[lbergmann]

Hi,

I am for the first time venturing in to the unknown land of moving meshes. I have followed the tutorial 22 with the ball check valve. My first problem is a very simple one:

I have a pipe with a ball in it. The ball doesn't fill out the pipe and water (or whatever other fluid I choose to use) can flow past it. I want to move the ball.

First I created a steady state simulation with no movement to use as input for the transient. The transient model I set up more or less exactly like the ball check valve tutorial.

The mesh is done by cutting as close as possible to the ball and doing multizone on the endpieces (theese should be able to deform quite a lot). The domain right around the ball is a tet-mesh. I specified that domain as a subdomain with moving mesh and the rigid body solution as the

I run with quite small time steps (1E-5) and it crashes before I can see any movement of the ball, ie second time step. The negative elements occur in domain on the inlet side, not where they should be compressed.

I am in doubt weather I should create stationary sub domains for the multizone regions.

[ghorrocks]

FAQ: http://www.cfd-online.com/Wiki/Ansys..._went_wrong.3F

Is this a pre-defined motion or rigid body?

[lbergmann]

This is a rigid body movement.

[ghorrocks]

Try running an even smaller time step. Debugging is much easier if you can get a single time step done so you can see the motion.

Also - is the immersed solid model suitable for this application? It is much simpler and does not require remeshing.

[lbergmann]

By lovering the velocity and the time step I managed to get four timesteps done (I get negativ elements in the fifth) done. I can now see the ball moving in the results file. Also now the negative element occurs on the side where the mesh is being compressed.

I assume I need to optimize the mesh I have an orthogonal angle of 33.9, expansion factor of 142 and an aspect ratio of 160.
The majority of the "bad" elements are due to inflation layers.

[ghorrocks]

Don't forget about the mesh motion parameters like increase stiffness near walls. This can help keep inflation layers together.

[lbergmann]

Thanks a lot. I managed to get an orthogan angle of 38.1, an expansion factor of 49 and an aspect ratio of 99.

I have tried increasing the stiffness with a model exponent of 2 both near boundaries and at small volumes. The result is the same. What would you suggest having the model exponent at?

[ghorrocks]

It is problem dependant. You have to try some values until you find one which works. Also look at the mesh motion diffusion variable as that can help see what is going on.

But in my experience problems like this are a sign that the meshing for mesh motion is not defined well. Can you show an image of how you have meshed this and what motion you expect to see?

[lbergmann]

I have created an Imgur album http://imgur.com/a/1hcit

Also; where do I find the mesh motion diffusion variable. I haven't heard about that one before?

[ghorrocks]

You will have more success with this I suspect if you make the inflation mesh/tet region region move with the sphere rigidly, and the extruded mesh on the left and right stretch to do your motion. It is much easier to keep extruded meshes working in mesh motion than inflation or tet meshes.

[lbergmann]

The tet mesh moves with the rigid body. The multizone mesh (is that what you call extruded mesh?) how do I get that to stretch if not just by "letting it be". Do I need to have no inflation on the multizone?

[lbergmann]

I just tried taking the inflation layers off on the whole geometry, this is not perfect obviously, but it is now running on the 11'th iteration, so it did fix something.

[ghorrocks]

Have a close look at the mesh as it is running. You will probably see large mesh deformations in the same region the other mesh was failing at.

[lbergmann]

How do I look at the mesh deformation while it is running?

I crashed after 13 iterations

[lbergmann]

Another problem:

When I want to visualize the movement of the ball I don't see any movement until the last timestep (the one that crashes) This is true for all of the runs.

[ghorrocks]

Quoting from the FAQ (http://www.cfd-online.com/Wiki/Ansys...ent_wrong.3F):

On the Output tab, go to "Transient Results Files" and set it to save a results file every time step. To keep the file size manageable, select "Include mesh", but make it "Selected Variables" and select no variables.

If nothing happens then it suddenly starts moving and crashes this could also be a rigid body motion problem. Are you sure you have reasonable values for the mass of the body and all the moments of inertia? Are you sure your fluid model is stable or does it go bezerk? It would be good to put some monitor points looking at things like the rigid body motion and flow conditions so you can see if something goes crazy near the crash.

[lbergmann]

I have the same velocity and mass for the ball as in the tutorial I was following. I was monitoring the mass flow and that looks fine. Will try to monitor the velocities as well.

[lbergmann]

I can't seem to get it to plot the mesh while solving? It just shows the monitors as normal.

[ghorrocks]

You have to load the results files in the post processor. They are not shown as the simulation progresses

[lbergmann]

I am not sure if I managed to plot the mesh or what I did here. If I did it does not compress the mesh in the mapped regions.

I showed the regions and picked "Draw as lines" under Render.

I have created another album with the snaps http://imgur.com/a/TdM8V

Thank you so much for all your help. I feel completely hopeless at this.