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

Is there any steady state solution for Gear pump simulation?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 23, 2017, 08:31
Default Is there any steady state solution for Gear pump simulation?
  #1
Senior Member
 
sluzzer
Join Date: Jul 2014
Posts: 127
Rep Power: 4
shivasluzz is on a distinguished road
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?
shivasluzz is offline   Reply With Quote

Old   May 23, 2017, 18:50
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,535
Rep Power: 104
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   May 23, 2017, 20:43
Default
  #3
Senior Member
 
sluzzer
Join Date: Jul 2014
Posts: 127
Rep Power: 4
shivasluzz is on a distinguished road
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
shivasluzz is offline   Reply With Quote

Old   May 24, 2017, 01:49
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,535
Rep Power: 104
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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?
ghorrocks is offline   Reply With Quote

Old   May 25, 2017, 00:55
Default
  #5
Senior Member
 
sluzzer
Join Date: Jul 2014
Posts: 127
Rep Power: 4
shivasluzz is on a distinguished road
IMG_9944.JPGIMG_9942.JPGIMG_9940.JPGIMG_9941.JPGIMG_9943.JPGIMG_9947.JPG
shivasluzz is offline   Reply With Quote

Old   May 25, 2017, 00:57
Default
  #6
Senior Member
 
sluzzer
Join Date: Jul 2014
Posts: 127
Rep Power: 4
shivasluzz is on a distinguished road
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 is offline   Reply With Quote

Old   May 25, 2017, 01:01
Default
  #7
Senior Member
 
sluzzer
Join Date: Jul 2014
Posts: 127
Rep Power: 4
shivasluzz is on a distinguished road
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
shivasluzz is offline   Reply With Quote

Old   May 25, 2017, 07:18
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,535
Rep Power: 104
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   May 25, 2017, 08:31
Default
  #9
Senior Member
 
sluzzer
Join Date: Jul 2014
Posts: 127
Rep Power: 4
shivasluzz is on a distinguished road
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
shivasluzz is offline   Reply With Quote

Old   May 25, 2017, 20:49
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,535
Rep Power: 104
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   May 28, 2017, 03:46
Default
  #11
Senior Member
 
sluzzer
Join Date: Jul 2014
Posts: 127
Rep Power: 4
shivasluzz is on a distinguished road
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
shivasluzz is offline   Reply With Quote

Old   May 28, 2017, 19:14
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,535
Rep Power: 104
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   May 31, 2017, 09:49
Default
  #13
Senior Member
 
sluzzer
Join Date: Jul 2014
Posts: 127
Rep Power: 4
shivasluzz is on a distinguished road
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
shivasluzz is offline   Reply With Quote

Reply

Thread Tools
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
error message cuteapathy CFX 14 March 20, 2012 07:45
mass flow in is not equal to mass flow out saii CFX 2 September 18, 2009 08:07
initialize flow field with steady state solution holg FLUENT 0 July 13, 2009 17:10
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 14:37


All times are GMT -4. The time now is 06:57.