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Extracting Internal Volume for Flow analysis (GTAC Article)

[ Edited ]

Following is another great article from the Siemens PLM GTAC team.

 

 

NX Flow solver in Advanced Simulation requires all elements used in modeling Flow to be 3D elements.  While the solid mesh for a design part occupies the part itself, the fluid mesh occupies the void between the bodies.  Because the void itself is not a body, one must create a solid body to occupy the void.  This solid body is generated in the idealized part I and then a mesh is applied on this body with 3D fluid elements using the NX meshing tools.  This internal fluid volume can be created by one of the following 3 methods:

 

  1. Define a sketch representing the 2D shape of a regular fluid volume and then Extrude and/or Revolve the sketch.  Use this technique if one knows the shape and dimensions of the fluid volume.
  2. Use Boolean operations to create the fluid volumes.  Users create a solid representing the enclosed space and select the Unite, Subtract, or Intersect to modify the shape of the volume based on the intersecting solid component geometry.  Use this technique if you want to create this fluid volume for single use in an analysis and if you are not interested in maintaining links for geometry updates.
  3. Create the enclosed fluid volume as a separate part file and component in the assembly file structure using the WAVE Geometry Linker command.  This command copies an instance of the geometry of the inner volume and the components from the assembly part file.  One then modifies the contour to represent the fluid volume by using the Delete Face command (on the Synchronous Modeling toolbar).  Use this technique if you want to maintain a link to the geometry of assembly components to allow for geometry updates.

 

In this article we will go over the 3rd method specified above to extract the flow volume.  Consider the task of extracting the internal flow volume in the following valve:

 

Here are the steps to extract the internal volume:

  1. Open this CAD model in NX. Select ‘Start -> Advanced Simulation’ to switch to Advanced Simulation application.
  2. In the Simulation Navigator, select ‘MB3 -> New FEM and Simulation’.  Set the solver to ‘NX Thermal / FLOW’, Analysis Type to ‘Flow’ and OK all the forms.
  3. Double-click on the idealized part to make it the ‘Displayed’ part.
  4. If you do not see ‘All but Selected’ icon in the ‘Selection’ toolbar, select ‘Tools -> Customize’ command.  Here, in the ‘Commands’ tab, select ‘All But Selected’ from the ‘Selection Bar’ category as shown below.  Then, drag and drop this command in the ‘Selection’ toolbar.
  5.  Now, select ‘Insert -> Associative Copy -> Wave Geometry Linker’ command. Set the ‘Type’ to Body and select the valve.  In the dialog, toggle ON ‘Associative’ and ‘Hide Original’. OK the dialog.  This creates an associative copy of this valve in the idealized part. Any changes made to this copy will not affect the original CAD valve geometry.
  6. Select ‘Insert -> Synchronous Modeling -> Delete Face’ command.  Set the ‘Face Rule’ to ‘Boss or Pocket Face’ and select any internal face of the valve as shown below:
  7. Now, select ‘All But Selected’ icon  from the ‘Selection’ toolbar as shown in the previous image.  This will select 66 Faces as shown below.                                                                     
  8. Choose OK from the ‘Delete Face’ dialog.  This will result in the internal volume being extracted as shown below.  This internal volume can then be meshed with 3D tetrahedral mesh in the fem file to represent the flow volume.  

 

Thanks to SR for the tip.

 

Jerry

 

- - - -
Jerry Sarfati
Siemens PLM Software
8 REPLIES

Re: Extracting Internal Volume for Flow analysis (GTAC Article)

Can you show how to extract flow volume from assembly 

Re: Extracting Internal Volume for Flow analysis (GTAC Article)

[ Edited ]

Flow volumes in the context of an assembly can be created using surface wrapping techniques in Advanced Simulation. NX 9 CFD Modeling is a new pre-processing add-on product for CFD analyses. The attached video demonstrates the surface wrapping capabilities in the context of an exhaust manifold assembly. The manifold, exhaust pipe, gasket, and cylinder head geometry is represented.

 

(view in My Videos)
 

 

Mark Lamping

Simulation Product Management

Product Engineering Software

 

Siemens Industry Sector

Siemens Product Lifecycle Management Software Inc.

2000 Eastman Drive

Milford, OH  45150

mark.lamping@siemens.com

www.siemens.com/plm

Re: Extracting Internal Volume for Flow analysis (GTAC Article)

Hi:

 

I am using NX 8.5. Is there any way in NX 8.5 to get the flow volumes in the context of an assembly?

 

I would appreciate your help.

 

Thanks,

Aydin

Re: Extracting Internal Volume for Flow analysis (GTAC Article)

You can try to unite all bodies in the assembly to form a single solid body. Then use synchronous modeling's Delete Face command as documented in the original topic of this thread.

 

Regards,

Mark

Re: Extracting Internal Volume for Flow analysis (GTAC Article)

Thank you for your answer. 

 

I tried your method. It went well, till at the end which gave me this error:

 

Delete failed because the remaining faces cannot close the area after deleting the slected face.

 

Any idea what is this error for?

 

Thanks

Re: Extracting Internal Volume for Flow analysis (GTAC Article)

Delete Face begins with a solid body and must finish with a solid body. It literally deletes the faces you select and tries to close the holes that remain. Typically when you get this message it is because NX was unable to close a hole. Take a block with a cylindrical hole passing through it as an example. If you choose to delete the hole, then the solid is left with free edges at each end of the cylinder. For each free edge loop, NX will create a face to "heal" the solid body. If every free edge loop produces a face, then you should end up with a solid body.

 

It sounds like one or more of the free edge loops on your solid body failed to produce a face. You can diagnose the error by choosing to not heal the solid body in the Delete Face dialog. In Delete Face, expand the Settings block of the dialog and turn OFF Heal. The output from Delete Face will be a sheet body with many free edges. Examine your free edge loops to see if any look like they would have a difficult time creating a face. You could even try creating faces from the loops with N Sided Surface, Bounded Plane, or Fill Surface commands. 

 

It could be that you selected too many faces for the delete face operation. That is, if you selected a face that should remain as part of the fluid volume, then I could see this error popping up. That's about all I can think of without having the part to test with.

 

Regards,

Mark

Re: Extracting Internal Volume for Flow analysis (GTAC Article)

turning off the Heal helped, thank you. However, I encountered another problem.

My geometry is a spool ( with complicated notches) that is assembled inside the valve body. The diameter of the spool is 0.05 mm less than the diameter of the hole inside the valve. After assembling the spool with the valve body, I tried to unite them, but it did not accept, giving the error that the tool is outside the target. So I created a cylinder with the same diameter as the hole diameter and unite that valve with this new cylinder. In this case, I am able to get the fluid volume. However, I need to use the real spool with the notches on it to capture the flow path through these notches as well. I think this gap makes the problem. Any idea how can I get the fluid volume using the notched spool with diameter of 0.05 mm less than the hole diameter? How should I unite them and use the delete face?

Thanks,

Re: Extracting Internal Volume for Flow analysis (GTAC Article)

The error during the unite that the tool is outside of the body means that NX thinks there is no intersection between the bodies to act as the "conduit" to unite the two into a single body. Without having your geometry, I can't really elaborate more on ways to achieve the fluid body that you desire. I have no idea what size your geometry is, but it seems like a 0.05mm gap can be idealized away to a 0.00mm gap. I imagine that a good mesh that represents that small of a gap is going to produce a ton of elements with little benefit with respect to the analysis results. Just for reference, default NX Modeling tolerance is 0.01mm. Typical minimum element sizes are a minimum of 10-100 times larger than the modeling tolerance.

 

Regards,

Mark