How much oil / water / air in that system?

Those of you using the Inventor Tube and Pipe Environment to populate your designs with welded pipe, tube and fittings, flexible hose or a combination of all three will have asked or been asked this question; How much oil / water / air in that system? 

Tube and Pipe System

To answer this question, some additional work has to take place.
Firstly, open the pipe run you are querying and observe the components that make up the pipe run (sub-assembly)

Tube and Pipe Run - Windows Explorer Navigation

This pipe run is typically placed in a folder named TUBE AND PIPE, in a folder named AIP, in a folder named “Parent Assembly.IAM” name.

Tube and Pipe Run - Sub-Assembly Components

This assembly named “Edit Routes and Fittings.Tube and Pipe Runs.iam” will be the assembly I will query to find its volume.
The task in hand is to model the inside of the pipes and fittings that make up the pipe run assembly and query that solids iproperties, namely volume.
This can be achieved by using the derive command in Inventor.

Start a new standard part file and then 3D Model TAB > Create Group > Derive ICON

Derive the Pipe run assembly into the part file making sure the Derive Style is “Single Solid body merging out seams between planar faces”

Tube and Pipe Run - Derive the Assembly
Tube and Pipe Run - Derived Solid

Save the resulting part file.

Next Using the 3D Model TAB > Surface GROUP > Delete Face ICON tool, delete the surface perpendicular to the pipe orientation at the termination of the pipe run. Do this at all terminations of the pipe run.

Create a boundary patch, 3D MODEL TAB > Surface GROUP > Boundary Patch ICON, on the cylindrical end of the pipe run to create a closed envelope representing the inside of the pipe run system

Tube and Pipe Run - Edit the Derived Solid to create an envelope

Use the 3D MODEL TAB > Surface GROUP > Sculpt ICON to create a solid based upon the previously defined envelope.

Select All Boundary Patches plus the pipe run surfaces.

Tube and Pipe Run - Use the envelope to create a New Solid

The resulting solid can now be queried by calling the part iProperties.
In this example the volume is noted as being 10500431.970 mm^3 (Relative Error = 0.329858%)

Tube and Pipe Run - Query the New Solid iProperties

In the image below I have shown the derived solid placed into the pipe run assembly.
The pipe run assembly has an appearance = Clear and the derived solid = Light Red (for visual effect only)

Tube and Pipe Run - Desired Result

Thank You to JDMather, Expert Elite, for guidance and advice regarding this procedure.
http://forums.autodesk.com/t5/user/viewprofilepage/user-id/108623

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