# Moving wall vs. SRF vs. Moving mesh

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

February 8, 2015, 11:44
Moving wall vs. SRF vs. Moving mesh
#1
Senior Member

Daniele
Join Date: Oct 2010
Location: Italy
Posts: 993
Rep Power: 17
Hi all,
I have some questions about a test case I'm running.
The case is very simple: a cylinder (radius=5 cm, height=1 cm, positive Z), filled with water, rotating at 105 rad/s around Z axis; cylinder is centered in 0,0,0.

I'm using fluent to evaluate results.
I thought that single reference frame, moving mesh and moving wall (set up in the wall boundary panel) simulations should give similar results.

Instead, I got similar results for SRF and moving wall, but not for the moving mesh..
Can anybody explain why?

I'm attaching velocity contours in xy plane, at mid-height of the cylinder, cell centered values, (variable velocity for fluent, velocity in stn frame for cfd-post) for the three cases.

Daniele
Attached Images
 Rotating_Cylinder.jpg (32.0 KB, 41 views)
__________________
Google is your friend and the same for the search button!

 February 8, 2015, 15:52 #2 Senior Member   Joern Beilke Join Date: Mar 2009 Location: Dresden Posts: 197 Rep Power: 10 This is a nice testcase for the moving mesh implementation :-) Unless you specify the motion of the wall to be rotation, the fluid should stay in rest. When dealing with moving meshes you also have to take into account the "space conservation law" (Raumerhaltungsgesetz). ghost82 likes this.

 February 8, 2015, 15:56 #3 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 993 Rep Power: 17 Strange thing to me is that in the moving mesh case I specify both the motion of the mesh and the absolute rotational velocity of the walls... (I did 2 tests, the first with relative motion, 0 rad/s relative to adjacent fluid zone and the second with absolute rotational velocity, 105 rad/s, but results are the same)..so I don't understand why the fluid seems stationary... __________________ Google is your friend and the same for the search button!

 February 8, 2015, 16:15 #4 Senior Member   Joern Beilke Join Date: Mar 2009 Location: Dresden Posts: 197 Rep Power: 10 For moving mesh cases you might get 2 different sets of velocities for postprocessing -- absolute and relative velocity. Did you check this? ghost82 likes this.

 February 8, 2015, 16:23 #5 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 993 Rep Power: 17 Yes, I checked in cfd post because fluent has only 'velocity magnitude' (and it should be absolute vel.). In cfd post velocity in stn frame should be the absolute velocity (equivalent to velocity magnitude). Moreover, all results were compared with ensight and I chosed the same velocity variable for all the cases. __________________ Google is your friend and the same for the search button!

 February 8, 2015, 16:36 #6 Senior Member   lore Join Date: Mar 2010 Location: Italy Posts: 464 Rep Power: 10 I don't have any experience with fluent so I may be completely wrong here. Usually, moving wall and SRF (I'm assuming it's the same thing as a MRF) can be used with both a steady state (a RANS for instance) and transient simulation (a DES for instance). On the other hand, a sliding mesh would make sense for a transient simulation only although in your case the geometry position would no change in time for a fixed observe, being your cylinder completely smooth. Did you run a transient simulation for the sliding mesh? If yes, did you run for long enough in terms of physical time (seconds)? ghost82 likes this.

 February 8, 2015, 16:40 #7 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 993 Rep Power: 17 Thanks for reply. Yes, moving mesh test case was run in transient, for 1 second, starting from the srf solution. __________________ Google is your friend and the same for the search button!

February 10, 2015, 09:03
#8
Senior Member

Daniele
Join Date: Oct 2010
Location: Italy
Posts: 993
Rep Power: 17
It seems the problem was the timestep: I didn't check the timestep independence and I set up a timestep so that 100 timesteps were needed to complete a revolution.
Even if the solution converged (continuity residual below 1e-4, below 1e-5 for others) and the area weight average velocity magnitude did not change vs physical time on the xy z-mid-range plane the result was not true.

Timestep of 1e-4 was needed to have a solution independent of the timestep (this means 600 timesteps per revolution!!!!).
Attached Images
 Rotating_Cylinder.jpg (32.6 KB, 30 views)
__________________
Google is your friend and the same for the search button!

 February 10, 2015, 09:44 #9 Senior Member   Joern Beilke Join Date: Mar 2009 Location: Dresden Posts: 197 Rep Power: 10 Thats why it is a common practice to do a steady mrf run for the initialisation :-)

 February 10, 2015, 09:46 #10 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 993 Rep Power: 17 Sure, however, even if the solution is initialized with the mrf solution, and you don't set a correct time step (and the only way is to perform a timestep independence study) results will be wrong as the solution tends to go always to 0 velocity. __________________ Google is your friend and the same for the search button!

 February 11, 2015, 14:22 #11 Senior Member   Cees Haringa Join Date: May 2013 Location: Delft Posts: 440 Rep Power: 9 600 timesteps, that's quite a steep requirement. Especially for a case that looks so simple. Nice test!

 February 11, 2015, 14:39 #12 Member   Join Date: Jul 2013 Posts: 49 Rep Power: 5 Hello, It is indeed a nice test that you are performing. I can't help but find that the plot that you posted seem quite different one from the other. You should consider plotting along the radial direction, and overlay the 3 result curves. I also suggest that you plot for velocity component instead of magnitude. Again, I would plot radial velocity and tangential velocity along a chosen direction.

 February 16, 2015, 15:21 #13 Senior Member   Joern Beilke Join Date: Mar 2009 Location: Dresden Posts: 197 Rep Power: 10 It sounds very strange that the velocity should go to zero when using a too large time step. So I tried it myself with CCM+ and was able to specify timesteps as large as 600 degree/step without problems. It requires some more inner iterations but there is no sign that the velocity goes to zero. ghost82 likes this.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post swahono OpenFOAM Running, Solving & CFD 8 February 26, 2015 05:30 ADGlassby OpenFOAM Native Meshers: snappyHexMesh and Others 18 June 18, 2013 06:07 aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 04:52 wayne FLUENT 3 June 11, 2008 23:23 Althea FLUENT 21 February 6, 2001 08:05

All times are GMT -4. The time now is 10:08.

 Contact Us - CFD Online - Top