Check Net Connectivity and Pads with Similar Numbers

[BuGG]

Is there a way for "Check Net Connectivity" to alert when a pattern has pads with similar numbers that aren't connected?

For example, I have a pattern designed to accommodate two different size trim potentiometers.

Pin 1 and Pin @1 should always be connected together by a trace in the PCB Editor. I'd prefer to not add the connection to the pattern because it might need to be on different layers depending on the project.

If I leave these pads disconnected there is a visible ratline showing that a connection should be made, but "Check Net Connectivity" does not alert that these pads are not connected.


Also, if I do make this connection with a trace when I run "Renew Layout from Schematic" the trace is removed and the ratline reappears.

Shouldn't these pads remain connected when renewing from schematic? And shouldn't "Check Net Connectivity" alert when they are NOT connected in the PCB Editor?

Trim.png (8.45 KiB) Viewed 44967 times

[Tomg]

...If I leave these pads disconnected there is a visible ratline showing that a connection should be made...

Those are not ratlines, they are lines that show the component's internal connections.

...if I do make this connection with a trace when I run "Renew Layout from Schematic" the trace is removed and the ratline reappears...

If the schematic shows a connection the trace should not disappear. Could be wrong, of course. Try connecting the pins in the schematic to see what happens to the traces when running the "Renew Layout from Schematic" tool.

[BuGG]

There are no additional pins to connect, the schematic component has pins 1, 2, and 3. There are no @1, @2, and @3 pins on the component, only the pattern.

What I don't understand is, if DipTrace isn't going to notify me that these internal connections haven't been made on the PCB what is the purpose of linking the pins in the component/pattern to begin with?

I could just create as many pins as I want in the pattern, ignore them completely in the component, and then connect them manually when laying out the PCB.

The dotted lines are helpful, but when working with fine pitch components they aren't always visible without zooming in closely to inspect. If I have to remind myself to check these connections I don't completely understand the reason for connecting them in the component. Shouldn't there be a way to alert the user that those internal connections have been left open, since DipTrace does acknowledge (by the dotted lines) that they should be connected?

If we're going to consider these internal connections a completely different entity from nets shouldn't there be a "Check Internal Connections Connectivity" verification? If these connections are left unconnected one can end up with an entire batch of fabricated PCBs that end up in the trash. (Ask me how I know this )

I could permanently connect them in the Pattern with the Signal layer, but depending on the particular project those small traces might need to be on different layers.

Since it seems there is no option for this, maybe it's fit for a "Feature request".

[Tomg]

I see what you mean. Perhaps the developers should consider changing the "Renew Layout from Schematic" tool to prevent it from deleting traces between internally-connected pins; or at least offer the option.

[Alex]

You can right click on either of internally connected pads and open "Component Internal Wire" from submenu. There are some options there. You can change "Connect Any Pad" to "Connect All Pads". If you run "Check Net Connectivity" the software will find you broken nets if any of internally connected pads has not routed.

[BuGG]

Perfect, exactly what I needed, thank you!

I think it's time I review the documentation again and familiarize myself with new features that have been added over the past few major versions.