Bug in Schematics - Display of >NAME and >VALUE

[tracy.wynn]

I believe I have discovered a bug in how Fusion carries over Library data to schematics.

I have created a library for 0505 ceramic capacitors. There are multiple component entries, each for a different capacitance value. All components share a schematic symbol. The schematic symbol includes the tags ">NAME" and ">VALUE", on separate layers. Each component has an attribute called "VALUE" defined in its attribute list (along with entries for local p/n and manufacturer's p/n), and the data contained therein is the capacitance of that component. Each component also has two variants, one using a footprint with Component Exclude (Courtyard) graphics, and one without. Both footprints also include tags for >NAME and >VALUE, also on separate layers.

When I use a component from this library in a schematic, the "NAME" is populated with the proper reference designator, as expected, but the "VALUE" data, which should be the capacitance value, is ignored, and replaced with the "Variant" string. EXCEPT . . . every now and then, when I drop a new capacitor onto the schematic, >VALUE is populated with the expected capacitance value string from the attributes.

If I right-click one of the correctly-populated components in the schematic and look at Attributes, the correct information for local p/n and manufacturer's p/n is there (though, for some reason the "Value" attribute does not show up in the list). Also, when I right-click and look at Properties, the "Value" field is populated with the capacitance value, as expected. For a component with DOES NOT display correctly, the attribute list comes up empty and the Property dialogue doesn't even contain a field for "Value" (and the Attributes list is empty). I cannot predict when a component will populate correctly and when it will not, though correct population does not always choose the same component in the list, and the ratio of incorrect to correct is something like 30:1 or worse.

I made some very similar libraries around the same time (for inductors) and these appear to behave correctly. I am not sure how to proceed, but I am at my wits' end and frustrated.

Here's an illustration in a sample schematic. C1 and C2 are correct. C3-C6 are incorrect.

Here's what the schematic symbol definition looks like in the library.

[jorge_garcia]

Hi @tracy.wynn,

I hope this message finds you well. Go into your library, and check the components that are failing. In their component definition there is a radio button that says Value and it can be set to Off or On.

I would hazard a guess that the ones what the are not working have Value set to Off. By definition if Value is set to off then the value will be the component name in the library. For the way you have designed your library they should all be set to On. 

With that said to see if this works, remove the caps from the design and then re-insert them. Values are not touched when you do a library update. So the sure-fire way to see if it's fixed is by doing the above.

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

Best Regards,

[tracy.wynn]

Jorge,

That does appear to have fixed the >NAME string, but I have one follow-up
problem and one additional question.
First, while the >NAME string now populates as the reference designator,
now the >VALUE string does not show up. I do have the Value layer turned on
in the schematic editor, and the library symbol does include both >NAME and
>VALUE. The attribute set does also include an entry for VALUE.

Second: what does the described radio button actually *do*? I have gone
through quite a number of tutorials and I don't recall hearing it
mentioned. Further, the other libraries I created appear to be behaving as
intended, but the Value radio button is set to "off."

Regards,
Tracy

[jorge_garcia]

Hi @tracy.wynn,

I hope you're doing well.  So first let's answer what the Value radio button does, from the documentation

In Device Mode

If the VALUE command is used in the device edit mode, the parameters ON and OFF may be used:On: Permits the actual value to be changed in the schematic.

Off: Automatically enters the actual device name into the schematic (for example 74LS00N). The user can only modify this value after a confirmation.

Now the part that concerns is that there may be a bug here. If you have defined a custom VALUE attribute in the component editor then that should work regardless of the radio button setting. See this documentation from the ATTRIBUTE command.

The attribute VALUE and other special attributes

Names of text variables like NAME or GATE can't be used as attribute names. The only exception is the attribute VALUE, which can be used for assigning a value to each device in a library. If such a device is added to schematic, this value is used as part value regardless if the device set has 'Value On' or 'Value Off'. The attribute VALUE is then no longer available in schematic or board to avoid confusion. Changing the part value can be done in the usual way with the VALUE command. The attribute VALUE is also processed in library update, CHANGE PACKAGE/ATTRIBUTE SET and REPLACE. The part value is replaced by the newer or different value of this attribute if necessary. The attribute name EXTERNAL is reserved for marking of external devices (see PACKAGE).

Could you confirm how your setting up the VALUE attribute? A screenshot would suffice. IF you are doing it like I think you are doing it then I think we have a bug.

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

Best Regards,

[tracy.wynn]

Jorge,

Here is a screenshot of how I have set up the VALUE attribute in this
library. The confounding thing is that this is how I have set it up in ALL
of my libraries, and this is the only one with a problem. I agree that it
looks like a bug.

[image: image.png]

I am happy to provide any additional information that might help.

Regards,
Tracy

[jorge_garcia]

Hi @tracy.wynn,

The image did not make it try posting again

Best Regards,

[tracy.wynn]

Sorry - let me try again. Here's how I have my Attributes set up (see below).

I also have some new information to share:

I realized that my capacitor library (the one that's not behaving) does have a difference from my other libraries, which is that I added a second variant to each one of these parts. I created it as a footprint variant, since I can't seem to easily modify footprint characteristics (like courtyard graphics) after a part is placed. My other libraries only have a single variant per part (for now). I discovered that if I delete the second variant, everything is fine, and the library behaves as expected. Investigating further I discovered that, even if the second variant is present, if I choose the original variant, it also behaves correctly.

From there I right-clicked each variant and looked at "Attribute Sets". Both had "Default" checked, so I assumed they were equivalent. However, when I highlighted the original variant in the variant table, right-clicked the component in the component list, and looked at attributes, I found that the expected attributes were populated, but when I highlighted the second variant and then looked at the component's attributes, the attribute set was empty.

So, I think I've discovered how to make this work properly. And, now that I understand that, I don't think I'd call this a bug, per se, but I would call it a UI/UX issue. When a variant is created, it appears to inherit some of the characteristics of the parent (the schematic symbol, for instance), but not all the characteristics (e.g., the attribute set), but it gives each one's attribute set the same default name ("Default"). So, it works, but it's far from intuitive, and I haven't seen any treatment of this level of detail in any tutorial. Attributes and variants, as Autodesk implements them, could be a very powerful tool for creating and maintaining libraries, which are an essential tool in industry use. I think that an attribute manager, in which all attribute sets over all variants of a part could be viewed and edited, would be a very, very helpful feature.

Regards,

Tracy

[jorge_garcia]

Hello @tracy.wynn,

I hope you're doing well. I'm glad you figured it out, you had me worried.

I have created a feature request for an organized table editor.

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

Best Regards,

[tracy.wynn]

Thank you, Jorge. Let me know if there's anything I can contribute to the
effort.

That said, does Autodesk have a beta-testing program for Fusion
Electronics? If so, I'd love to contribute.

Regards,
Tracy