Using NX to find the interior volume of a pipe (for Fluid volume)

[junfanbl]

This isn't so much a technical question, as it is a mathematical and functionality one. I am looking for a way to find the interior volume of pipes. Typically finding the volume for a straight cylinder is easy, but when it comes to reducing cylinders, I am not sure of the best way to find the interior volume. Usually I would use calculator to find volumes, but sometimes it isn't so easy when you are working with unique pieces. I guess I need to brush up on my geometry. Is there a way NX can find it for me, or how can it be done mathematically?

Thanks for the help.

 

[cowski]

Extract the interior face(s) of your pipe, cap the ends, sew the sheet bodies to form a solid, and use the "measure body" function to find the volume.

www.nxjournaling.com

 

[junfanbl]

Okay, so basically you are reversing the model? How do you extract the interior faces and sew the sheet bodies together?

 

[cowski]

Extract interior faces: use the "extract geometry" command; for the "type", use "face" or "region of faces".

Cap the ends: the "bounded plane" command works well for this (assuming the ends of the pipe are planar).

Sew the sheet bodies together: use the "sew" command. As long as the edges of the sheet bodies match up within tolerance (which they should if you have a decent pipe model), the sew command will create a solid body. You can then use this "interior volume" solid body in the "measure body" command.

www.nxjournaling.com

 

[junfanbl]

Okay, there is just one more thing I need to do. Because of the way I modeled it I need to merge two faces together. How can I do that?

 

[Toost]

Somewhere there is a video created by John Baker which shows how one "reverses" a solid body by the delete face feature. This can be used in conjunction with the Extract Body. ( such that you have a extracted body ( = a copy) which is the reversed volume.)

I found this which i think shows the delete face trick.

https://www.youtube.com/watch?v=97XGafpranM

Regards,
Tomas

 

[JohnRBaker]

What version of NX are you using? And if possible, can you provide us with the model, or at least an image of what it looks like?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[junfanbl]

Sure, I can provide an image. I do not think I can properly extract bodies with two faces on the inside of the cylinder. At least I think so. So I am trying to merge the two so I can select the entire interior as one face before extracting bodies.

I am using NX 10.

 

[JohnRBaker]

How is it that there are two faces on the inside of the pipe? Is it a constant diameter or is there a taper at one end (can't tell from the picture)?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[cowski]

You can extract them separately or use "region faces" to get them both in one extract feature. It won't matter if it is one or many faces when you sew them together later.

www.nxjournaling.com

 

[thomaskoer]

If it's getting more complex or if you don't want to think too much about it, you can use "Space Finder" (if you have a license).

 

[junfanbl]

Well it was a cone to start with. I extruded one end of the pipe with a 4.5 diameter with a wall thickness of .5. However I couldn't figure out how to reduce the extrude so it would match the diameter of the other side. Which is supposed to be 2.5 with a wall thickness of .4. So I added a circle and subtracted the geometry on the other end of the model and gave it a diameter of 2.5. I then extruded the larger hole only as far as the first face shows. From there, I used edge blend to hollow out the rest of the pipe until it practically lined up with the edge of the smaller hole. Hope that explains it!

 

[JohnRBaker]

This appears to be a very simple part. Could you simply upload IT? Or at least show a section cut through the axis of the pipe so that it's clear as what the relationship is between those TWO internal faces.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[JohnRBaker]

Attached is an example similar to what I think you're modeling. If you un-suppress the last feature of the model tree, you'll have a solid body of the interior volume of the pipe.

The way I created this was by using the 'Delete Face' function (make sure that the 'Heal' option is toggled ON), selecting ONLY the internal faces and then pressing the 'All But Selected' icon on the Selection Bar (you may have to turn this icon ON), which will reverse the selection of the faces so that when you hit the OK button, the result will be a solid body representing the internal volume of the original model.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[junfanbl]

Oh okay, thanks a lot. That was a very simple approach. I wish I had thought of that to begin with. Well I did learn quite a bit in this post about the different features in NX. Thanks again!