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

Problem with mesh movement in small gap

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 27, 2018, 09:42
Unhappy Problem with mesh movement in small gap
  #1
New Member
 
Join Date: Mar 2014
Posts: 8
Rep Power: 9
Fred_Erik is on a distinguished road
Hello!

I'm doing a transient rigid body simulation of a rotating cylinder in a bearing sleeve with CFX. Fluid is air as ideal gas, energy equation is isothermal. I simulate only half of the bearing in axial direction with a symmetry plane. For the fluid entry I use an opening with constant static pressure. To realize damping effects I placed the opening some axial distance away from the edge of the bearing. I take a hexaeder mesh designed in ICEM. At the beginning of the simulation the position of the cylinder is concentric to the bearing sleeve. The gap between the cylinder and the bearing sleeve is small (< 0,06 mm). As the cylinder moves due to an acting force the gap is getting smaller and smaller. The overall mesh movement works fine. But when the gap size reaches round about 0,005 mm the first nodes on site of the bearing sleeve move radial over the boundary and I get negative cells. As I use constant mesh stiffness I expected that the radial distance between the nodes would further decrease, but there seems to be a limit. I tried to fix it with different mesh stiffness, but it was not successfull. Maybe a decrease in number of nodes in radial direction in the gap may help, but then I also decrease the space discretization.

I looked for similar threads in this forum, but I found no adequate solution. Does anybody know to handle this problem?

Thanks,

Fred_Erik
Fred_Erik is offline   Reply With Quote

Old   February 27, 2018, 15:03
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,645
Rep Power: 130
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
This is a common problem in moving mesh simulations, especially when you are compressing the mesh (as you appear to be doing). You can often improve the situation by adjusting the mesh smoothing parameters - not just the mesh stiffness but the other options as well. But be aware this can be tricky and frustrating to fix.

If your geometry and motion is simple you may be able to directly specify your mesh as a CEL expression and not use mesh smoothing at all. This completely avoids the mesh folding problem, but it does mean you need to write a function which completely defines your entire mesh which can be challenging.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 27, 2018, 18:13
Default use immersed solid as sink for pinch region
  #3
Member
 
Join Date: Jan 2015
Posts: 62
Rep Power: 8
Christophe is on a distinguished road
image1.jpg you can make an artificial wall where the fluid mesh will pass through and not pinch by putting in a immersed solid.
Christophe is offline   Reply With Quote

Old   February 28, 2018, 10:51
Default
  #4
New Member
 
Join Date: Mar 2014
Posts: 8
Rep Power: 9
Fred_Erik is on a distinguished road
First of all thank you for your quick replies!

I have some questions to your advices:

To ghorrocks:

Quote:
You can often improve the situation by adjusting the mesh smoothing parameters - not just the mesh stiffness but the other options as well.
Do you mean to adjust the mesh smoothing parameters by the expert parameter "meshdisp diffusion scheme"? The documentation recommends to use scheme number 3 (Positive definite values (interior), positive definite values (boundary)) for uniform mesh deformation? I tried it, but there was no success.

Quote:
If your geometry and motion is simple you may be able to directly specify your mesh as a CEL expression and not use mesh smoothing at all. This completely avoids the mesh folding problem, but it does mean you need to write a function which completely defines your entire mesh which can be challenging.
I think, the movement and the geometry are simple. If you consider cylindrical coordinates, then the nodes only move in radial direction dependend of their circumferential position and the excentric position of the cylinder. Is it right that I change the mesh motion option to "Specified Displacement" with cylindrical components and define the radial component with an CEL expression? In this way is it possible that nodes on boundary can't move? Maybe I define the movement for nodes in a subdomain?

To Christophe:

The main disadvantage of the method with immersed solid is that I don't resolve the gap with enough nodes for a good space discretization, because the nodes move outside of my fluid domain, right? So I have to discretize the gap very fine to ensure enough nodes in the gap and this is more numerical effort for solving.

Thanks,

Fred_Erik
Fred_Erik is offline   Reply With Quote

Old   February 28, 2018, 15:48
Default
  #5
Member
 
Join Date: Jan 2015
Posts: 62
Rep Power: 8
Christophe is on a distinguished road
Can you set up the geometry to be able to offset the centerline of the rotating and stationary components? Then run analysis at multiple eccentricity values and based on the forces calculated on your rotor, extract the rotordynamic coefficients that way? Or just use XLRotor's XLHydrodyn program?
Christophe is offline   Reply With Quote

Reply

Tags
body, gap, mesh, movement, rigid

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Gambit problems Althea FLUENT 22 January 4, 2017 03:19
CFX Mesh Deformation problem Silmaril CFX 7 October 19, 2010 10:00
[snappyHexMesh] external flow with snappyHexMesh chelvistero OpenFOAM Meshing & Mesh Conversion 11 January 15, 2010 19:43
Convergence moving mesh lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 14:09
unstructured vs. structured grids Frank Muldoon Main CFD Forum 1 January 5, 1999 10:09


All times are GMT -4. The time now is 23:01.