Is there any steady state solution for Gear pump simulation?

shivasluzz · May 23, 2017, 09:31

Most of the Gear Pump simulation in technical papers and in Ansys tutorials was done for Transient condition. Is it possible to get steady state solution for Gear Pump?

ghorrocks · May 23, 2017, 19:50

Why don't you try it and work it out? I am not 100% sure whether immersed solids works in steady state, so that is what I would do to confirm.

shivasluzz · May 23, 2017, 21:43

I tried.. it's not converging.. after some 20 iterations, it fails with fatal overflow error.. Mesh quality and resolution is very good (full structured mesh and quality is good as written by solver statistics). Boundary layers are resolved as per y+ value. Initialisation is good. Double precision is used for solving. Still it fails! So I doubt whether there is steady state solution or not?

Gear Pump outlet pressure is pulsating in nature. So can we say there is no steady state solution for Gear Pump?

Is there anything like Immersed solid simulation doesn't support steady state simulation?

Sent from my iPhone using CFD Online Forum mobile app

ghorrocks · May 24, 2017, 02:49

A steady state run of a gear pump would have the rotors stationary, so the flow would be from leakage around the rotors. Obviously this is likely to be small, but in a well resolved model it should be possible.

Note the immersed solid approach works by putting body forces on the elements covered by the body. This means that in the fine gap between the rotor and the wall it may be difficult to get any mesh which is not covered by rotor, and this means you will get no flow (and probably convergence difficulties). Have you got enough mesh in the gap so there can be a flow?

shivasluzz · May 25, 2017, 01:55

IMG_9944.JPG IMG_9942.JPG IMG_9940.JPG IMG_9941.JPG IMG_9943.JPG IMG_9947.JPG

shivasluzz · May 25, 2017, 01:57

Here I attached the mesh pics and velocity contour at the final iteration before it failed due to fatal linear solver error! Sufficient care is taken to resolve the clearances.
So my doubt is whether the failure is due to Transient nature of the flow or not?
How to confirm this?

Sent from my iPhone using CFD Online Forum mobile app

shivasluzz · May 25, 2017, 02:01

One thing I observed is Immersed solid is able to resolve vortex and fine pressure distribution! However many technical paper claims that Immersed solid is unable to resolve suction and tip vortex!
Am working on it to quantify the accuracy of Immersed solid methods.
Any input regarding this is appreciated
Thanks

Sent from my iPhone using CFD Online Forum mobile app

ghorrocks · May 25, 2017, 08:18

The velocity plot doesn't mean much because the simulation diverged so the results are meaningless. More useful is a plot of when the numerical instability is first seen, because that can tell you where the problem area is.

The CFX documentation has several recommendations on convergence with immersed solids. Have you read it, and tried the suggestions?

Immersed solid approach can theoretically resolve any Navier Stokes flow, so you it can model vortex and instabilities and everything else. In fact the open source CFD code gerris does not use wall boundaries for internal features at all, it always uses a similar approach. So some CFD codes only use this approach to model walls.

But it uses mesh less efficiently than a body fitted grid, meaning more mesh to get the same resolution. But when a body fitted grid is not practical (eg gear pumps) then immersed solids is great.

shivasluzz · May 25, 2017, 09:31

Thanks for the explanation ghorrocks..
Do you mean the rms error convergence plot?

Yes I am trying all those recommendations given in CFX documentation. By now my only doubt is should I try with Steady state simulation or should I try Transient simulation because Steady state simulation is not converging?

Sent from my iPhone using CFD Online Forum mobile app

ghorrocks · May 25, 2017, 21:49

The steady state simulation should converge, providing there are no flow instabilities.

View either the velocity field or the RMS residuals when the simulation first shows signs of numerical instability.

shivasluzz · May 28, 2017, 04:46

Thanks for the suggestion ghorrocks.
The simulation is converged after reducing the Momentum source scaling factor, as given in the CFX documentation.
The default value of Momentum source scaling factor is 10.
Why it should be 10? Why we need to scale the Momentum source? Ideally it should be 1 rite?
The simulation is converging with ease when we use Momentum source scaling factor less than 1. All other initialization method like running first with Laminar condition, ramped speed increase, ramped outlet pressure increase has failed.
Now I am facing the 100% artificial wall problem at both end. Initially i thought, the length of inlet and outlet may be insufficient or the direction of rotation has some problem. But even after ensuring these two factors, i persistently facing artificial wall problem. However the simulation has converged. But when I check the mass flow rate at the outlet, it shows 0. Any suggestion?
Also the CFX documentation says that the initialization and stability can be used by using inside() function.
I created two Coordinate reference frame for the 2 gears. Now I want to specify the angular velocity of the fluid inside the gears using inside function with respect to the co-ordinate reference frame of the gears. Since there are 2 gears which rotates in opposite direction with each other, I need to create expression with reference to 2 co-ordinate frame. Any suggestion on how to do this?
for example,
to give initialization, for theta direction, in cyclindrical coordinate system, for the fluid fluid, i like to use
(inside()@Driven gear * angular velocity w.r.t Driven gear coordinate frame) + (inside()@Driving gear * angular velocity w.r.t Driving gear coordinate frame)
Any idea?
Thanks

ghorrocks · May 28, 2017, 20:14

Quote:

Why it should be 10? Why we need to scale the Momentum source? Ideally it should be 1 rite?

This is all discussed in the documentation. Have you read it?

Quote:

Now I am facing the 100% artificial wall problem at both end.

Use the post processor to check what the flow field looks like. Check it is behaving as you expected.

shivasluzz · May 31, 2017, 10:49

No I couldn't find why the momentum source scaling factor should be 10.

Yes I checked in the post processor and for some unknown reason flow was not coming out from Fluid volume in which the Immersed gears rotates. I changed the outlet boundary condition from static pressure to mass flow rate and now the artificial wall problem has solved.

Thanks for the suggestions ghorrocks

Sent from my iPhone using CFD Online Forum mobile app

Sanjv9473 · September 7, 2021, 02:48

s there any steady state solution for Gear pump simulation ?

A model for the prediction of the dynamic behaviour of an external gear pump is presented. We took into account the most important phenomena involved in the operation of this kind of machines. Fluid pressure distribution on gears, which is time-varying, is instantaneously computed and included as a resultant external force and torque acting on the gears.

May 23, 2017, 09:31	Is there any steady state solution for Gear pump simulation?	#1
shivasluzz Senior Member sluzzer Join Date: Jul 2014 Posts: 146 Rep Power: 12	Most of the Gear Pump simulation in technical papers and in Ansys tutorials was done for Transient condition. Is it possible to get steady state solution for Gear Pump?

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
mass flow in is not equal to mass flow out	saii	CFX	12	March 19, 2018 06:21
error message	cuteapathy	CFX	14	March 20, 2012 07:45
initialize flow field with steady state solution	holg	FLUENT	0	July 13, 2009 18:10
material property in steady state CHT simulation	NVSD BABU	CFX	3	February 25, 2009 01:58
About the difference between steady and unsteady problems	Lisa	Main CFD Forum	11	July 5, 2000 15:37

May 23, 2017, 19:50		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,852 Rep Power: 144	Why don't you try it and work it out? I am not 100% sure whether immersed solids works in steady state, so that is what I would do to confirm.

May 23, 2017, 21:43		#3
shivasluzz Senior Member sluzzer Join Date: Jul 2014 Posts: 146 Rep Power: 12	I tried.. it's not converging.. after some 20 iterations, it fails with fatal overflow error.. Mesh quality and resolution is very good (full structured mesh and quality is good as written by solver statistics). Boundary layers are resolved as per y+ value. Initialisation is good. Double precision is used for solving. Still it fails! So I doubt whether there is steady state solution or not? Gear Pump outlet pressure is pulsating in nature. So can we say there is no steady state solution for Gear Pump? Is there anything like Immersed solid simulation doesn't support steady state simulation? Sent from my iPhone using CFD Online Forum mobile app

May 24, 2017, 02:49		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,852 Rep Power: 144	A steady state run of a gear pump would have the rotors stationary, so the flow would be from leakage around the rotors. Obviously this is likely to be small, but in a well resolved model it should be possible. Note the immersed solid approach works by putting body forces on the elements covered by the body. This means that in the fine gap between the rotor and the wall it may be difficult to get any mesh which is not covered by rotor, and this means you will get no flow (and probably convergence difficulties). Have you got enough mesh in the gap so there can be a flow?

May 25, 2017, 01:55		#5
shivasluzz Senior Member sluzzer Join Date: Jul 2014 Posts: 146 Rep Power: 12	IMG_9944.JPG IMG_9942.JPG IMG_9940.JPG IMG_9941.JPG IMG_9943.JPG IMG_9947.JPG

May 25, 2017, 01:57		#6
shivasluzz Senior Member sluzzer Join Date: Jul 2014 Posts: 146 Rep Power: 12	Here I attached the mesh pics and velocity contour at the final iteration before it failed due to fatal linear solver error! Sufficient care is taken to resolve the clearances. So my doubt is whether the failure is due to Transient nature of the flow or not? How to confirm this? Sent from my iPhone using CFD Online Forum mobile app

May 25, 2017, 02:01		#7
shivasluzz Senior Member sluzzer Join Date: Jul 2014 Posts: 146 Rep Power: 12	One thing I observed is Immersed solid is able to resolve vortex and fine pressure distribution! However many technical paper claims that Immersed solid is unable to resolve suction and tip vortex! Am working on it to quantify the accuracy of Immersed solid methods. Any input regarding this is appreciated Thanks Sent from my iPhone using CFD Online Forum mobile app

May 25, 2017, 08:18		#8
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,852 Rep Power: 144	The velocity plot doesn't mean much because the simulation diverged so the results are meaningless. More useful is a plot of when the numerical instability is first seen, because that can tell you where the problem area is. The CFX documentation has several recommendations on convergence with immersed solids. Have you read it, and tried the suggestions? Immersed solid approach can theoretically resolve any Navier Stokes flow, so you it can model vortex and instabilities and everything else. In fact the open source CFD code gerris does not use wall boundaries for internal features at all, it always uses a similar approach. So some CFD codes only use this approach to model walls. But it uses mesh less efficiently than a body fitted grid, meaning more mesh to get the same resolution. But when a body fitted grid is not practical (eg gear pumps) then immersed solids is great.

May 25, 2017, 09:31		#9
shivasluzz Senior Member sluzzer Join Date: Jul 2014 Posts: 146 Rep Power: 12	Thanks for the explanation ghorrocks.. Do you mean the rms error convergence plot? Yes I am trying all those recommendations given in CFX documentation. By now my only doubt is should I try with Steady state simulation or should I try Transient simulation because Steady state simulation is not converging? Sent from my iPhone using CFD Online Forum mobile app

May 25, 2017, 21:49		#10
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,852 Rep Power: 144	The steady state simulation should converge, providing there are no flow instabilities. View either the velocity field or the RMS residuals when the simulation first shows signs of numerical instability.

May 28, 2017, 04:46		#11
shivasluzz Senior Member sluzzer Join Date: Jul 2014 Posts: 146 Rep Power: 12	Thanks for the suggestion ghorrocks. The simulation is converged after reducing the Momentum source scaling factor, as given in the CFX documentation. The default value of Momentum source scaling factor is 10. Why it should be 10? Why we need to scale the Momentum source? Ideally it should be 1 rite? The simulation is converging with ease when we use Momentum source scaling factor less than 1. All other initialization method like running first with Laminar condition, ramped speed increase, ramped outlet pressure increase has failed. Now I am facing the 100% artificial wall problem at both end. Initially i thought, the length of inlet and outlet may be insufficient or the direction of rotation has some problem. But even after ensuring these two factors, i persistently facing artificial wall problem. However the simulation has converged. But when I check the mass flow rate at the outlet, it shows 0. Any suggestion? Also the CFX documentation says that the initialization and stability can be used by using inside() function. I created two Coordinate reference frame for the 2 gears. Now I want to specify the angular velocity of the fluid inside the gears using inside function with respect to the co-ordinate reference frame of the gears. Since there are 2 gears which rotates in opposite direction with each other, I need to create expression with reference to 2 co-ordinate frame. Any suggestion on how to do this? for example, to give initialization, for theta direction, in cyclindrical coordinate system, for the fluid fluid, i like to use (inside()@Driven gear * angular velocity w.r.t Driven gear coordinate frame) + (inside()@Driving gear * angular velocity w.r.t Driving gear coordinate frame) Any idea? Thanks

May 31, 2017, 10:49		#13
shivasluzz Senior Member sluzzer Join Date: Jul 2014 Posts: 146 Rep Power: 12	No I couldn't find why the momentum source scaling factor should be 10. Yes I checked in the post processor and for some unknown reason flow was not coming out from Fluid volume in which the Immersed gears rotates. I changed the outlet boundary condition from static pressure to mass flow rate and now the artificial wall problem has solved. Thanks for the suggestions ghorrocks Sent from my iPhone using CFD Online Forum mobile app

September 7, 2021, 02:48		#14
Sanjv9473 New Member Sanjeev kumar Join Date: Sep 2021 Location: India Posts: 3 Rep Power: 5	s there any steady state solution for Gear pump simulation ? A model for the prediction of the dynamic behaviour of an external gear pump is presented. We took into account the most important phenomena involved in the operation of this kind of machines. Fluid pressure distribution on gears, which is time-varying, is instantaneously computed and included as a resultant external force and torque acting on the gears.