Problem with mesh movement in small gap

Fred_Erik · February 27, 2018, 10:42

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

ghorrocks · February 27, 2018, 16:03

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.

Christophe · February 27, 2018, 19:13

image1.jpg you can make an artificial wall where the fluid mesh will pass through and not pinch by putting in a immersed solid.

Fred_Erik · February 28, 2018, 11:51

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

Christophe · February 28, 2018, 16:48

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?

February 27, 2018, 10:42	Problem with mesh movement in small gap	#1
Fred_Erik New Member Join Date: Mar 2014 Posts: 8 Rep Power: 12	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

February 27, 2018, 16:03		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	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.

February 27, 2018, 19:13	use immersed solid as sink for pinch region	#3
Christophe Member Join Date: Jan 2015 Posts: 62 Rep Power: 11	image1.jpg you can make an artificial wall where the fluid mesh will pass through and not pinch by putting in a immersed solid.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Gambit problems	Althea	FLUENT	22	January 4, 2017 04:19
CFX Mesh Deformation problem	Silmaril	CFX	7	October 19, 2010 11:00
[snappyHexMesh] external flow with snappyHexMesh	chelvistero	OpenFOAM Meshing & Mesh Conversion	11	January 15, 2010 20:43
Convergence moving mesh	lr103476	OpenFOAM Running, Solving & CFD	30	November 19, 2007 15:09
unstructured vs. structured grids	Frank Muldoon	Main CFD Forum	1	January 5, 1999 11:09

February 28, 2018, 16:48		#5
Christophe Member Join Date: Jan 2015 Posts: 62 Rep Power: 11	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?