[abhishek_patil_06]

Hi
I'm doing transient analysis of electronic throttle valve. In case setup of this problem i used morphing(motion wise) and rotation motion. With the help of this two motion i'm able to generate rotational motion of throttle plate, but unable to realign the mesh after some degree of rotation and because this after 10 degree rotation some cells are going in negative volume. Is anyone done this type of simulation or know how to realign the mesh in star ccm+?
For better idea attaching the screenshotsafter rotaion.PNG

before rotation.PNG

[Fiedde1887]

I would create a Threshold with bad cell Quality or high skewed cells and create a stopping criteria with that. After that you can create a macro wich tell the Simulation to mesh - run until criteria is realised - mesh - run ...etc.
I think, that should work

[Schwob77]

The method to simply remesh after a certain threshold for a mesh metric is reached will not help here. Instead of remeshing the current position of the volume mesh the initial position of it will be remeshed. The reason is that the volume mesh is always created from the provided geometry which doesn't move together with the volume mesh.
If you want to remesh from the current position of the volume mesh you need to extract the surface mesh from it by a right-click on the Representation->Volume Mesh->Extract Surface. This will create a new Surface Representation that represents a triangulted version of the volume mesh surface. You can now export it and re-import it to REPLACE the old initial surface to remeesh from there. Depending on your geometry tree structure this can be tedious because you possibly don't have the same structure under parts than under regions.
The second problem with this method is that you slightly modify the geometry with each remeshing step as curved surfaces get shrinked or stretched. The third problem is that it's irreversible because with every remeshing step you replace the initial geoemtry of the previous step and cannot go back to it.

Instead of that I would look into the morpher setup in the first place. It seems that you have only applied a motion to the valve itself. The planar surface at the bottom and top seem to have a fixed boundary conditions. This leads to bad meshes after only a few timesteps. A better solution is to apply a "Fixed Plane" or "In-Plane" condition to them. "Floating" is possible as well but not very accurate. If your motion is only small this is maybe enough for your setup. Otherwise I would think about using sliding or overset interface to allow larger displacements.

[abhishek_patil_06]

Thank you for your response.
In plane or fixed plane option will not work because my wall is circular. As you suggested i tried floating option but it doesn't work, you will get idea by seeing this screenshot while using floating option.Floating.PNG

floating_cross.PNG

[Schwob77]

In this case I would use "slide on guide surface" for the boundary. That one will keep them on the surface but still allow a motion to avoid bad skewness after each timstep.

[me3840]

Originally Posted by Fiedde1887

I would create a Threshold with bad cell Quality or high skewed cells and create a stopping criteria with that. After that you can create a macro wich tell the Simulation to mesh - run until criteria is realised - mesh - run ...etc.
I think, that should work

In my experience this is really unreliable. It's much better to make a macro that detects negative volume cells when they occur.

As far as this problem goes, you can probably use slide on guide surface. An alternative is using overset.

[abhishek_patil_06]

Thanks for your response.
I tried with slide on guide surface, it worked up to 55 degree of rotation after that cells are going in negative volume. when i seen cross section of mesh came to know that mesh is not realigning just simply stretching or compressing the cells. Is there any option to realign the mesh after particular skewness? Or can we write macro if so please explain me some basic step as i'm new to this
after rotaion.PNG

before rotation.PNG

[ping]

i would be doing this with zero gap overset mesh and this will get around all your mesh distortion issues and no need to remesh

but if you really want to continue with the painful remeshing route then i suggest you don't use extract surface since this changes the surface slightly at every extraction

the modern way of doing this is to use parts based meshing operations - you need to report on the angle of the throttle and at remesh time you transform the throttle part to the new angle and then do the remesh and then tranform it back so that it is in the starting position for the next reported angle for another remesh

[Schwob77]

I have no macro at hand that I could share with you. However in general the degree of deformation you show here indicates that it would be something for an overset mesh setup.

[abhishek_patil_06]

Hi Ping
As you suggested i did overset mesh with zero gap. When i diagnose the mesh there was no error, but when the solution was initialized some cells near the throttle plate and body wall were becoming in active. Due to this problem solution is diverging. You can see it below images.can you suggest me how to troubleshoot this error? Before initialization.JPG

After initialization.JPG

Cross section.JPG

[ping]

you need to search the steve support portal for overset and read the good article on how to debug overset cases ie view the overset representation and look for where the various cell types are and ensure hole cutting has happened correctly