Unresolved Negative Element Volume Error
 

Dear all,
I am modelling blood flow in a realistic artery model. The middle section of the artery starts to gradually narrow from t=0 to t=0.4s and then from t=0.4s to t=1, it returns to its initial state. At t=0.16s, I got "negative element volume" error. As suggested in FAQ, I tried the following steps to resolve this problem:
1- Refined the mesh to get a better fluid mesh
2- Mesh stiffness: 1 [m^3 s^-1]/Wall Distance, and 1 [m^5 s^-1]/Volume of Finite Volumes
3- Reduced time step from 0.01 to 0.0025 and to 0.001

None of these methods helped and still got the same error at around 0.16s. I've also done the debugging described in the FAQ. An image of deformed artery at t=0.16s is attached here. The red color represents the section of the artery which narrows. The blue parts of stationary.
http://tinypic.com/r/10qf9ci/8

It would be appreciated if anyone could help me to solve this issue.

Thanks

Check the exported mesh on every timestep to get an idea where the neg. volume is located - AND definitely set the mesh movement calculation to reach a sufficient order of convergence (<1e-5 max) or even lower.

Thanks Matthias. How can I check the location of negative volumes. What I did is just save the mesh every time step, but I do not know how to find the negative volumes in CFD-Post?? Can you please elaborate more?

Check for the worst angles.. they should be right next to the distorted/negative elements.

Dear Matthias- I've located the worst angle elements. As seen in the attached image, they are at boundaries between the stationary and moving parts.

http://tinypic.com/r/14dne47/8
As suggested, I also reduced the convergence criteria for mesh movement (5e-6), but it did not help.
In this case, Do you have any other idea which could help for converging my moving mesh problem. Thanks

I had that issue recently in a square corner betwwen two walls. I was using too thick layer (inflation) of too many prisms on the wall. Where these tow layers meet and tetrahedra starts, a negative volume was generated... By reducing the number of inflation layers the problem dissapeared. Did not have that issue in the CFX v. 13.0 only in 14.0. Who know's what it was.

Have you tried to Plot your Interface pressure / wall pressure? Does it oscillate before it crashes? Have you tried it without inflation layers? It is often the problem that the solver does not remesh the transition tetras and the elements crash. With only one type of elements, that problem doesn't occur. It's not that you have to do the final calculation without inflation, but it helps determine the cause of the error.

Dear Kina. I have not used inflation, the mesh consists of pure tetra elements. What do you mean by interface pressure, is it pressure between stationary and moving parts?

interface pressure is the integrated wall pressure at your artery wall. what version are you using? when the pressure is oscillating, there might be stability issues. what velocity / pressure are you using initially? have you thought about UDFs to ramp that value up to get smaller initial deformations?

I am using ANSYS CFX 14.5.
I use pressure waveform as inlet and outlet BCs. What I did, first I solved the problem as steady and then used the results as the initial condition for the transient analysis. I expect to have 36% contraction in the middle section of the artery. I defined an expression to ramp the deformation so that the amount of deformation gradually rise up. Actually, I could have converged this problem in a pipe with structured mesh, but in the real model due to the complexity, I had to generate unstructured mesh and have not been able to converge it yet. I have tried several methods to get rid of negative elements like Refining the mesh, using Mesh stiffness and reducing time step. However, still getting the same error.

If your mesh motion is large enough that you keep getting negative volume elements, then you should consider dynamic remeshing using mesh quality as a trigger.

Dear Glenn,
I used remeshing method to get rid of the negative element volume, but I still get this error after three times remeshing. Do you have any idea to get better results

Thanks

Have you looked at where the neg volume elements are occuring? I bet something about your meshing setup is causing a wonky mesh.

Yes, it occurs on the interface between undeformed and deformed segment, as shown by circle in the following image. The middle part (dark blue) shows the deforming segment and the light blue shows the stationary part.
http://tinypic.com/r/14kayh4/8

I used tetra mesh with element size 0.2[mm] and low smoothing.
Do you have any recommendation to get a better mesh?

The image was not attached.

sorry. here it is

http://tinypic.com/r/14kayh4/8

Dear Glenn, the other problem is related to minimum mesh orthogonality.
Minimum orthogonality of my initial mesh was 6.6, I defined a minimum orthogonality angle<6 [deg] as the interrupt control. As the orthogonality drops below the 6 [deg], the remeshing starts, but surprisingly the minimum orthogonality angle keeps decreasing (please see the attached graph for minimum orthogonality angle) and finally the solver gives negative element volume error. I think after the remeshing the minimum orthogonality angle should increase as a new mesh is created, but in my case it keeps decreasing even after remeshing.

http://tinypic.com/r/v6rurq/8

The image loink was in the email alert but stripped from the forum post. I will try to post it again for you: http://tinypic.com/r/14kayh4/8

By the way, you cna post images directly in the forum in the "Go Advanced" button. No need for external sites. (I know the FAQ says you should use external sites, I should update that.)

But I cannot see any useful detail in your image, I have no idea what it is showing.

What is probably happening is that the position of the new mesh means the mesher is unable to generate a high quality mesh. It looks like the way you have connected the deforming part to the non-deforming part is a problem as well. Are you sure it generates a step like that? You model a step very differently to a gradual squeezing (ie GGI versus just deformation).

Thanks Gelnn.
Actually the interaction between the deformed and non-deformed should not be like a step. I did the same simulation in an idealised model for which I defined an expression to create a smooth transition between non-deformed and deformed sections. However, in the real model I have no idea how I can create a smooth transition.
As you mentioned, if I find a way to create a smooth transition between deformed and non-deformed sections, then my problem most likely will be solved. Do you know how I can do that in the real model.

Replace the step with a short section where the wall condition is defined as "unspecified" motion. The mesh smoother will then transition it from the fully moving mesh to the stationary mesh.