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Autodesk Inventor - Tube and Pipe Environment - Inspect 'Fluid' volume

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Message 1 of 10
Neil_Markham
1730 Views, 9 Replies

Autodesk Inventor - Tube and Pipe Environment - Inspect 'Fluid' volume

Hello,

 

After creating the Runs required in the Tube and Pipe environment, is there a method to find the volume of media (Fluid, Air, etc) within those runs?

 

Thank You in advance.

 

Neil Smiley Happy

9 REPLIES 9
Message 2 of 10
JDMather
in reply to: Neil_Markham

You could Derive Component as Surface Body, Patch the ends and Sculpt (might have to Delete Face at least one face).

Post a real simple dataset here if you have trouble figuring it out.


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Message 3 of 10
Neil_Markham
in reply to: JDMather

Hi JD,

 

Thanks for your response but I don't quite follow what you mean.

 

I have zipped the data for the following assembly and attached it to this post. 

 

How would I find the volume of media (Fluid, Air, etc) carried by the flexible black hose pipe?

01.jpg

 

Your time and consideration are much appreciated.

 

Neil

Message 4 of 10
JDMather
in reply to: Neil_Markham

Start new part file.

Manage>Derive Components and select pipe.

Set to derive as composite surface body.

Delete Face one of the ends.

Patch the holes.

Sculpt the new enclosed envelope.

Check iProperties.

 

Pipe Volume.png


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Message 5 of 10
Neil_Markham
in reply to: JDMather

Thank You JD, your solution is perfect for this single pipe example.

 

To expand on my question. How would one find the volume through an assembly of pipe & fittings?

 

01.jpg

 

Neil

 

Message 6 of 10
JDMather
in reply to: Neil_Markham

You can derive the entire iam in the same way.


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Message 7 of 10
Neil_Markham
in reply to: JDMather

Hi JD, 

 

Granted, the SCULPT tool works well for single components but I am finding the tool cannot build a meaningful solid due to the complex surfaces that exist around the engagements between pipe and fitting components.

It would take lots of rework, deleting faces and boundary patching surfaces that do not mate nicely to achive a good result.

 

Its a shame there's no easy way in the Tube and Pipe environment to query the pipe runs volume.

 

Note: Using the derived assembly tool allowed me to create a sinlge solid body of the pipe run, which I then derived as a part (Bodies as Work Surfaces)

 

02.jpg

 

Neil

Message 8 of 10
Neil_Markham
in reply to: Neil_Markham

Hi,

 

Can anyone expand on this question where the pipe run is an assembly of components, not just one part?

 

Neil

Message 9 of 10
JDMather
in reply to: Neil_Markham

Derive your assembly like this

(and then attach the *.ipt file here if you can't figure out the solution)

 

New Derived.PNG

 

Your last assmbly did not include the fittings.

 

Here is an example - Extrusion1 & 2 should not have been necessary - but it was not modeled correctly, so I had to fix it up a bit.


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Message 10 of 10
Neil_Markham
in reply to: JDMather

Thank you JD your explanation enabled me to solve the query. I have written a blog post detailing my steps here ->

 

http://cadprosystems.blogspot.co.nz/2014/05/how-much-oil-water-air-in-that-system.html#more

 

Neil

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