[awesim]

Hello everyone,

I encountered a problem at the beginning of my simulation. The solver found a negative sector volume and hence exited.
I'm modeling moving meshes and I am pretty much sure that the mesh is alright.

I also know that there's an expert parameter that prevents the solver from crashing when finding a negative sector volume because of another simulation I reviewed that also had a negative volume in it.

There it says: This warning (the negative volume warning) may be made fatal by setting the expert parameter 'negative volume option = 1'.

Does anyone know where to edit this parameter? I am not able to find it, either in CFX-Pre or in any help document.

If I could tell the solver to not exit when finding a negative sector volume my simulation should be able to run.


Thanks and kind regards,
Simon

[Felipe Mendes]

Dear Awesim, I don't know how to activate this parameter.
But maybe you could prevent the moving mesh from producing these undesirable negative volumes by setting a higher value of "Mesh Stiffness" with the "mesh motion model". Have you tried that?

[Opaque]

The warning is there for important reasons. If you understand the details of the discretization, you may be able to know how a negative volume sector may degrade the quality of the solution.

A negative volume sector may be due to corrupt topology, way too skewed elements, etc. Removing the warning opens the door for unpredictable solutions; otherwise, developers would have ignored the issue the same way you are attempting to do.

[ghorrocks]

I agree with Opaque, if you remove this error you will get divergence in the linear solver instead so you have not gained much. Better to fix the underlying problem and stop the negative volume elements.

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

[awesim]

Thanks for your help.

No Felipe, I haven't tried that. I'm not modeling any Mesh Deformation; "just" a two stage turbine with moving blade rows. Could it help to adjust the Stiffness here?

Opaque and Ghorrocks, I know that removing the warning is not the best way to deal with this problem. I certainly have undesirable elements in my mesh due to my meshing approach. Maybe you can give more advise if I explain my setup more detailed.

I'm trying to create unstructured meshes for a two-stage turbine. It's part of my masters thesis that I compare those unstructured meshes to structured ones.
The blades I'm modeling are shrouded. So my idea was to create a hybrid mesh that consists of a sweeped quasi-structured mesh where the labyrinth seal is and a tetra-mesh in the main passage where the blade is. The sweeping should prevent the mesher to create too many tetra-elements in the sealing-region since my focus is not on the flow topology in that area. But because of that the cells in this region always have large aspect ratios and hence bad quality.
Another problem is the connection between the two meshes. I want to get a 1:1 connection to avoid using an interface, but the transitional elements always seem to be a lot skewed.
Last but not least the geometry I got is not really great. The trailing edge is very thin, the fillet radii were modeled "by hand" (using free surfaces) and at some points there are sharp edges or holes. I tried to fix all that in the workbench design modeler, but as you can see there's plenty of opportunities for the mesher to fail.

So, what I'm trying to say: It will be hard for me to obtain a good mesh, but of course I won't stop trying (at least not until the time for my thesis runs out haha).
So if there's a chance to ignore the warning so that I could see how the simulation behaves on this mesh, I would gladly take it.

Sorry for my long post, just wanted to give you a hint of what I'm dealing with. If you're interested I can possibly post some pictures as well.


Thanks and regards,
Simon

[Chris_321]

Why dont you use a Rotating Reference Frame? Its mutch easier than a moving mesh simulation.

[ghorrocks]

Negative volume elements are a problem in moving mesh simulations. But your simulation does not sound like moving mesh - it sounds like a fixed mesh (or maybe a rotating frame of reference, but that is a different model to moving mesh).

In this case you definitely should not be getting negative volume elements. It means that your meshing is poor. You MUST fix these problems in the mesher. They most commonly come about when you do too much smoothing on the mesh and some elements go inside out. I would recommend not doing any manual smoothing at all and just use the meshes the tet/hybrid mesher gives you.

If you are modelling thin regions (eg into the seals) then you cannot mesh this nicely with tets. You will want to use a structured mesh in this region so you can stretch the mesh to reduce the element count. And then you need to interface the seal mesh with the main mesh, either with an interface, or if you are proficient at meshing you can make it contiguous so you do not need an interface.

On second read it appears you are using moving mesh to model a rotating simulation - as Chris says you should be using rotating frames of reference, not moving mesh. Then you will not have negative volume errors.

[awesim]

Yes, I'm using rotating frames indeed. I thought it was the same as doing a moving mesh, sorry for the confusion!

I actually found a negative element in my mesh and am trying to fix it now.

I'm not doing manual smoothing since I use the Workbench Mesher. But I will try meshing without any smooting and see where it takes me.

That was my idea too, that I can't mesh the seal region properly with tet's. Right now I'm trying to obtain a 1:1 connection but when there's no other choice I will have to use a GGI instead. This should also solve the negative volume problem since it appears that these elements are within the transition region of the different meshes.

Will keep you updated, thank you so far!

[awesim]

So I was actually able to get rid of the negative volume by adjusting my meshing options! I haven't tried to run another simulation because I think I will first look for problems in every other mesh too.

I could fix it by forcing certain edges to be meshed with a prescribed amount of nodes.

If I'm able to fix all meshes and start another simulation I'll come back to you.

Edit: The Simulation is working now, it really was a problem with the mesh.

Thanks and regards,
Simon

[Bdew8556]

hey there!

What meshing parameters did you change? if you can recall.

Brett

[ghorrocks]

The adjustments required to fix a specific case are unlikely to work in other cases. If you describe your problem we might be able to help you.

[Bdew8556]

Thanks Greg, my fellow Australian I believe...

Basically I'm doing centrifugal compressor simulations and I had previously come up with a set of mesh parameters that worked nicely and produced no errors.
I've since moved on to analysing a new compressor of a larger size, the blade contours/angles remain unchanged.
For some reason I now get the following error:

ERROR
Mesh Elements with negative volumes detected in domain Passage.

I've never seen this before.

Any thoughts?

[ghorrocks]

The name's Glenn actually

Negative volume error is a FAQ: https://www.cfd-online.com/Wiki/Ansy..._went_wrong.3F

Why are you doing a moving mesh simulation of a compressor? What are you trying to model?

[Bdew8556]

Thanks Greg,

Well to my knowledge im not doing a moving mesh simulation, that's added to my confusion.

It's just a standard centrifugal compressor model. Inlet domain: stationary, impeller domain: rotating, outlet domain: stationary. Frozen rotor interfaces between.

[ghorrocks]

My name is still Glenn, and has not been Greg for some time

Check that you have not activated the moving mesh options. Also check you are modelling this using rotating frames of reference, not moving mesh. If that is all OK then your meshing software appears to have generated an invalid mesh with inside out elements. You will need to fix this inside the meshing software as CFX cannot do anything about it.

[Bdew8556]

sorry Glen, my mistake.

Where abouts is the option to activate the moving mesh?

[ghorrocks]

In the domain tab.

[Bdew8556]

Thanks Glen,

Looks like I have no mesh deformation set so it can't be that.
Any other thoughts?

Brett

[ghorrocks]

As I said a few posts ago....

If that is all OK then your meshing software appears to have generated an invalid mesh with inside out elements. You will need to fix this inside the meshing software as CFX cannot do anything about it.