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: 

Representing internally connected device pins

6 REPLIES 6
SOLVED
Reply
Message 1 of 7
josh_l
682 Views, 6 Replies

Representing internally connected device pins

Hi,

 

I have created a Fusion 360 electronics library device that represents a small prototyping board that will be mounted onto my PCB via header pins as a "sub-board" kind of arrangement.

 

The sub-board has multiple GND pins. I would like to be able to connect any of my traces to the nearest GND pin and have F360 know that they're the same thing. Is there a way to achieve this by altering the design in my Library device? At the moment I get a bunch of unnecessary airwires because the PCB editor doesn't know that the multiple GND pins on the sub-board are internally connected, even though there is a path path to GND connected everywhere there needs to be.

 

I'm aware I can just hit Approve on the DRC errors - I'm just looking for a better solution.

 

Thanks in advance for your help!

 

Josh

 

6 REPLIES 6
Message 2 of 7
jorge_garcia2
in reply to: josh_l

Hi @josh_l,

I hope you're doing well. This is something you can correct in the library. Open the Device for this component and click on the Connect button on the bottom right.

Make sure that you have all of your ground pads connected to the same pin in the symbol. If you have a 1:1 pin to pad relationship this won't work so it's recommended that you assign all of the gnd pads to the same pin. Make whatever adjustments you need to make to the symbol for this to work.

When you do this you'll see a little icon show up next to the connections, to the left. If you hover over it, it will say either all or any. Left click it to change it.

In your particular case you wan Any, that means that as long as any of them are connected the netlist will be satisfied and you won't get the extra airwires.

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.
Message 3 of 7
josh_l
in reply to: jorge_garcia2

Thanks Jorge! I'll change my symbol to only have one ground pin - I think that's where I was going wrong. I just made a symbol that represented all of the physical pins, but I see now that there was no point modelling the extra ground pins in the symbol when that's more of a detail of the physical part than the schematic.

 

Cheers!

Message 4 of 7

Is the use of swap-level on the pins ever useful in this context?
Message 5 of 7
jorge_garcia2
in reply to: josh_l

Hi @roatchristopher,

 

It would be hard to find a use from swap-level in this context because you are consolidating all the ground connections onto a single pin. So swap level would imply that there is some other gnd equivalent pin that we could swap with, but that's not possible in this case because all the gnd pads have been consolidated into 1 pin.

 

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.
Message 6 of 7
roatchristopher
in reply to: josh_l

I like the idea of connecting the ground pads to a single pin, as then the schematic makes sense semantically. 

 

But, if the pins were not tied together, would it work to use swaplevel instead? 

Message 7 of 7
jorge_garcia2
in reply to: josh_l

Hi @roatchristopher,

 

I hope you're doing well. If they were not on a single pin, then you would go the old school way. One pin for each pad, swaplevel the same non-zero value for all of them and you would name them GND, GND@1, GND@2, GND@3, etc.

 

The @x syntax is important, it allows each pin to have a unique name as required but when used in the schematic the @x is dropped so you see all the pins named GND.

 

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