board pin connections do not match schematic

[pblase]

I have a standard board shape and bus connections (which I should be able to use a design block for!). For some reason, the net on some of the pads doesn't match the connection to the symbol. For instance, Bus1:Pin1 is SS8 and not VBUS like it should be, and I can't seem to change it. Needless to say, the board throws all kinds of ERC errors. Any figuring out what's wrong would be appreciated. 

[jorge_garcia]

Hi @pblase,

I hope you're doing well. Thanks for posting the design. First off, I'm surprised the synchronizer runs in this design. Generally speaking the synchronizer doesn't support modules and using it on designs with modules just breaks them more.

For dealing with consistency errors, the ERC is the more surefire way. To figure what out what is wrong.

Just to be clear, you are using modules (hierarchy) not design blocks. These behave fundamentally different, so it's important to be clear in the distinction. Looking at the errors it seems your board is pretty mangled since almost all of your nets have been removed from the board, which makes me pretty confident that you have run the synchronizer on this design.

Since very little has been done so far, I would recommend starting over instead of trying to repair the file. If you don't need the benefit of modules (abstraction and nesting) then I would suggest you draw these connections on their own sheet in the schematic to simplify organizing the design.

I'm going to report this because the synchronizer should not be functioning on designs with modules.

Best Regards,

[pblase]

Thank you. What I need to do is to set up a base board with common components that can then be used in future boards, which have to mate with the first board. What I did to generate this one was take the first board and chop off everything that wasn't going to be a common component. Any advice on how to best to this would be appreciated. 

[jorge_garcia · Accepted solution]

Hello @pblase,

So the key is to save the base board as it's own board schematic pair. Then in any new design you can use the Insert Electronic Design command in the Place panel to bring in the Base board and then you build from there.

Let me know if that's clear.

Best Regards,

[pblase]

I wanted to put the module into the design block. So you're recommending simply not using the module at all? 

[jorge_garcia]

Hi @pblase ,

That is correct, for this application the module won't help you at all and will only create problems.

Best Regards,

[pblase]

Ok. I really really don't want to have to re-enter all the pins, so I moved the pins from the module into the main schematic. I had to rename and renumber everything because when I did the cut-and-paste it messed up all of the pad connections. However, now the pads are not connected to the schematic pins and I can't get them reconnected. The pads are connected to some arbitrary net and not to where the schematic says they're supposed to be. How can I get them reconnected properly? 

[jorge_garcia]

Hello @pblase,

So consistency has been broken, which is the reason stuff isn't linking correctly. Easiest way to fix this is to use the slice tool and cut the nets near the pins. This will preserve the names you've defined and then you can delete the stubs connected to the pins. Since most of the inconsistencies occur because a net has not been defined in the 2D PCB so eliminating them in the schematic will make the two consistent.

Once consistency is restored you'll be able to drag the nets onto the pins to reconnect them quickly. See the image you'll see I made a small gap in the nets to be able to preserve the naming and then remove the connection from the pins

Let me know if you continue to run into problems. You are an experienced user so I figure you kept the schematic and 2D PCB open at all times. I know pulling out a module can create some issues so that's probably the cause.

Let me know if you continue to run into problems.

Best Regards,

[pblase]

Yes, I have both PCB and schematic open. 

I did as you said and sliced the lines, deleting the segments attached to the pins. That fixed most of them, but there are still some pads that have nets associated with them, and I can't get them to delete. 

Also, when I, on the schematic, try connecting a net between the existing net segment (after the slice) and the pin, it won't connect the two. 

[pblase]

Ok. I went through and sliced all the pins and cleared things up. Now it won't let me connect to the pads at all. Is there a way to manually re-enable sync? 

[pblase]

Also, another weirdness: After I snip the pin:

When I try to reconnect the net, going from the pin to the existing trace, it doesn't reconnect when I click on the leftmost end of the trace. 

I have to go over the trace, and then remove the junction that results. 

In general, there is a problem joining with existing traces. The Junction command doesn't always work. On the Gnd and VBUS connections:

the error check kept insisting that the stub between the pin and the vertical net wasn't connected to the rest of the net, even though the segment ended right at a junction. 

[pblase · Accepted solution]

Ok, I got it fixed. Royal PITA!!! There is no easy manual method to set the signal for a pad which has disconnected from the schematic. I had to 

1) use the manual "SIGNAL" command to attach a signal airwire to the pin. Since you can't have a one-ended airwire, I had to run it to another pin. This will assign the signal "S$1" to both pins. 

2) Route a trace between the two pins. Put at least two bends in it so that you have three segments. This makes the next step easier. 

3) "Slice" the trace in the middle and delete the two resulting stubs, leaving two stubs, one on each pin. One will now be labeled "S$1" and the other "S$2". 

4) You can now use the "NAME" command to rename the two stubs to the proper names, matching the schematic.

You have to leave all of the named stubs in place until final routing. Once all pins that lack a signal have their proper signals attached, the schematic and layout will now be synchronized. 

Suggestions: Fusion 360 should have the following implemented to avoid this trap. 

1) At the very minimum, the "SIGNAL" command needs to be able to manually assign a signal name to a pin that lacks one. 

2) Better, the "SYNCH" function should be able to manually name a pad signal from the corresponding schematic pin's net. I'm not actually sure what "SYNCH" does, since I could never get the "RUN" button to be active, it was always grayed out. 

[jorge_garcia]

Hi @pblase,

Congratulations on getting things sorted. Once you do the slice, if you want things to re-connect you can't start from the pin and try to meet the end of the existing net because it's off grid. You have to use the MOVE command grab the existing net and drag it onto the pin.

The synchronizer won't run on a design that has had a module in, but it will still try to show you what the inconsistencies are. That's why the dialog pops up.

The synchronizer is intended to help restore consistency, but since it can't handle modules it's not useful in that context. Hence why it gets grayed out.

Your method works obviously but it's more work than necessary as you have already discovered.

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

Best Regards,