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: 

Fusion 360 Electronics - ODB++

21 REPLIES 21
SOLVED
Reply
Message 1 of 22
mario.brizida
1887 Views, 21 Replies

Fusion 360 Electronics - ODB++

Hi;

I'm trying to use ODB++ to generate files to be sent to my PCB manufacturer.

Since it'sm my first time, I'm having a lots of difficulties and questions, like how I setup  to export Vcut data, info regarding layer and copper thickness, dielectic materials, colour of solder resist and silk screen, etc... etc.

Do you plan to have detailed instructions to use and configure  ODB++ setup files?

 

Thank you;

21 REPLIES 21
Message 2 of 22

Hi @mario.brizida ,

 

Thank you very much for asking.

Could you please check this blog post and see anything else is still unclear for you?

https://www.autodesk.com/products/fusion-360/blog/fusion-360-odb-export/

 

Hope it helps.

Regards,

Helen



Helen Chen
Principle QA for Fusion 360 Electronics
Message 3 of 22

Hi Mario,

The answer to your questions is as follows:

1. "how I setup to export Vcut data" - there is no automatic support for V-cut, rout-tabs at the moment but it'll be added in the near future. In the meantime you might be able to add any rout data on milling layer and this is exported as ROUT information to ODB++. Then you can let the Fab House know that all your rout data is on the ROUT layer.

2. "layer and copper thickness" - we do export copper and dielectric layers thickness and the values are taken from the board layer stack-up.

3.  "dielectric materials" - there is no support for dielectric materials in Fusion Electronics ODB++ output because the board design doesn't have it at the moment (support will be added in not too distant future).

4.  "colour of solder resist and silk screen" - I am not sure how this is handled in ODB++ but if this is possible we should be able to add support for it.

If you have more questions please don't hesitate to ask and I will try to answer them. Also if you need help to set-up the ODB++ output using the current capabilities then I'll be glad to help.

I hope this helps.

 

Kind Regards,

Constantin Popescu



Constantin Popescu
Principal Software Engineer
Message 4 of 22

Hi Constantin;

Thanks for your answer. It's good to know that you are still working to improve ODB++

As I think you know, today Fusion was upgraded.

As I'm not yet working with ODB++(still with Gerber X2 untilI completely understand new format), and I needed to generate gerbers for a new pcb, and I have a X2 cam processor file configurated for what I need, I downloaded that configuratiuon file and noticed:

- It takes a lots of  time until cam processor configuration screen appears (the default one)

- When I open my own configuration file (X2), it takes again a lots of time to open

- On the top always appears ODB++ configuration, that I don't want to use. I tried to delete them by right clicking on it, but the only option I got was "Delete all", that has no effect at all.

- Even when I disable all output options of ODB++, it creates ODB++ folders when exporting (that I don't want)

- It takes a lots of time to generate the gerber files (was very quick in last versions)

 

My questions are:

1. Do you know if I can do something to decrease procesing time (that is really high)?

2. How do I disable ODB++ process (that I think is responsible for great part of time increase) in order to avoid generation of ODB++ files that I will discard. 

 

I think was very useful to publicate some user instructions for this new cam processor, with specific procedures to handle ODB++

 

Thank you

Message 5 of 22

Hi Helen;

 

Thank you for your reply.

Unfortunately the blog doesn't have the answer to my question.

 

Regards;

Message 6 of 22

Hi Mario,

It is not good to hear that you have speed issues with the CAM Outputs generation in the latest Fusion Electronics. Regarding your questions:

  1. "- It takes a lots of  time until cam processor configuration screen appears (the default one)" - we have also noticed this but only when the board document has many copper pour polygons and this is not caused by the addition of the ODB++ output. Is your file containing a lot of copper pours? We have made some changes to speed-up the filling of copper pour polygons that should've helped with the CAM Processor opening speed. We also timed the CAM Processor with ODB++ and without and we didn't notice this sort of speed drop.
  2. "- When I open my own configuration file (X2), it takes again a lots of time to open" - yes this takes pretty much the same amount of time as opening the CAM Processor in the 1st place so if that's slow then opening your custom configuration will also be slow unfortunately.
  3. "- On the top always appears ODB++ configuration, that I don't want to use. I tried to delete them by right clicking on it, but the only option I got was "Delete all", that has no effect at all." - I can see this as well and it is an oversight on my part when I implemented ODB++. The good news is if you remove all the ODB++ layers and turn off all the options the output is actually empty (no image data, component layers, eda data or netlist are generated) so no time is spent on generating ODB++ so I don't think ODB++ is the reason for the slow CAM Output generation. I am saying this because I have timed the ODB++ generation as well and I found to be very close with the amount of time it takes to generate Gerber.  
  4. "- Even when I disable all output options of ODB++, it creates ODB++ folders when exporting (that I don't want)" - Yes this is true and for now unfortunately you'll need to delete the ODB++ folder manually. I will add a ticket for this issue and we'll try to fix it in the next update.
  5. "- It takes a lots of time to generate the Gerber files (was very quick in last versions)" - as I mentioned above I don't think this is because of the ODB++ output based on our testing. Did anything change in your board or the CAM Outputs since you last generated the outputs apart from us adding ODB++ support? Also have you used Fusion Electronics to generate the CAM Outputs previously or Eagle Desktop? Also what's the time difference between the current CAM outputs generation and the previous one if you can recall (I don't need exact numbers).
  6. "1. Do you know if I can do something to decrease processing time (that is really high)?" - I can't think of anything else without seeing your design so if you are willing to send it to me I will investigate and see what can be done. My email address is: constantin.popescu@autodesk.com
  7. "2. How do I disable ODB++ process (that I think is responsible for great part of time increase) in order to avoid generation of ODB++ files that I will discard." - the answer is that you cannot disable the ODB++ output generation fully at the moment. You can remove all the ODB++ layers and turn off all the options and nothing will actually be generated. The only step that will run for ODB++ that could be time consuming is processing and filling all copper pour polygons before the ODB++ output is generated (this step is the same for Gerber).

I hope this helps and look forward to hearing from you.

 

Kind Regards,

Constantin Popescu



Constantin Popescu
Principal Software Engineer
Message 7 of 22

Hi Constantin;

 

Thanks for your detailed reply.

Time consuming is really related with polygons filling. I tried the same settings I used in Eagle and CAM processing got faster, so I think speed issue is clarified.

 

Regarding ODB++, I would like to start using it, I understand his structure and how info is managed by manufacturers (you have all info you need to understand it on Internet), I even spoke with manufacturers that told me that accept and is good for them to use that new format,  but you don't have anywhere detailed info regarding how to interact with it on Fusion CAM processor. I still have many questions of how to configure CAM with ODB++ in order to get all process automatized for each kind of pcb I need.

I suggest to follow the example of Eagle when introduced the new (at the time) X2. On Eagle manual was explained with detail how to use it , what's the function of each file and how to configure CAM to get personalized configurations.

I think Fusion Electronics is a really good upgrade to Eagle, you are doing a good job indeed. But there are some "small irritating  issues" like problems with libraries configuration, unexpected crashes, the way files are managed, and now also with ODB. I belive that some issues could be solved easily, some others (like odb) neeed more work and detailed instructions, and yet others need big corrections, like components creation. I personally use Eagle to create new libraries or create new componets, because until now Fusion in this case is a big confusion, and certainly you agree that is not pleasant to use 2 platforms to design electronics instead of a unified one.                   

 

And thats all.

 

Regards;

MB                                       

 

 

Message 8 of 22

Hi Mario,

Thanks a lot for your response and good to know that at least one of your issues has been clarified. Regarding the ODB++ configuration there is nothing to be afraid of, the out of the box configurations available for 1, 2,4 .., 16 layers should be good enough to start with. Please read the attached PDF document (ODB++ Fabrication Output.pdf) that contains details about how to use the ODB++ output including the CAM Processor as well as the available CLI commands like the new manufacturing odb command. If you encounter any issues or you have any concerns please don't hesitate to ask and I will try to help. If you can share with me the way you'd like to automate the ODB++ output generation then I will try to see what's possible with what we currently have and if there are any limitations then we'll try to fix them in the near future.

Another thing I wanted to mention is that I have fixed the issue with the ODB++ output getting generated even when no layers are configured and the fix will be available in the next Fusion360 update.

The other issues you are faced with are known by us and my collogues are actively working on making these workflows better.

I hope this helps.

 

Kind Regards,

Constantin Popescu

 



Constantin Popescu
Principal Software Engineer
Message 9 of 22

Constantin;

 

Thanks for the info. I will try to use it in a next opportunity. If I have further questions I will let you know.

It's good to know you are working on the issues.

 

Message 10 of 22

Hi Mario,

One more thing I wanted to mention, I have a couple of relatively short videos that I made while I was implementing the ODB++ output and might be worth watching even if they are not very polished. So if you want these videos please send me an email and I will send them to you. I don't think I can post them here because they are rather large (one is > 150MB in size).

Hope this helps.

 

Kind Regards,

Constantin Popescu



Constantin Popescu
Principal Software Engineer
Message 11 of 22

Hi Constantin;

 

I'm trying to use ODB++...

I'm trying to cereate a CAM configuration file for my own pcb, in order tu understand complete mechanism.

When I open CAM processor:

mariobrizida_0-1632914633800.png

 

As far as I understood, I only need ODB++ files, so I can erase all other "families" like Gerber, Drill. Assembly, drawings and legacy. Is this right?

 

Then I think I don't need to send layer comp_+top to pcb manfacturer, right? So I should erase it, but if I do so, I will get a yellow triangle signing something is wrong, so what should I do?

mariobrizida_1-1632914896155.png

The rest of odb layers I understand, except  prepeg_+top. What is it? Why  top layer is selected? What kind of info is sent to manufacturer from this layer?

 

mariobrizida_2-1632915311073.png

 

I need also to add a router + milling layer (I don't see where that info is sent from standard structure), but how do I do it? 

The layer "rout" doesn't have any pcb layer to select, doesn't allow to select a type, and I don't use pcb layer 20 to define outline... So, please help me how to configure it.

mariobrizida_3-1632915464432.png

As far as I understood, I can copy a layer (for instance solder-mask+top), change the name for "milling+routing" but then which is the right option on "Type" tab?

mariobrizida_4-1632915902965.png

I don't have any option for milling. I have it for router but in that case I'm not able to select any pcb layer.... so what do I do?

 

 

By now that's all.

 

Thank you.

 

 

Message 12 of 22

Hi Mario,

Here are my answers:

"As far as I understood, I only need ODB++ files, so I can erase all other "families" like Gerber, Drill. Assembly, drawings and legacy. Is this right?" - yes this is true you can remove all the other outputs because ODB++ includes all necessary image, drill and rout information. You can also customize the default configuration with layers that are not present by default (e.g.: milling).

"Then I think I don't need to send layer comp_+top to pcb manfacturer, right? So I should erase it, but if I do so, I will get a yellow triangle signing something is wrong, so what should I do?" -  you should not remove either of the comp_+_top and comp+_+bot layers but instead turn off the "Export EDA data (eda/data)" option from the ODB++ Options page. If you don't want to send the components then none of the EDA data will be generated (only Gerber, Drill and Rout information will be generated). This is the way the ODB++ format works you cannot remove the components only because they are linked to the eda/data as well as the netlist.

"The rest of odb layers I understand, except  prepeg_+top. What is it? Why  top layer is selected? What kind of info is sent to manufacturer from this layer?" - The layers between the signal (copper) layers are dielectric layers either Core or Prepreg they are taken from the board layer stack-up (drc command). In this case it is the core dielectric laminate on which the top copper layer sits. We only export the attributes below that ODB++ format supports for these layers and no image data because none exists:

  • .layer_dielectric - dielectric layer thickness as defined in the Layer Stackup;
  • .dielectric_constant - dielectric constant, we use a default value at the moment because we don't have real support at the moment;
  • .loss_tangent - dielectric loss tangent (dissipation factor), default value as well.

The dielectric layers information is used by 3rd party tools that use ODB++ for other purposes then fabrication (e.g.: electromagnetic simulation or signal integrity, etc.).

"I need also to add a router + milling layer (I don't see where that info is sent from standard structure), but how do I do it?  The layer "rout" doesn't have any pcb layer to select, doesn't allow to select a type, and I don't use pcb layer 20 to define outline... So, please help me how to configure it." - the rout layer contains all the defined board cut-outs and it is auto generated from the board shape. For now you can add another layer called milling_+_routing to the ODB++ configuration, please see the attached picture: Add-Milling-Layer2ODB-Configuration.png. Similarly you can add any image layers you need and are not present in the default ODB++ configuration. The only thing to keep in mind is that at the moment the Drill and Rout layers are auto-generated from the drill and rout information available in the design and they cannot be customized.

"As far as I understood, I can copy a layer (for instance solder-mask+top), change the name for "milling+routing" but then which is the right option on "Type" tab?

constantinpopescuXD3CL_0-1632956014745.png

I don't have any option for milling. I have it for router but in that case I'm not able to select any pcb layer.... so what do I do?" - yes this is the way to go the only valid Type that you can use is Document because as I mentioned the rout and drill layers are auto-generated and there is no milling type in ODB++.

I realize that this is a restriction that I haven't thought about and I'll look into relaxing it in a future update. For now you can go with the Document type and let the FAB House know that these are the milling/rout features so they can convert them to rout program.

Please let me know if you have any other questions and I'd try to help.

 

Kind Regards,

Constantin Popescu 



Constantin Popescu
Principal Software Engineer
Message 13 of 22

Hi Constantin;

 

Thanks for your answer. I will try, but I think that with your explanation I will be successful.

 

 

Message 14 of 22

Hi @mario.brizida - I know others have shared content with you, I just didn't see this Youtube Tutorial by our own Edwin Robledo. Hope this helps!

Message 15 of 22

Hi Loren;

Thanks for your video. Unfortunately, it didn't answer to my configuration questions.

For instance I use layer 125 to draw silkscreen, and inthat case how do I correctly configure ODB++ processor?

I didn't find any detailed documentation about how to configure ODB++ processor...

As far as I undestood ODB++ processo is not yet concluded, so I decided by now to use Gerber X2 format until ODB++ is stable and better documented.

 

Message 16 of 22

Hey @mario.brizida - I was able to get a response from Edwin, who sent these instructions for configuring Layer 125. Also we are grateful for your feedback so we can keep in mind when updating our documentation:

 

"Updating in the CAM processor is fairly easy if you know how to do it.  It’s a step that is not really obvious.

1 + 2: From the manufacturing Tab select the CAM Processor

3: From the ODB++ group, select the section you want to edit the layers

4: At the bottom of the ODB++ layers, use + and – to add or remove layers.

5: If adding layers, select them from this dialog box.

6: After selecting the layers press OK to complete.

 

odb-layer-125.jpg

 

 

Message 17 of 22

Loren;

Thank you for the explanation. In understood it perfectly.

But the fact is that Autodesk needs to improve ODB++ CAM configuration interface.

The main difficulties I have (as I told in anterior post) are:

 

  • If I don't use (and I personally don't use) layer 20 for routing (ex. v-cut) I need to create a "Document" job because is not possible to indicate to CAM processor that rout information is in another layer, as we can do on Gerber X2 files.
  • We don't have where to put info like dielectric or prepeg materials, like FR4 or aluminium.
  • Was also very important to have a field where to put info about silkscreen and solder resist colours, because markek is now working with several colours for both solder resist and silkscreen, and as the objective of ODB++ is to send a unique file to manufacturer with all info he needs to produce (and even assemle) the pcb, that I think is fantastic, we should have fields where to put all that info, or we fall again on Gerber x2 where we must send also an associated file with pcb constitution info.

 

Message 18 of 22

Hi, 

I've just had my first go at ODB++ export for a new supplier. They need ODB++ version 7 for their system. I can see there is an option for different formats in the CAM processor window, but the window is greyed out and set to version 8.1. Guessing there are some more files needed somewhere? 

 

Any suggestions appreciated.

 

Steve

Message 19 of 22

Hi Steve,

Unfortunately Fusion360 can only export ODB++ V8.1. The reason for this is that V7 is very different (before the ODB++ format was standardized) from V8 and would have required a lot of customization that we didn't have time for so we chose to supress it for the time being. Since we released this a year or so ago you are the 1st user to ask for V7 compatible format. I will add a feature request to our issues tracking database so we can look into implmenting this in a future release.

Please let me know if there is something else I can help you with.

 

Kind Regards,

 



Constantin Popescu
Principal Software Engineer
Message 20 of 22

Hi Constantin,

 

I just saw the documentation you posted, about the ODB++ export.

We try to automate the ODB++ conversion with an external script. 

 

Your documentation describes, that CLI and LibEagle CLI can be used to do so.

The problem is, that there is no "eagle.exe" as far as I see and I really don't know what the "LibEagle CLI" is.

Could you please clarify that?

 

Kind regards
Bernhard

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

Post to forums  

Autodesk Design & Make Report