topic Re: Important feature removed in the latest update in Fusion Electronics Forum

Important feature removed in the latest update

marcocipriani01 — Mon, 08 Jul 2024 20:25:35 GMT

Probably inadvertently, a feature which is very importat to me has been removed in the latest update: it is now impossible to change the signal that a net or a via is associated with.

Suppose, like in the following example, that a PCB contains two identical sections (two motor drivers here). Routing the same stuff twice is very tedious, so I've always followed this procedure:

Arrange the components of the fist "block" as necessary
Use the "Copy format" tool to copy the coordinates of each component in the first block and apply them to the components of the second block
- In the case of the two blocks aligned vertically, I start by copying only the X coordinate
- Then, I move the entire second block to the side of the first one, and transfer the Y coordinate of every component
- I finally move the second block back to its original position
Route the first section with wires, vias and polygons
Using the selection filter, copy only wires, vias and polygons from the first block and paste them on the second block
Change the signals associated to the newly copied wires, vias and polygons, either using the "Name" command or by changing the signal name from the object's properties

The last step has now become impossible because the latest update changes the behaviour of the "Name" command in the PCB environment. Previously, the "Name" command, when executed from the PCB, would only change the signal associated with an object (e.g. a wire associated with SIGNAL_1 becomes associated with GND, and not anymore with SIGNAL_1).

Since the latest update, the "Name" command renames the signal associated with an object, e.g. SIGNAL_1 is renamed to GND. This has following bad side effects:

The command fails every time SIGNAL_1 was also connected to something else, because Fusion tries to merge SIGNAL_1 and GND, returning an error (see picture below).
If, instead, I use the "Name" command to rename SIGNAL_1 to NEW_SIGNAL, and NEW_SIGNAL isn't already connected to something else, the schematic is modified from the PCB environment, i.e. back-annotated, which is very undesirable. No change on the PCB should ever modify the schematic!

The same is also true when changing an object's signal name from its properties.

Please, bring back the previous behaviour. I can't see a use case for the new behaviour (renaming signals from the PCB environment, why?), and back-annotating the schematic is a very bad thing.

I am available to send example projects and discuss the issue further via email.

Regards,

Marco Cipriani

Re: Important feature removed in the latest update

jorge_garcia — Mon, 08 Jul 2024 21:40:47 GMT

Hi @marcocipriani01,

Dang dude, that is definitely doing it the hard way. If you have circuitry that you intend to re-use it's easiest right now to save it as it's own electronic design. You can then insert it into your current electronic design as many times as you need. The net renaming in this feature is intelligent, power signals will not automatically rename but all other signals will. This workflow is simpler and more efficient than what you are currently doing.

With that said, your current workflow should work. Normally the copy command will renumber the nets when you make a copy to avoid collisions. However it also has the option retain the original signal names which is the default, you'll see it as a checkbox that says use source signal. Uncheck that box and you'll have the behavior you are used to.

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

Best Regards,

Re: Important feature removed in the latest update

marcocipriani01 — Tue, 09 Jul 2024 19:20:16 GMT

Thanks man, you're right. That's what happens when someone (me) started using EAGLE years before "Insert Electronic Design" was a thing. I had been using my workaround for ages.

I hadn't noticed the new "Use Source Signal" option, since I always use Ctrl-C Ctrl-V. That solves it.