[foamF]

Hi, Formers.

I am simulating two gears in a rotating motion induced by a high velocity jet, with OpenFOAM v1712.

Since the gears are closely located with each other, I use the overset grid method to avoid the severe distorted grids in the tradition meshing technique. For this, I use overPimpleDyMFoam as the solver. For the flow induced rotation, I use rigidBodyMotion as the motion solver. Also, I use kOmegaSST as the turbulence model.

In the setup of overset grids, I combined 3 set of grids as individual zones - background, gear1 and gear2. A wall patch is used to define the shapes of gears.

I can manage to make both gears rotating. But, an unwanted situation happens: the gears collide with each other, or in other words, the meshes inside the wall of gears overlap.

Any experts can give me guidance on the model setting to avoid the unwanted gears overlapping? Thanks in advance.

[Lookid]

Hello, don't know how to solve this, but I saw this : https://www.youtube.com/watch?v=6rls...gsNmA&index=22

You might want to ask the author some info

[foamF]

Lookid, thanks for yr info.

i also saw this video before as well, but my case is a bit different. I think that the case in the youtube link is based on the user-defined rotational speed to make the gears to rotate. My case is the gears rotation driven by a high velocity jet.

[benchwell]

So your solid parts overlap, which is non-physical.



Did you check that your background-mesh and your gear-mesh are similar in resolution for proper interpolation and that the timestep is small enough? Ideally, per timestep the mesh should not move further than one grid cell in length (i.e. meshCO < 1).


Kind regards

[hxaxtma]

Did you add proper constraints to your DOF dict?

[foamF]

Originally Posted by benchwell

So your solid parts overlap, which is non-physical.



Did you check that your background-mesh and your gear-mesh are similar in resolution for proper interpolation and that the timestep is small enough? Ideally, per timestep the mesh should not move further than one grid cell in length (i.e. meshCO < 1).


Kind regards

The mesh resolution of background and gear in the overlapping regions is in similar order. I didn't check whether the time-step is small sufficient.

It is easy to understand that mesh resolution and time step affect the simulation results. But, I don't care about the results at the moment, since it is just a testing case for me to understand how overset grid works.

As u said, overlapping of the solid parts is non-physical. Do you know if the current code of overPimpleDyMFoam + rigidBodyMotion is able to simulate the contact of multiple objects so that no solid parts are overlapped, provided that the model setting is correct?

If the current code works, can you give me some hint how to do that?

[foamF]

Originally Posted by hxaxtma

Did you add proper constraints to your DOF dict?

I presume the DOF dict you means is dynamicMeshDict, pls correct me if I am not correct.

i didn't set any "restraint" in dynamicMeshDict. any hint from you how to set the contraints (or restraints) properly?

[hxaxtma]

Hi,

Two recommendations:

1) overPimpleFoam in current implementation should be able to handle your problem:
Minimum of 4 cell layers between bodies and chimera boundaries. Therefore 8 cells between wall boundaries in multiple overlapping regions! (2nd order interpolation!)

In your praticular case (close proximity) I would even recommend to double the minimum cell layers at least to 8 per region!

At the moment "no zero gap techology" is not implemented in OpenFOAM. A student of mine is working on this.

Make sure that your background meshes and chimera meshes at the interpolation regions are conformal in size!


2) I am not sure if you use a prescribed rotation motion or a 6DOF motion, where the rotation rate is a result of the incoming fluid flow forces. Anyway, a summary of the sixDoFRigidBodyMotion options of OpenFOAM can be found here:
https://openfoamwiki.net/index.php/P...onSolverFvMesh

If you gonna share your "simple" test case users here can also have a closer look.

[foamF]

Originally Posted by hxaxtma

Hi,

Two recommendations:

1) overPimpleFoam in current implementation should be able to handle your problem:
Minimum of 4 cell layers between bodies and chimera boundaries. Therefore 8 cells between wall boundaries in multiple overlapping regions! (2nd order interpolation!)

In your praticular case (close proximity) I would even recommend to double the minimum cell layers at least to 8 per region!

At the moment "no zero gap techology" is not implemented in OpenFOAM. A student of mine is working on this.

Make sure that your background meshes and chimera meshes at the interpolation regions are conformal in size!


2) I am not sure if you use a prescribed rotation motion or a 6DOF motion, where the rotation rate is a result of the incoming fluid flow forces. Anyway, a summary of the sixDoFRigidBodyMotion options of OpenFOAM can be found here:
https://openfoamwiki.net/index.php/P...onSolverFvMesh

If you gonna share your "simple" test case users here can also have a closer look.

hxaxtma, thanks for your advice.

The motion in my case is flow induced rotation, NOT prescribed rotation.

I tried to run with a finer mesh, but the results look more strange. I also tried to switch off the flow induced motion, but the results look strange again.

There should be something wrong in my setup with overset grid, but I couldn't figure it out.

My setup can be found in https://drive.google.com/open?id=1je...4l_20SyemIOx2c

Hope some experts here can give me some advice what's going wrong.

[hxaxtma]

I had a quick look at your case. There were some principle errors, best you just have a look at the running case I provided for a prescribed rotation motion based on your setup for laminar RAS model.

In principle the setup is running, few things to do:

- Adapt fvSolution and fvSchemes file to your turbulence model
- Small geometry issue in a corner of a gear which causes a floating point (no donor cells found)
- Set the inlet velocity to your needs, I put it to zero in order to check the velocity distribution due to rotation without superomposing mass flux through the inlet.

If I have time the next days I will also check your 6DOF dict.

Happy foaming

https://drive.google.com/file/d/1wKq...ew?usp=sharing

[foamF]

thanks, hxaxtma.

I took a look at your revised setup, and further did a hundred additional trials.

I tried to make the problem easier, changing back from two gears to one gear. The case is still flow induced rotation.

In short, I found an interesting problem with overset grid on my case: coarse grid result looks okay but fine grid result is unreasonable. Below is a detailed description:

Coarse grid scheme: nominal size 0.01m for both background and gear layers): the results look physical, which is qualitatively similar to my previous run on non-overset grid approach. This somehow indicates that my model setup works reasonably.

Fine grid scheme: nominal grid size 0.0075m for both background and gear layers: the result is very unreasonable. it appears that the model cannot realize the solid wall of gear; the flow field passes through the solid wall. When i use paraview to filter the cellTypes (based on a threshold filter from 0 to 1.5), no hole is gone.

Any experts can give me some advice? Thanks.

[foamF]

Hi all. End up, I tried to further refine the mesh by a halve locally (in the single gear case), and the model appears working normally.