Fusion Electronics Assembly Variants

The concept of assembly variants is pretty cool. There is an assembly variant table which you can add additional variations of your schematic assembly. You can add assembly variants which copies every component and allows you to:

• remove the component (uncheck it)

• replace the component with a variant (like a red LED with a green LED, or to unpopulate the component)

• change the value of the component (change resistor and capacitor values).

This requires alot of back ground knowledge:

• Library Editor

• Device/Component attributes

• Footprint variants

• Footprint attribute sets

Library Editor

If you want to work in Fusion Electronics you need to use the library editor. It is a confusing tool, but it is essential. If you have a project open, you can get to it easily.

• #1 click the "LIBRARY" tab at the top of the page (in Schematic or PCB screens)

Then look for the "Open Library Manager" (see #2) and click it.

This should list all of the libraries you have. Note that there are three types of libraries. 

1. Managed Libraries reside on the cloud Library.io. While they are stored on the cloud, the libraries are managed, meaning you need permissions to be able to modify the libraries.

2. Fusion Hub (or Fusion Team) are libraries that are kept on-line as part of the subscription service and provides Cloud Storage and collaboration tools for data. Fusion Team libraries are electronic libraries created or uploaded to Fusion Cloud.

3. Local disk. The libraries are stored on the local disk, but are not available via the cloud. 

In general you want to use Fusion Hub or Managed Libraries as they are available on the cloud so your Fusion Electronics will work anywhere or on any machine (as long as you log into the cloud).

So there are different icons and filters for looking at the libraries. Pick a library you wish to use, and edit it by right clicking on the library and clicking the edit.

Example to create, Generic Resistor

In this example, we'll create a reverse 1206 LED in five colors. The basic function is to have an LED component called "LED_1206_REVERSE" and then be able to pick a "variant" (RED, GRN, BLU, YEL, ORG, ...) and then place the LED in the schematic, along with a footprint for the PCB, and a 3D model for the 3D PCB. Additionally we'll have the 3D model with different colors.

First we want to define some attributes that each LED will have.

Box - where the parts are stored

DIGIKEY# - the digikey part number so that we can purchase this led (appear in BOM)

LABEL = A label to identify the LEDs in the box

MANF - who makes the LED (in our case WURTH)

MANF# - the manufactures part number for the part

VALUE - the color of the LED

Here is a table of the data we will need:

Creating the Component

It makes is much easier to download the CAD for the component. Most sellers (Mouser, DigiKey) have the symbol, footprints and 3D models available. I'll assume you have downloaded a symbol, footprint and 3d model (step file) from the web.

First we create the component and give it a name "LED_1206_REVERSE" and click "OK".

Next in the "Device" Icon group click the Add Symbol:

Pick an existing symbol (or the symbol you downloaded for an LED) and then it iwll appear in the symbol area. Center the LED on the cross hairs and release, the LED symbol is now part of your new component.

Next import your footprint  (Digikey allows you to down load the footprint, symbol and 3d model)

Next take the footprint and duplicate it so there are five copies appending the color of the LED.

Now edit the component again, and in the footprint area click the "New" button and then the "Add Local Package" and pick the footprint you just created and name the variant the name of the color (BLU, GRN, ORG, RED or YEL).

Next go back to the Component menu and open up the tree of the LED_1206_REVERSE. You should see a hierarchy of the Component on top, followed by the symbol, then followed by the five foot prints (each with a different color).

Next for each footprint click on the three dots and choose "Create New 3D Model". This will bring you into the 3D model editor and will ask you to save the foot print. Select and click "Save".

Next in the data panel, open it to the folder which has the 3D models of the LEDs. Right click once on the preview and then click the "insert into current design". The step file is inserted into the footprint and you need to adjust the 3d model such that it is sitting correctly on the footprint. Once done save. and repeat for all different colors.

Creating the Attribute Sets

Previously this was called "Technologies" but is now called "Attribute Sets". In the footprint editing area are the five different variants you have created. You need to right click on each variant and choose "Attribute Sets". A menu of all of the different variants are shown, unclick "Default" and choose (add if needed) the color of your variant (give it the same name, "RED", "GRN", "BLU", ...).

Next click and highlight the package variant in the footprint editor, and then select the LED_1206_REVERSE component, and then click on the "View Attributes". You should See BLU, then add the attributes for BOX, DIGIKEY#, LABEL, MANF, and MANF# for that color LED as shown in the table above. Click OK, then select the next color LED from the footprint editor and repeat the process (click the show attributes).