topic Re: Different GND pins are connected in PCB even though they are not in the sche in Fusion Electronics Forum

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

CaptainMJ — Thu, 04 Jun 2020 11:52:49 GMT

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.

Re: Different GND pins are connected in PCB even though they are not in the sche

kb9ydn — Thu, 04 Jun 2020 20:18:47 GMT

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.

Re: Different GND pins are connected in PCB even though they are not in the sche

jorge_garcia — Thu, 04 Jun 2020 20:32:44 GMT

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,

Re: Different GND pins are connected in PCB even though they are not in the sche

CaptainMJ — Fri, 05 Jun 2020 01:23:45 GMT

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

Re: Different GND pins are connected in PCB even though they are not in the sche

CaptainMJ — Fri, 05 Jun 2020 01:26:11 GMT

@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!

Re: Different GND pins are connected in PCB even though they are not in the sche

CaptainMJ — Sat, 06 Jun 2020 08:34:46 GMT

@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.

Re: Different GND pins are connected in PCB even though they are not in the sche

CaptainMJ — Sat, 06 Jun 2020 09:34:48 GMT

@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.

Re: Different GND pins are connected in PCB even though they are not in the sche

kb9ydn — Sun, 07 Jun 2020 14:54:09 GMT

@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.

Re: Different GND pins are connected in PCB even though they are not in the sche

jorge_garcia — Mon, 08 Jun 2020 21:41:06 GMT

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,