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: 

How to export the 2D PCB outline?

7 REPLIES 7
Reply
Message 1 of 8
anthonyEX9NB
537 Views, 7 Replies

How to export the 2D PCB outline?

In Eagle 7.7.0 I could export a DXF file that represented the 2D PCB outline along with milled cutouts and holes. I imported the DXF file into Microsoft Visio, in which I created a panelization drawing for my PCB fab house. I can manipulate the individual PCB outline into multiple versions to show how I want the panel to be made.

 

Is it possible to do this in Fusion 360?

 

I tried pushing the 2D PCB into the 3D PCB and then making as many objects in the 3D model invisible as possible. Then I tried exporting this into an DXF file. However, the DXF file is 95 monstrous megabytes and Visio takes a very long time to import this file. In fact, the import into Vision just keeps going. I expect that the import will not be successful.

 

I have read reports from others that say trying to panelize a design in Fusion 360 is so difficult that it is not worthwhile even trying.

7 REPLIES 7
Message 2 of 8
anthonyEX9NB
in reply to: anthonyEX9NB

Apologies. When I said the exported DXF file was 95 MB, I meant that it's 95 GB. It's no surprise that Viso chokes when trying to import this large a file.

Message 3 of 8

Hi @anthonyEX9NB ,

 

Thank you very much for asking.

How about try this workaround below? It's not very straight forward, but it should help you. 

 

1. Open 2D PCB in Fusion

2. File > Export it into .fbrd or .brd format to local

3. File > Open the exported local .fbrd or .brd file which will have no link information with schematic file

4. Delete all the things you don't need in the 2D PCB but only leave the outline

5. Push to 3D PCB 

6. Save the 3D PCB

7. If there is no hole in your outline, then you could: In 3D PCB > File > Export to .dxf format, that's it.

8. If there is hole in your outline, then suggest to In 3D PCB > File > Export to STEP format to local > Open the exported STEP file > Create a sketch and project the top face to this sketch > Right click sketch in browser > Save as DXF, that's it.

 

Hope it helps a little.

 

Best regards,

Helen



Helen Chen
Principle QA for Fusion 360 Electronics
Message 4 of 8
anthonyEX9NB
in reply to: anthonyEX9NB

I tried your solution, but I don't think I'm doing it exactly right.

 

I get down to steps 7 and 8 in your solution. When I export to a DXF file, I think the DXF file is still a 3D representation of the stripped down PCB. Visio cannot import this DXF file - Visio reports that the file is in a format it can't handle.

 

My assumption is that I need to be able to creat a 2D DXF file for import into Visio. I think I need to be able to convert the 3D model into a 2D drawing, and then convert the 2D drawing into a DXF file for importing into Visio.

 

I am not proficient with the 3D modelling part of Fusion 360 (I am an electrical engineer) so solutions involving 3D modelling will require more description, please.

 

As a work around, starting with the Layout Editor in Fusuion 360 I export the layout as a BRD file. I can then open this file in my version of Eagle 7.7.0.  There are a bunch of errors because Eagle 7.7.0 can't understand the new features of Fusion 360, but there is still an outline with holes and items on the milling layer. Then I can export the BRD to a DXF which I can then import into Visio.

 

My work around is not ideal because when Eagle 7.7.0 creates the DXF file, the board outline is made up of many line segments, and the DXF conversion doesn't necessarily have the exact same coordinates for line segment endpoints (probably due to rounding, or something). So the resulting outline in Visio isn't a closed polygon and I can't fill the polygon in Visio. But at least I have a PCB outline.

Message 5 of 8
anthonyEX9NB
in reply to: anthonyEX9NB

Oh man!! I am such a dummy!

 

With Eagle 7.7.0 I had to export the PCB outline so that I could make a drawing to show the PCB fab how I wanted the panel to be made. I used Microsoft Visio to create this drawing because I couldn't make drawings in Eagle 7.7.0.

 

But now that I am using Fusion 360 I should be able to make panelization drawing right in Fusion 360 ... because Fusion 360 is also a drawing and 3D modelling tool! I just need to learn how to make drawings in Fusion 360.

 

Can you please suggest the best way to take the PCB outline, make copies of it, and place the copies fixed distances apart?

Message 6 of 8

Hi @anthonyEX9NB ,

 

I hope you're doing well. You could proceed in the following way

1. Start a new design

2. Insert your 3D PCB into this new design

3. On the top left switch from the design workspace to the drawings workspace.

4. Now in the drawing you can insert the top view(which will have the outline in it) multiple times.

 

The drawings environment is pretty straightforward to use but reach out if you run into problems.

 

Best Regards,



Jorge Garcia
​Product Support Specialist for Fusion 360 and EAGLE

Kudos are much appreciated if the information I have shared is helpful to you and/or others.

Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.
Message 7 of 8
anthonyEX9NB
in reply to: anthonyEX9NB

@jorge_garcia2 , To make this panelization drawing I need to be able to place copies of the board outline at specific distances from each other. I may need to rotate some of the board instances in the panel, and I may need to flip some of the board instances over so that the bottom face is showing instead of the top face. And I will need to add handling rails to the panel.

 

So I think I may need to make a copy of the 3D PCB in a new design and remove all the components so the panel design isn't too many giga-bytes. Then I should be able to make as many copies of it as I want and distribute each copy as I need to create the panel. Further, I can add handling rails to the panel. Then I can psuh this 3D panel to a 2D drawing and add text and instructions as required.

 

So I think I need to learn how to do some basic 3D modelling, right?

Message 8 of 8

Hi @anthonyEX9NB,

 

It never hurts to learn so I don't want to dissuade you from learning 3D modeling. However, it pays to step back and see if there is a better way.

 

If you need to spec out the full panel it may be best to do it in the 2D PCB. Here's how I would handle it, keep in mind this is a workaround so it's a little bit painful.

1) Save a copy of the board as it's own file that way you can leave the original intact and unmodified.

2) In the copy go to preferences > Electronics and uncheck the board shape feature. 

3) Run the Panelize.ulp by going to Automation and then clicking the ULP icon. This ULP copies all of the reference designators as simple text to other layers so that they won't change once you start making copies of the design.

4. Now you can make copies of the board and lay them out on the panel 

5. THen you can draw any supplementary features.

 

I know the above is a lot and we want to improve this, but this is the situation for now. Just a reminder, once you are done make sure to go back and re-enable board shape features otherwise you won't be able to produce 3D PCBs for your other designs.

 

Let me know if there's anything else I can do for you.

 

Best Regards,



Jorge Garcia
​Product Support Specialist for Fusion 360 and EAGLE

Kudos are much appreciated if the information I have shared is helpful to you and/or others.

Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.

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

Post to forums  

Autodesk Design & Make Report