Library: how to create components with multiple package variants

[anthonyEX9NB]

I'm trying to make some components in my library that have more than one package variant. I saw a post by tracy.wynn who seemed to be trying to do something similar. Jorge Garcia suggested she look at the RCL library as an example structure.

First, I cannot open the RCL library. And it looks like I can't open ANY library that isn't my own. The error I get is that the library I am trying to open is in Library.io and I get an authentication error.

So I tried to copied the structure from my old copy of Eagle in which you name the Device, for example, 74*00 (the * is a wildcard character). When you put this Device in the schematic, the * is replaced with the Package Variant name. If I us the * as a wildcard in Fusion 360, the Package Variant is APPENDED to the Component name. For example, if I name a Component ESD321*R and I have two package variants with Variant names DPY and DYA, in the schematic the Component Value is ESD321RDPY.

Note - I want Fusion 360  to generate the Component name based on the name that I assign the Component with the Package Variant inserted into the Component Name at the wildcard. The Component Name then gets inserted into the schematic as the Component Value which I use as the manufacture's part number.

What wildcard character do I use as a placeholder to put the Variant name anywhere I want in the Component name?

Lastly, I spent a good amount of time trying to find how to do this on the internet, on youtube, and in the autodesk website and could not find details on how to make Components with multiple Package Variants. Surely, I am not the only one that wants to do this. Okay, accept for that post by tracy.wynn that might have led me to an example library that I couldn't open.

Please help!

@jorge_garcia 

[jorge_garcia]

Hello @anthonyEX9NB,

I hope you're doing well. The * will allow you to place Technology names anywhere you want, not the package variants. For package variants you use the ? mark as the wildcard character.

Go into the library manager in Fusion and then search for the library rcl, then right click on the library and select edit to open it.

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

Best Regards,

[anthonyEX9NB]

Thanks for this information, Jorge. I never really understood how the Technologies and Package Variants in the library mapped into the schematic and hence, the BOM in Eagle. The English manual for Eagle was hard to read (it was a translation from German) so I just skipped it.

For Fusion 360 I had to spend considerable time experimenting to see how the library information mapped into the schematic. It would have been much easier if there was some documentation that explained how this works. It seems the Fusion 360 Electronics documention just copies the English manual for Eagle.

Regardless, it seems that Fusion 360 Electronics has renamed the Eagle concept of Technologies to Attribute Sets. Can you please confirm this? But I am assuming that Attribute Sets are supposed to serve the same purpose as Technologies? Please confirm.

I read a post by @jwilkin8475 who talked about the same issues with library work flow and trying to find explanations of things that I have. Is there enough user support to drive an unpdate to the documentation?

[anthonyEX9NB]

Oh man!! I should take better notes!

I tried using Techonologies (Attribute Sets) and Package Variants in Eagle and discarded the idea. I guess I went through the same process over the last couple of days with Fusion 360 and arrived at the same conclusion.

I have an internal company part number for all my parts. I can use the Attribute Sets nad Package Variants to build the mnaufacturer's part number, but there is no way to build my internal compnay part number using the same process.

For example, lets say there is a manufacturer's part number, say ABC-, that comes in 2 different packages, say Pack1 and Pack2. I can use the Package Variants to generate the manufacturer's numbers, ABC-Pack1 or ABC-Pack2, which would be the Name of the compnent when placed in the schematic. And I use an Attribute that holds my company part number and the Attributes are assigned at the Component level, not the Package level, so both ABC-Pack1 and ABC-Pack2 would get the same company part number.

Further, the IPC defines 3 defferent categories for PCB density, and this translates to 3 different possible pad sizes for the same Package. 

I could go on in great detail how the Fusion 360 library system can't be used to map all this stuff and generate correct part numbers, but suffice to say that the only way to accomplish capturing all this detail (or setting up a library to expand to capture all this detail) is to create a one library Component that maps to one Symbol which maps to one Footprint which could map to many Packages.

[jorge_garcia]

Hi @anthonyEX9NB,

You are correct, Technologies are now Attribute sets. Since you are diving deep this is how I would handle a component like the one you describe.

3 IPC densities, 2 footprint options. This could potentially be handled without going into attribute sets.

You will need a total of 6 2D footprints (3 IPC densities x 2 footprint options), these can actually be generated automatically using the package generator in most cases as long as the footprint is supported by the wizard. The Package generator supports the IPC density definitions so you can use it to generate the footprints in Most, Nominal, and Least densities.

In the component editor you would create a package variant for each of those footprints. Each of those variants can have it's own attributes in which you could add your own internal part number among other attributes like MPN, pricing info, availability and whatever other information you may want to include.

UPDATE: Agree that we need more documentation and easier to find documentation.

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

Best Regards,

[anthonyEX9NB]

Your solution, @jorge_garcia , defeats the purpose of using wildcards to generate the Component Name, doesn't it? I realize that your solution may be the only way to handle multiple IPC footprint categories and multiple footprint.

Unfortunately, I haven't used other schematic capture and layout tools so maybe there is no better way to manage this.

Also, as I mentioned, I am using the Component Name as the manufacturer's part number so If I implement your solution I would have to re-create all my libraries. Fusion 360 doesn't have a way to do bulk changes to a library so I would have to re-create each component. I have using Eagle since 2016 and imported my libraries into Fusion 360 in 2022 and have since added more parts to my libraries. Suffice to say that re-creating my libraries no would be a major overhaul.

[jorge_garcia]

Hello @anthonyEX9NB,

I hope you're doing well. So I don't see how my solution would invalidate the use of wildcards. So let's say the 6 package variants. Lets say footprint 1 is through-hole and the datasheet calls it N, the other footprint surface mount and abbreviated as SM. The six package variants would then be

NL, NN, NM

SML, SMN, SMM

Then use ? to indicate where that needs to be in the component name.

I understand your concern with re-creating libs. There are a few ways to deal with this. One option is to adopt this moving forward. You make a copy of your existing library and use that as a trampoline point for future work. The original lib would be left alone to support existing designs while the new one would implement a paradigm like this one.

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

Best Regards,

[anthonyEX9NB]

My apologies, @jorge_garcia . I didn't fully explain myself.

Let's reduce the proble to 3 IPC densities and 1 package style. By your method that would mean three 2D footprints If those three footprints are linked to the same Component they each have to have a unique Name, and this unique Name is what gets inserted into the Component Name whereever the wildcard is inserted. The result would be a different Component Name when one places the Component into the schematic. In this case, the Component Name cannot be used to generate the manufacturer's part number (MFG-PN) because the MFG-PN doesn't include any characters for what the actual footprint looks like. The MFG-PN has to be an attribute of the Component, which would be the same for all three IPC densities. Further, the Component Name would only be used in the schematic as an indicator to the reader what density is used in the design.

My assumption was that the original design intent of the Eagle software was to use the Component Name to generate the MFG-PN. My assumption may have been true, but perhaps the original designers of the software were not aware of IPC densities.

And this is where I would need to re-create my entire library system.

[jorge_garcia]

Hello @anthonyEX9NB,

See this picture of a 555 timer datasheet 

Notice that each footprint type corresponds to a different suffix CM, CMM, CMX these would be the name of the package variants. Additionally every package variant in the Component editor get's it's own set of attributes. So each of those package variants would have individualized attributes for ordering info. 

Now lets say you create additional package variants for the CM footprint to cover the IPC densities. In that case each of the 3 variants could have the same attributes so that the same part is ordered for all of the densities. Ordering and BOM information isn't strictly dependent on the Component name, the attributes offer a flexible way to make sure that regardless of IPC density the same part is ordered.

Let me know if you continue to run into difficulties.

Best Regards,

[squigleyZWHQC]

or the MOUNT-HOLE Library there are several hole sizes(effectively DRILLS). How can I get the different VARIANTS to show on the schematic when I place them?

[jorge_garcia]

Hello @squigleyZWHQC ,

I hope you're doing well. The component name is what shows the size. In the case of the MOUNT-HOLE components form the HOLES library, it's default value is set to the be the COMPONENT NAME so when you place them you should see the diameter written as MOUNT-HOLE3.2 for a 3.2mm hole. 

Are you not seeing this? If not, what are you seeing?

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

Best Regards,

[squigleyZWHQC]

I figured it out. I use Attribute Fields for all of my components and
display the specific fields I want to see in the schematic.

For MOUNT-HOLES there are several variants(2.8mm, 3.0mm etc). I want that
info.to be displayed in the schematic when I bring in each variant.

What I didn't understand was how to access the fields for each variant to
enter the data into the fields.

But I understand now.