engaged rotating gear in multiphase flow

wjy-c · August 28, 2013, 01:18

Hi, recently i'm trying to simulate oil splashing caused by rotating gear.

At the beginning, I was recommended that rotate frame reference is a good choice, but after a few attempts, there is a problem that how could rotate frame reference simulate the process of gear engagement? In addition, i also tried the immersed solid, but the CFX help document says the immersed solid model is not suitable for multiphase flow.

So, as far as i know, in CFX i could only set the gear pair as rigid body which i read a similar case in CFX tutorial 32 (modeling a buoy using the CFX rigid body solver), i have not done any thing using rigid body, so i was wondering if i can read temperature messaged on rigid body?

Moreover, i think in my situation, mesh adaption must be needed to combined with rigid body solution, i do not quite understand mesh adaption neither, i also want to know whether my method of rigid body with mesh adaption is correct for my model? The most concerned result is temperature, and i would do some experiment to check the CFX simulation result.

after all i mentioned above, is there some other method i do not know? please let me know, also, for start, i would like to do a gear pump simulation to master the ways of rigid body and mesh adaption, do anyone have some similar gear pump model for me to study? or do you have any suggestion? Thank you very much!! !

ghorrocks · August 28, 2013, 02:52

This is easily done using immersed solids (I think there is a tutorial on exactly this) but that cannot work with multiphase. If you want to run this multiphase I fear your only option is remeshing.

As the geometry is highly periodic you might be able to do this with several meshes with the gears at various mesh points. Then you run that mesh for a few degrees of rotation before switching to the next pre-meshed mesh points. This means you do not need to do dynamic remeshing, just run over a series of pre-meshed geometries.

wjy-c · August 28, 2013, 04:32

Hi,ghorrocks. Thanks for your reply.

I do not understand what you mean by mesh points? do you mean i can divide the whole time of this transient process of gear engagement into several smaller time process,and calculate each time process?

my model is a complicated gear box, and i'm going to figure out the velocity and temperature during the oil splash lubrication, and finally i will evaluate the performance of the oil splash lubrication in the gear box. so there are five pair of gear engagement participated in the process and only one or two big gear involved in oil agitating. so i do not know whether the method you offer could work in this complicated situation.

ghorrocks · August 28, 2013, 07:40

No, it would not be practical if you are modelling an entire gearbox. And modelling the detailed oil splashing with any method would not be practical either. I suggest you are going to have to simplify this somewhat to make it possible - for instance by removing the teeth on the gears and using tangential velocity conditions on the gears instead of rotating gears (so using a stationary mesh) or soemthing like that.

This sounds like a very challenging simulation so I hope you are not expecting quick answers.

wjy-c · August 28, 2013, 09:39

Thank you.
I know it is a big challenge, today, in stationary domain, i set the gears as immersed solid with rigid body solution, and it works. i'm not sure the results is proper or not, maybe experiment would help. if the results is far too ridiculous, rotate frame reference seems to be my only choice. Otherwise, maybe i should try fluent to do my job. thank you again for all your answer.

ghorrocks · August 28, 2013, 19:06

Read my previous post carefully - if you remove the teeth from the gears then you do not need rotating frame of reference or immersed solid, it can be done as a "simple" stationary mesh simulation with multiphase.

You will not be able to do this simulation with rotating frames of reference - at least not with meshing gears.

brunoc · August 28, 2013, 22:22

If you have the option, run this simulation in FLUENT. As mentioned by Glenn, the only way to correctly run this in CFX is by constantly remeshing your domain, and that will be impractical. Running in FLUENT will also require remeshing, but depending on your geometry you could run it in 2D plus the remeshing process is handled by the solver itself and only done on the regions of your mesh that require it. From experience it should take about a quarter to half the computational effort required by CFX for the same problem using a 2.5D mesh.

If you do have to run it with CFX, the pre-generated meshes approach will be your best option.

ghorrocks · August 28, 2013, 22:31

Post #3 suggests this is a complex gearbox with 5 gears. Presumably they are in a 3D arrangement not suitable to be simplified to 2D.

I doubt this model can be done in any CFD code including the gear teeth. The mesh required to get that level of detail accurate sounds impossible to me. So my suggestion is to remove the teeth from the gears and run it as a stationary mesh (with tangential velocities on the gears). This is straightforward and CFX/Fluent should be well capable of this. But you might need to add a source term to model the effects of the gear teeth. This is the only way I can see to make this model realistic.

wjy-c · August 30, 2013, 00:08

Hi. ghorrocks, thanks for your advice.
i have made a small simplified model to try your suggestion. on the stationary cylinder surface wall, i set the wall velocity with radial component and theta component, but the CFX Slover says that"the angle between the specified velocity and the element surface is 87 degree at this face, and the error implies the mesh is moving". i do not understand why, is my wall velocity setting applied to the girds near the wall rather than the water and air? if so, where should i set the velocity?
i'm looking forward to your replies. thanks a million!

wjy-c · August 30, 2013, 00:15

Hi, Brunoc. I read a similar 2D-gear pump example in fluent using your way. i do not know much about Fluent, as Ghorrocks mentioned above, is the available in my complicated 3-D gearbox model with several engaged gears. if it works, maybe i should learn Fluent. Thank you!

ghorrocks · August 30, 2013, 07:58

Your error message simply means you made a mistake setting the tangential velocity. It is saying it is not tangential.

As I said in my post #8 I do not think the model you propose (modelling the actiual gear teeth) is going to be possible in any CFD code. You might be able to get some code to handle the remeshing and all the other stuff, but there is no way you are going to be able to get the mesh fine enough to resolve the flow features in this model. You are going to have to simplify it.

August 28, 2013, 01:18	engaged rotating gear in multiphase flow	#1
wjy-c New Member Jingyao Wang Join Date: Jun 2013 Posts: 29 Rep Power: 13	Hi, recently i'm trying to simulate oil splashing caused by rotating gear. At the beginning, I was recommended that rotate frame reference is a good choice, but after a few attempts, there is a problem that how could rotate frame reference simulate the process of gear engagement? In addition, i also tried the immersed solid, but the CFX help document says the immersed solid model is not suitable for multiphase flow. So, as far as i know, in CFX i could only set the gear pair as rigid body which i read a similar case in CFX tutorial 32 (modeling a buoy using the CFX rigid body solver), i have not done any thing using rigid body, so i was wondering if i can read temperature messaged on rigid body? Moreover, i think in my situation, mesh adaption must be needed to combined with rigid body solution, i do not quite understand mesh adaption neither, i also want to know whether my method of rigid body with mesh adaption is correct for my model? The most concerned result is temperature, and i would do some experiment to check the CFX simulation result. after all i mentioned above, is there some other method i do not know? please let me know, also, for start, i would like to do a gear pump simulation to master the ways of rigid body and mesh adaption, do anyone have some similar gear pump model for me to study? or do you have any suggestion? Thank you very much!! !

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
mesh size in Eulerian multiphase flow - liquid/solid mixture	microfin	FLUENT	4	December 23, 2016 14:55
Multiphase Flow	Pavlos	FLUENT	0	August 8, 2011 09:43
Multiphase flow in atomiser	santhosh1987	FLUENT	0	May 12, 2011 05:26
Multiphase flow & porous media	Hisham	OpenFOAM	3	April 10, 2011 08:04
Multiphase flow problem	icedou	FLUENT	6	July 10, 2005 03:52

August 28, 2013, 02:52		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,872 Rep Power: 144	This is easily done using immersed solids (I think there is a tutorial on exactly this) but that cannot work with multiphase. If you want to run this multiphase I fear your only option is remeshing. As the geometry is highly periodic you might be able to do this with several meshes with the gears at various mesh points. Then you run that mesh for a few degrees of rotation before switching to the next pre-meshed mesh points. This means you do not need to do dynamic remeshing, just run over a series of pre-meshed geometries.

August 28, 2013, 04:32		#3
wjy-c New Member Jingyao Wang Join Date: Jun 2013 Posts: 29 Rep Power: 13	Hi,ghorrocks. Thanks for your reply. I do not understand what you mean by mesh points? do you mean i can divide the whole time of this transient process of gear engagement into several smaller time process,and calculate each time process? my model is a complicated gear box, and i'm going to figure out the velocity and temperature during the oil splash lubrication, and finally i will evaluate the performance of the oil splash lubrication in the gear box. so there are five pair of gear engagement participated in the process and only one or two big gear involved in oil agitating. so i do not know whether the method you offer could work in this complicated situation.

August 28, 2013, 07:40		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,872 Rep Power: 144	No, it would not be practical if you are modelling an entire gearbox. And modelling the detailed oil splashing with any method would not be practical either. I suggest you are going to have to simplify this somewhat to make it possible - for instance by removing the teeth on the gears and using tangential velocity conditions on the gears instead of rotating gears (so using a stationary mesh) or soemthing like that. This sounds like a very challenging simulation so I hope you are not expecting quick answers.

August 28, 2013, 09:39		#5
wjy-c New Member Jingyao Wang Join Date: Jun 2013 Posts: 29 Rep Power: 13	Thank you. I know it is a big challenge, today, in stationary domain, i set the gears as immersed solid with rigid body solution, and it works. i'm not sure the results is proper or not, maybe experiment would help. if the results is far too ridiculous, rotate frame reference seems to be my only choice. Otherwise, maybe i should try fluent to do my job. thank you again for all your answer.

August 28, 2013, 19:06		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,872 Rep Power: 144	Read my previous post carefully - if you remove the teeth from the gears then you do not need rotating frame of reference or immersed solid, it can be done as a "simple" stationary mesh simulation with multiphase. You will not be able to do this simulation with rotating frames of reference - at least not with meshing gears.

August 28, 2013, 22:22		#7
brunoc Senior Member Bruno Join Date: Mar 2009 Location: Brazil Posts: 277 Rep Power: 21	If you have the option, run this simulation in FLUENT. As mentioned by Glenn, the only way to correctly run this in CFX is by constantly remeshing your domain, and that will be impractical. Running in FLUENT will also require remeshing, but depending on your geometry you could run it in 2D plus the remeshing process is handled by the solver itself and only done on the regions of your mesh that require it. From experience it should take about a quarter to half the computational effort required by CFX for the same problem using a 2.5D mesh. If you do have to run it with CFX, the pre-generated meshes approach will be your best option.

August 28, 2013, 22:31		#8
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,872 Rep Power: 144	Post #3 suggests this is a complex gearbox with 5 gears. Presumably they are in a 3D arrangement not suitable to be simplified to 2D. I doubt this model can be done in any CFD code including the gear teeth. The mesh required to get that level of detail accurate sounds impossible to me. So my suggestion is to remove the teeth from the gears and run it as a stationary mesh (with tangential velocities on the gears). This is straightforward and CFX/Fluent should be well capable of this. But you might need to add a source term to model the effects of the gear teeth. This is the only way I can see to make this model realistic.

August 30, 2013, 00:08		#9
wjy-c New Member Jingyao Wang Join Date: Jun 2013 Posts: 29 Rep Power: 13	Hi. ghorrocks, thanks for your advice. i have made a small simplified model to try your suggestion. on the stationary cylinder surface wall, i set the wall velocity with radial component and theta component, but the CFX Slover says that"the angle between the specified velocity and the element surface is 87 degree at this face, and the error implies the mesh is moving". i do not understand why, is my wall velocity setting applied to the girds near the wall rather than the water and air? if so, where should i set the velocity? i'm looking forward to your replies. thanks a million!

August 30, 2013, 00:15		#10
wjy-c New Member Jingyao Wang Join Date: Jun 2013 Posts: 29 Rep Power: 13	Hi, Brunoc. I read a similar 2D-gear pump example in fluent using your way. i do not know much about Fluent, as Ghorrocks mentioned above, is the available in my complicated 3-D gearbox model with several engaged gears. if it works, maybe i should learn Fluent. Thank you!

August 30, 2013, 07:58		#11
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,872 Rep Power: 144	Your error message simply means you made a mistake setting the tangential velocity. It is saying it is not tangential. As I said in my post #8 I do not think the model you propose (modelling the actiual gear teeth) is going to be possible in any CFD code. You might be able to get some code to handle the remeshing and all the other stuff, but there is no way you are going to be able to get the mesh fine enough to resolve the flow features in this model. You are going to have to simplify it.