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

[CaptainMJ]

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.

[kb9ydn · Accepted solution]

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:

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

C|

[jorge_garcia · Accepted solution]

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.

See attached picture.

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

Best Regards,

[CaptainMJ]

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

[CaptainMJ]

@jorge_garcia , 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! 

[CaptainMJ]

@jorge_garcia 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.

[CaptainMJ]

@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.

[kb9ydn · Accepted solution]

---

@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|

[jorge_garcia · Accepted solution]

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,