CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM

OpenFOAM - Problem on double gears flow induced rotation

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 10, 2019, 06:10
Default OpenFOAM - Problem on double gears flow induced rotation
  #1
Member
 
Join Date: Aug 2018
Posts: 43
Rep Power: 3
foamF is on a distinguished road
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.
foamF is offline   Reply With Quote

Old   June 10, 2019, 08:15
Default
  #2
Member
 
Lilian Chabannes
Join Date: Apr 2017
Posts: 52
Rep Power: 4
Lookid is on a distinguished road
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
__________________
Feel free to join the OpenFOAM Discord https://discord.gg/P9p9eHn, a live chat about OpenFOAM
Lookid is offline   Reply With Quote

Old   June 10, 2019, 09:34
Default
  #3
Member
 
Join Date: Aug 2018
Posts: 43
Rep Power: 3
foamF is on a distinguished road
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.
foamF is offline   Reply With Quote

Old   June 11, 2019, 07:48
Default
  #4
New Member
 
Felix Weiler
Join Date: Nov 2016
Location: Bremen
Posts: 14
Rep Power: 4
benchwell is on a distinguished road
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
benchwell is offline   Reply With Quote

Old   June 11, 2019, 08:22
Default
  #5
Senior Member
 
Join Date: Jan 2014
Posts: 157
Rep Power: 7
hxaxtma is on a distinguished road
Did you add proper constraints to your DOF dict?
hxaxtma is offline   Reply With Quote

Old   June 11, 2019, 11:27
Default
  #6
Member
 
Join Date: Aug 2018
Posts: 43
Rep Power: 3
foamF is on a distinguished road
Quote:
Originally Posted by benchwell View Post
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 is offline   Reply With Quote

Old   June 11, 2019, 11:33
Default
  #7
Member
 
Join Date: Aug 2018
Posts: 43
Rep Power: 3
foamF is on a distinguished road
Quote:
Originally Posted by hxaxtma View Post
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?
foamF is offline   Reply With Quote

Old   June 11, 2019, 13:45
Default
  #8
Senior Member
 
Join Date: Jan 2014
Posts: 157
Rep Power: 7
hxaxtma is on a distinguished road
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 is offline   Reply With Quote

Old   June 12, 2019, 04:13
Default
  #9
Member
 
Join Date: Aug 2018
Posts: 43
Rep Power: 3
foamF is on a distinguished road
Quote:
Originally Posted by hxaxtma View Post
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.
foamF is offline   Reply With Quote

Old   June 12, 2019, 09:26
Default
  #10
Senior Member
 
Join Date: Jan 2014
Posts: 157
Rep Power: 7
hxaxtma is on a distinguished road
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
hxaxtma is offline   Reply With Quote

Old   June 13, 2019, 05:55
Default
  #11
Member
 
Join Date: Aug 2018
Posts: 43
Rep Power: 3
foamF is on a distinguished road
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 is offline   Reply With Quote

Old   June 17, 2019, 21:40
Default
  #12
Member
 
Join Date: Aug 2018
Posts: 43
Rep Power: 3
foamF is on a distinguished road
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.
foamF is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
compiling udf for pulsatile flow Akshat Fluent UDF and Scheme Programming 1 June 21, 2018 04:07
How to contribute to the community of OpenFOAM users and to the OpenFOAM technology wyldckat OpenFOAM 17 November 10, 2017 15:54
Can not achieve statistically steady flow in Openfoam jiaodanuma OpenFOAM 0 August 16, 2016 06:49
OpenFOAM : flow around a sphere at low Reynold number maxou1993 OpenFOAM Running, Solving & CFD 1 July 7, 2015 05:13
segmentation fault--parrallel problem? donno OpenFOAM Running, Solving & CFD 2 March 20, 2015 21:23


All times are GMT -4. The time now is 11:27.