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: 

Different GND pins are connected in PCB even though they are not in the schema

8 REPLIES 8
SOLVED
Reply
Message 1 of 9
CaptainMJ
1208 Views, 8 Replies

Different GND pins are connected in PCB even though they are not in the schema

Hi!

I have a strange problem, one of the components i use has 6 GND and multiples of power supplies of same voltage. They do not need to all be connected, just one of each or a couple should be sufficient. In my schema i connected only one, but on the PCB it shows they are all connected to each other. How can I remove these connections?

 

In the attached image you can see pin 39 GND is connected to 34 GND, but in the schema this connection does not exist. I guess this could be a feature of the component, but i have not find a way to edit that.

Best Regards,
Marcus
8 REPLIES 8
Message 2 of 9
kb9ydn
in reply to: CaptainMJ

What you can do is to create a dummy part that has no footprint.  Then when you connect it in the schematic it won't show anything on the board.  I created one that looks like this:

 

 

kb9ydn_0-1591301778575.png

 

 

The nice thing about this is that it also specifically indicates in the schematic that the pin was left unconnected intentionally.

 

 

C|

Message 3 of 9
jorge_garcia2
in reply to: CaptainMJ

Hi @CaptainMJ,

I hope you're doing well. So what's going on here is perfectly normal, even though it's not the behaviour you want. What's happening is that the GND pins are defined as POWER pins in the symbol, so by definition they are all automatically connected because of that definition.

Here's what I would do in this situation. First put only one ground symbol in the schematic, in Electronics you can assign multiple pads to a single pin. In the device editor in the Library under the connect function you'll be able to assign all of the ground pads to 1 pin. Here you'll also be able to define if they all need to connect or if it's ok if only one of them connects.

In the connect dialog you'll see a little Icon next to the connections that have multiple pins. By default it's set to all but clicking it will change it to any. For your scenario you want any.

 

AnyVsAll.png

See attached picture.

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 4 of 9
CaptainMJ
in reply to: kb9ydn

@kb9ydn Thanks, that looks like a good simple solution. Many thanks for the help!

Best Regards,
Marcus
Message 5 of 9
CaptainMJ
in reply to: jorge_garcia2

@jorge_garcia2 , many thanks for the great explanation, I suspected it was something with the component but couldn't find it earlier. Really appreciate all the help! 

Best Regards,
Marcus
Message 6 of 9
CaptainMJ
in reply to: jorge_garcia2

@jorge_garcia2 Turns out the device I'm using doesn't quite look like that, I wonder is there a problem with how the device im using is setup? See attached image.

Best Regards,
Marcus
Message 7 of 9
CaptainMJ
in reply to: kb9ydn

@kb9ydn I tried your suggestion, but seems its not possible to add such a device to my schematic, do you have any idea what I may be missing? I attached the error message.

Best Regards,
Marcus
Message 8 of 9
kb9ydn
in reply to: CaptainMJ


@CaptainMJ wrote:

@kb9ydn I tried your suggestion, but seems its not possible to add such a device to my schematic, do you have any idea what I may be missing? I attached the error message.


 

@CaptainMJ 

Oh sorry, I had forgotten about that.  You have to add the "_EXTERNAL_" attribute to the device to allow it to be placed in the schematic.  I actually made this part in Eagle and then migrated it to Fusion, but you should still be able to do it in Fusion.  If you go into the library and edit the device; you can bring up the attribute editor by typing "attribute" on the command line.  Here you need to add a new attribute called "_EXTERNAL_".  Make sure to include the underscores or it won't work.

 

Now you should be able to add the device to a schematic.

 

 

C|

Message 9 of 9
jorge_garcia2
in reply to: CaptainMJ

Hi @CaptainMJ,

I hope you're doing well. You'll have to disconnect the connections that have been made and redo them. Additionally you'll want to remove all of the GND pins from the symbol except for one. That's how you'll be able to assign multiple pads to the same pin.

Let me know if you continue to 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.

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

Post to forums  

Autodesk Design & Make Report