CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Exhaust valve simulation

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   February 27, 2007, 05:15
Default Exhaust valve simulation
  #1
G
Guest
 
Posts: n/a
Hi,

I am trying to simulate transient flow around an exhaust valve and I am studying the tutorial Fluid Structure Interaction and Mesh Deformation. I am thinking to use Junction Box Routine in my case. Analogous with the description in the tutorial, I tried to create several meshes in ICEM-CFD, but I can't grasp which file types are in the meshes directory (CheckValve.0 - 19).

I am not sure, if the mesh files must be of the same type as in the tutorial, but I am not that good in FORTRAN, so I am thinking, that way I won't have to modify the FORTRAN subroutines too much.

I am thanking you in advance for any suggestion or explanation.

  Reply With Quote

Old   February 27, 2007, 22:05
Default Re: Exhaust valve simulation
  #2
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

Why are you trying to do FSI on an exhaust valve? If you are trying to model the valve motion to open and shut the valve you explicitly define the valve position using mesh motion. There is no need for FSI.

Glenn Horrocks
  Reply With Quote

Old   February 28, 2007, 02:40
Default Re: Exhaust valve simulation
  #3
G
Guest
 
Posts: n/a
Thanks for your response. I am not trying to do FSI, I just thought to automize the mesh replacing during the calculation. With mesh deformation, I have to stop the calculation before the mesh colapses(or it gets too bad), load another mesh manually and use results from previous step as initial conditions for the next one. So I thought it would be easier to prepare a set of meshes beforehand and and reload them for each time step using a Junction Box Routine (JBR)as described in the tutorial. If I misunderstood the procedure, please correct me. Is it possible to combine a mesh deformation and JBR?

  Reply With Quote

Old   February 28, 2007, 17:27
Default Re: Exhaust valve simulation
  #4
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

What you describe can be done with pure mesh motion as long as the mesh topology does not change. Have a look at the moving mesh tutorial problem as it shows doing this sort of stuff either by CEL expressions and user fortran. If you can do it purely by CEL expression it is much easier.

A hint on the moving mesh: Generate your meshes at the squished up condition and stretch them out rather than generating the meshes stretched out and you squish them up. The moving mesh algorithm by default stretches meshes more reliably than it squishes it up.

Glenn Horrocks
  Reply With Quote

Old   March 1, 2007, 03:31
Default Re: Exhaust valve simulation
  #5
G
Guest
 
Posts: n/a
Hi,

I tried just what you suggested, I stretched the mesh from the "closed" valve position, but at some point quality of the mesh gets too poor to describe physical phenomena correctly, so the mesh should be reloaded with new quality mesh at some point (new position of the valve).

And that's the thing, I don't know how to automize this. It would be great, if I could combine mesh deformation and JBR, but I think it can't be done. And now I can't even use the JBR, because I can't grasp what is the type of the mesh files (CheckValve.0 -.19) in the sub-directory meshes of the tutorial 20.
  Reply With Quote

Old   March 1, 2007, 17:18
Default Re: Exhaust valve simulation
  #6
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

You cannot do remeshing with a new mesh topology with a JBR. You need to stop the simulation, remesh and restart the simulation interpolating the results onto the new mesh.

This can be automated in a batch file.

Glenn Horrocks
  Reply With Quote

Old   March 2, 2007, 02:34
Default Re: Exhaust valve simulation
  #7
G
Guest
 
Posts: n/a
I thought so.

Thank you for you time, Glenn.

  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Resume Transient simulation HMR CFX 1 June 28, 2011 21:13
PCV valve simulation - FSI? farianka CFX 3 April 19, 2011 10:33
a problem of valve simulation in openfoam xck1986 OpenFOAM 2 January 21, 2011 21:08
exhaust manifold -steady state simulation turbotel CFX 0 November 30, 2010 07:09
micro valve simulation luitze OpenFOAM Running, Solving & CFD 2 May 15, 2009 12:57


All times are GMT -4. The time now is 01:10.