Let’s start by talking about Virtual components. Virtual Components are a method Inventor uses to represent non-CAD parts in a design. Non-CAD parts could be purchased items such as, Glues, Paints, Grease, Loctite, and many more items needed to make a products Bill of Materials complete. They are not defined by any geometry. Virtual components are “Geometry-less” and “File-less” components.
The benefits from using Virtual Components are as follows:
- They act as a place holder for iProperties.
- They become part of your assembly appearing in the assembly browser.
- They can be populated with iProperties which appear in Bill of Materials.
- They can be stored in Assembly Folders for easy management.
See the two images below for examples:
Virtual Components are created using the Create Component command from within an assembly file. They appear as a transparent and purplish colored component in the browser as shown below.
There is no Part (ipt) or Drawing (idw, dwg) files associated with virtual components. As mentioned, they are “Geometry-less” and “File-less” components. They exist only within the assembly (iam) file where they are created. Virtual components can be shared from assembly to assembly using the Windows Copy & Paste. This way as a “File-less” component, we can share iProperties that have already been added and used in previous designs.
Another way to share Virtual components with iProperties already populated is to add them to your Assembly (iam) template used when starting a new assembly file. Just delete the Virtual components you will not need when using that template. Much easier than re-creating them or finding an assembly to Copy & Paste from. See the image below.
Three disadvantages to Virtual Components are:
- They cannot exist in Vault, since they are “File-less”.
- We cannot create a drawing that purchasing may request, since they are “File-less”.
- We cannot use Vault to get “Where-Used” or “Used” information, since they are “File-less”.
This is where “Blank Parts” comes in. To start, Blank Parts provide all the benefits of a Virtual Component, PLUS MORE, since they ARE NOT “File-less”. A blank part is just like any other Inventor Part that you have created except it contains no model features, so they are for all intensive purposes, “Blank”. Well almost blank.
- We add iProperties to them.
- We add a point to the single Sketch in the Part.
The point is generated using the “Project Geometry” command and picking the Common Origin in your blank part file. Beyond that, they are Blank. Blank parts solve all 3 problems left vacant by Virtual Components. Because they ARE NOT “File-less”, they (1) can be stored as library parts inside of Vault, (2) can have drawings created from them for purchasing or other purposes and (3) Vault can provide “Where Used” and “Used” information. See the image below which shows “Sketch1” as the only geometry used to define a Blank part for “Loctite 603.ipt”.
So why the point you may be wondering. It’s simple. If there is no geometry in the part, Inventor cannot create an empty drawing view which links the IPT and IDW together. If a drawing is not needed, then NO sketch with a point is required in the Part, it can be 100% blank, except for iProperties that we populate for Bills of Material purposes.
Because we have a linked drawing due to the empty drawing view we create, we can <Right-Click> over that view name in the browser and Open the Blank Part file, just like any other Part and Drawing you have created. Without the point existing in the Blank part, this would not be possible.
Let’s talk a bit more about Blank Parts and how they work with Vault. Because we create an empty drawing view from the Blank Part, Vault is now able to show us Parent / Child relationships between both files as shown in the image at the right. We see the “Where Used” relationship highlighted in this example:
Now we have our design, including non-CAD files, fully managed by Vault.
Suggestion: As you are Placing a Blank Part into your Assembly, be sure to <Right-Click> and pick “Place Grounded at Origin”. If you randomly pick a point in space to place the Blank Part, you will have random points appearing in your assembly as shown in the second image below.
Should you discover that you have random points in your assembly because of randomly placing Blank Parts into your assembly, this is easily remedied.
- From that assembly, make sure all Blank Parts are not grounded.
- Select all your Blank Parts.
- Pick the “Ground and Root” command located in the Assembly tab > Productivity Tools panel. This command will constrain all selected components to the common origin of your assembly.
Another suggestion would be to store all your Blank Parts in an Assembly Folder. Maybe name it “Blank Parts”, or something that you prefer. See the image below showing a folder containing 4 Blank Parts in the Assembly Browser.
I hope this helps you with integrating non-CAD parts into your everyday design workflow.
About the AuthorMore Content by Randy Andracki