CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Dynamic meshing in CFX: (negative volume error) (http://www.cfd-online.com/Forums/cfx/80760-dynamic-meshing-cfx-negative-volume-error.html)

vmlxb6 October 5, 2010 17:44

Dynamic meshing in CFX: (negative volume error)
 
How do I solve the problem of negative mesh and skewness problems in my case.
I am using tetrahedral elements for my case. Is the problem because of the high Re am using ??? My Re= 42900.

Is it the type of mesh am using causing the problem ???

FLUENT had the option of smoothing for dynamic mesh.....Is there any such option available in CFX ???

ghorrocks October 5, 2010 20:12

Negative volume elements has nothing to do with the flow, only the mesh. I assume you are using moving mesh. It just means you are moving the mesh too far and either need better smoothing or remeshing.

CFX automatically does mesh smoothing with moving mesh.

pratikmehta October 6, 2010 05:15

You need to setup a interrupt criteria in your solver tab in CFX pre to get your cell under control for min orthogonal angle aspect ratio more ever I think if you make sure your cells with min orthogonality angle of above 15 , you should be safe to avoid negative volume.


Best of luck

michael_owen October 6, 2010 14:43

OP,

A negative element volume error indicates that your mesh is folding. One of the nodes of an element has crossed the plane formed by the other three nodes. This occurs during mesh motion, when the motion of the mesh that you are imposing is too radical for the mesh diffusion to accomodate.

You need to determine where and why the mesh is folding and fix the problem. Set your job to complete one iteration before the error, and then post process the results. Use planes with mesh lines displayed (rendering tab) to see where the mesh is about to fold. You can possibly address this with the mesh stiffness options. You can make the mesh stiffer either near boundaries or in smaller volumes. There is an exponent that controls the sensitivity. The higher this exponent, the stiffer are the stiff regions of the mesh compared to the loose regions. Sometimes the mesh folds because the timestep is too large, or you need more mesh relaxation coefficient loops. Sometimes the motion is simply too radical and you will need to remesh. Try to plan out ahead of time what sort of mesh will allow you to efficiently capture your range of motion. Consider using sliding meshes if possible.

Lance October 7, 2010 02:34

Quote:

Originally Posted by michael_owen (Post 278141)
OP,

A negative element volume error indicates that your mesh is folding. One of the nodes of an element has crossed the plane formed by the other three nodes. This occurs during mesh motion, when the motion of the mesh that you are imposing is too radical for the mesh diffusion to accomodate.

You need to determine where and why the mesh is folding and fix the problem. Set your job to complete one iteration before the error, and then post process the results. Use planes with mesh lines displayed (rendering tab) to see where the mesh is about to fold. You can possibly address this with the mesh stiffness options. You can make the mesh stiffer either near boundaries or in smaller volumes. There is an exponent that controls the sensitivity. The higher this exponent, the stiffer are the stiff regions of the mesh compared to the loose regions. Sometimes the mesh folds because the timestep is too large, or you need more mesh relaxation coefficient loops. Sometimes the motion is simply too radical and you will need to remesh. Try to plan out ahead of time what sort of mesh will allow you to efficiently capture your range of motion. Consider using sliding meshes if possible.

Great post Michael, you should consider adding it to the FAQ.

vmlxb6 October 7, 2010 12:51

PratikMehta: My min Ortho. angle is 44.9 while aspect ratio and exp. factor is 6 and 12 respectively. So I don't think orthogonality should be a problem.

Ghorrocks: Thanks !! :)

Michael Owen: Where do i find the mesh relaxation coeff loop ??? Do you have any tutorial to implement sliding mesh ???

Thanks a lot guys !!!!!!!! APPRECIATE :)

michael_owen October 7, 2010 14:25

Quote:

Michael Owen: Where do i find the mesh relaxation coeff loop ???
Equation Class Settings tab of the Solver Control.

Quote:

Do you have any tutorial to implement sliding mesh ???
No, I generally don't have time to write tutorials unless they're for paying clients.

What is the nature of the motion you are trying to model?

vmlxb6 October 7, 2010 14:56

@ Michael Owen: My case is a study of flow over a cylinder surface and study of the vibrations (in the transverse direction only) of the cylinder due to the phenomenon of VORTEX induced Vibrations. my geometry is pretty simple just a rectangular box with the cylinder at the center over which the fluid flows.
The cylinder is restricted to move linearly in the vertical direction only.

Thanx a lot !!!

Regards

michael_owen October 7, 2010 15:38

Quote:

Originally Posted by vmlxb6 (Post 278334)
@ Michael Owen: My case is a study of flow over a cylinder surface and study of the vibrations (in the transverse direction only) of the cylinder due to the phenomenon of VORTEX induced Vibrations. my geometry is pretty simple just a rectangular box with the cylinder at the center over which the fluid flows.
The cylinder is restricted to move linearly in the vertical direction only.

Thanx a lot !!!

Regards

1) Make sure your cylinder is not simply crashing into a wall.

2) You probably need to reduce the model exponent for the mesh diffusion. The default value of 10 is way too high in my opinion. It means that the mesh will transform from very still to very loose very rapidly, causing a "front" to form in the mesh. In your model you should be able to set this to a much lower value, even 1.

michael_owen October 7, 2010 15:43

Also, it sounds like you're trying to do something like this:

http://www.youtube.com/watch?v=-2zsUMwDXx4

vmlxb6 October 7, 2010 19:31

@ Michael Owen
 
Its exactly the same problem am trying to do but just that my cylinder is restrained to move in the vertical direction only. Drag force is not taken into consideration, just the lift force. I am expecting a very large displacement bcoz of high Re.
Am expected to maximize by vibrations rather than suppress it !!!!!

BTW shouldn't increasing the model exponent number increase stiffness rather than loosen it ??? I presume from ur previous post the other way round.

Thanx Michael.

michael_owen October 12, 2010 15:36

Quote:

Originally Posted by vmlxb6 (Post 278368)
Its exactly the same problem am trying to do but just that my cylinder is restrained to move in the vertical direction only. Drag force is not taken into consideration, just the lift force. I am expecting a very large displacement bcoz of high Re.
Am expected to maximize by vibrations rather than suppress it !!!!!

BTW shouldn't increasing the model exponent number increase stiffness rather than loosen it ??? I presume from ur previous post the other way round.

Thanx Michael.

Increasing the model exponent increases the ratio of the stiffness in the stiffer regions to the stiffness in the looser regions.

vmlxb6 October 16, 2010 16:41

Re-meshing option !!!
 
I am trying to using the interrupt control for remeshing but cant get the expression right !!!!!!!!!!!!!! My re meshing condition expression is as follows:

(minVal(Volume)@Default Domain < 0.01 )

but am getting the error as:

CEL error:

The following unrecognized name was referenced: Volume

Bad expression value detected in parameter remeshingcond.

Can anyone tell me what should my expression for re-meshing be ???

michael_owen October 17, 2010 19:18

Quote:

Originally Posted by vmlxb6 (Post 279467)
I am trying to using the interrupt control for remeshing but cant get the expression right !!!!!!!!!!!!!! My re meshing condition expression is as follows:

(minVal(Volume)@Default Domain < 0.01 )

but am getting the error as:

CEL error:

The following unrecognized name was referenced: Volume

Bad expression value detected in parameter remeshingcond.

Can anyone tell me what should my expression for re-meshing be ???

Volume()@<3D region> is an integrative function; it is not a field variable.

You want minVal(Volume of Finite Volumes)@Default Domain

vmlxb6 October 17, 2010 20:45

@ Michael Owen
 
Hey Volume of Finite Volumes did work !!! but there is another error that I am getting. Once the interrupt control is called and re-meshing begins it does the following:

CFX Solver Results generated before remeshing have been written to: C:\Documents and Settings\vmlxb6\Desktop\16th Oct 2010\case 2_
trial\Unnamed_007\1_oldmesh.res


Text output generated during remeshing has been written to: C:\Documents and Settings\vmlxb6\Desktop\16th Oct 2010\case 2_
trial\Unnamed_007\1_remesh.out


An error has occurred in cfx5solve:


Unable to retrieve 1_remesh.out from working directory: Cannot
move to C:\Documents and Settings\vmlxb6\Desktop\16th Oct
2010\case 2_ trial\Unnamed_007\1_remesh.out: Permission denied



Why is it unable to extract the 1_remesh.out file ???




Thanks a lot man !!!! Appreciate


BTW I am following the following tutorial for re-meshing:


http://www.edr.no/blogg/ansys_blogge...cfx_re_meshing


Thanks and Regards,


VMLXB6

michael_owen October 17, 2010 21:14

Read the error. Your account don't have the correct permissions to move the file.

vmlxb6 October 17, 2010 21:16

@ Michael Owen
 
Does that mean that the problem is with the license and not the way I am re-meshing??????

michael_owen October 17, 2010 21:20

Well from the looks of it you have it trying to move the file to the same place it already is, which is probably generating the permission denied error.

vmlxb6 October 17, 2010 23:55

Any suggestions as to what I should be doing to solve this thing????????

ghorrocks October 18, 2010 06:12

You can also get this message when it cannot find the file. Don't forget CFX runs in a temporary directory so if you just use a local path for the def file (like ./file.txt) the solver won't find it as it is running in a temporary directory. You might need to use ../file.txt to go back a directory level.


All times are GMT -4. The time now is 16:02.