences in the copper layers. That would be very bad." - There are no differences in the copper layers between Gerber and ODB++ in the default .cam configuration template files but even if there were any you should always check what data will be generated before sending the CAM data to your manufacturer, this is the rule of thumb that I always follow and will save you a lot of grief in the long run. The cam data is too important to assume that the EDA tool is always doing the right thing with the out of the box configurations.

"The manufacture preview in Fusion shows the silkscreen without tDoc layers.  I assumed that is shows what will be generated for the zip file." - the manufacture preview is just a nice picture of how the manufactured board will look like and it doesn't match what is in the CAM output for different reasons (example solder mask) so you shouldn't base you decisions on that (I would never do that). Always check what data is exported before sending it to manufacturing.

"So how can I absolutely be sure that the zip file contains correct information and that this is exactly as shown in the manufacter preview window?" - as I mentioned above the best is to use a 3rd party free CAM Viewer to check the Gerber, NC Drill data and the ODB++ Viewer to check the ODB++ data. Also keep in mind that the CAM data is not identical with the image displayed in the manufacturer preview, and that's because for example the solder mask is negative.

So in short you should always check your CAM data before sending it to manufacturing in order to make sure it contains all the outputs you intended to be there. Never assume anything about the EDA tool that is generating the data.

Hope this helps.

 

Kind Regards,

Constantin Popescu



Constantin Popescu
Principal Software Engineer

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report