CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FloEFD, FloWorks & FloTHERM

Problem rose from centrifugal impeller

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

Like Tree2Likes
  • 1 Post By Boris_M
  • 1 Post By kimmj

Reply
 
LinkBack Thread Tools Display Modes
Old   January 9, 2012, 22:06
Default Problem rose from centrifugal impeller
  #1
New Member
 
Tim Shute
Join Date: Jan 2012
Posts: 9
Rep Power: 6
tim_shute is on a distinguished road
Hi everyone
I am currently working on a flow simulation of vacuum cleaner,consisting of cover, centrifugal impeller, diffuser and a motor. The path of gasflow is from the inlet of cover—impeller(revolution:30,000rpm)—diffuser—moto r inlet—components in the motor needs to cool down—motor outlet. The tunnel between impeller and diffuser is rather narrow (about 0.2 in).

The BCs are given based on experiment test as:
Inlet: volume flow and environment pressure (90614)
Motor outlet): environment pressure (1atm)
Global rotation (both impeller and rotor): 30,000 RPM
Other parts are stator.

Improve local meshing of small solid feature and narrow tunnel. The goals are quite similar to e one in the tutorial.

Here comes to the questions:
During it is iterated, Two warnings rose up:
1. a vortex happen at the pressure openings;
2. supersonic flow blah blah dv/V=0.71541; Please turn on the High Mach Number.
I tried to get a cut view of the rough result first so as to check out where the shoe pinches but it failed.

As a result, I turned on High Mach Number Option somehow neither global rotation nor local rotation can be selected. Under High Mach Number option, I replaced global/local rotation with rotating wall based on Textile Machine Example, although I knew they are not the same thing, I got no choice and it was worth a long shot. Unfortunetely, another warning came up reminding me it is a subsonic situation, turn off high mach number option blah blah. It made me confused and freaked out.

Now, I am going to disable the impeller component and replace it with a fluid domain with pre-defined initial condition (tangential velocity: 30,000rpmm) . Can anyone get me out of the confusion, or give me any advice/comment on my process? Many THX in advance.

Tim
tim_shute is offline   Reply With Quote

Old   January 17, 2012, 04:54
Default
  #2
Senior Member
 
Boris Marovic
Join Date: Jul 2009
Posts: 464
Rep Power: 15
Boris_M will become famous soon enough
Hi Tim,
the initial model setup sounded good for me. Usually issues with hich mach number are either too few cells in an important flow channel or somewhere a single fraction of a cell getting very high velocities which is continuously increasing until solver crashes.
Either you stop the solver or use the r_abnorm.fld if the solver has already crashed and look for the responsible cell by using a cut plot and global min/max features.
The latter feature shows you according to the parameter where its min (blue) and max (red) value is as a small sphere, now place the cut plot that it's cutting this sphere and display the velocity as not interpolated and with mesh. Now you should see a small fraction of a cell causing this high velocity as everything around it is rapidly going into blue color and only this cell is red. You can get rid of this with either a finer mesh if your mesh is too coarse or by moving the mesh slightly. To move the mesh you can go into the initial mesh settings and simply add one cell in one of the directions to move it either further into the fluid or into the solid. Then try it again, usually this gets rid of the problem.
It can happen occasionally if the cell is at the wrong time at a wrong place :-)

Regards,
Boris
tim_shute likes this.
Boris_M is offline   Reply With Quote

Old   January 24, 2012, 23:17
Default
  #3
New Member
 
M_Jin/Kim
Join Date: Jan 2012
Location: Seoul, ROK
Posts: 11
Rep Power: 6
kimmj is on a distinguished road
Quote:
Originally Posted by tim_shute View Post
Hi everyone
I am currently working on a flow simulation of vacuum cleaner,consisting of cover, centrifugal impeller, diffuser and a motor. The path of gasflow is from the inlet of cover—impeller(revolution:30,000rpm)—diffuser—moto r inlet—components in the motor needs to cool down—motor outlet. The tunnel between impeller and diffuser is rather narrow (about 0.2 in).

The BCs are given based on experiment test as:
Inlet: volume flow and environment pressure (90614)
Motor outlet): environment pressure (1atm)
Global rotation (both impeller and rotor): 30,000 RPM
Other parts are stator.

Improve local meshing of small solid feature and narrow tunnel. The goals are quite similar to e one in the tutorial.

Here comes to the questions:
During it is iterated, Two warnings rose up:
1. a vortex happen at the pressure openings;
2. supersonic flow blah blah dv/V=0.71541; Please turn on the High Mach Number.
I tried to get a cut view of the rough result first so as to check out where the shoe pinches but it failed.

As a result, I turned on High Mach Number Option somehow neither global rotation nor local rotation can be selected. Under High Mach Number option, I replaced global/local rotation with rotating wall based on Textile Machine Example, although I knew they are not the same thing, I got no choice and it was worth a long shot. Unfortunetely, another warning came up reminding me it is a subsonic situation, turn off high mach number option blah blah. It made me confused and freaked out.

Now, I am going to disable the impeller component and replace it with a fluid domain with pre-defined initial condition (tangential velocity: 30,000rpmm) . Can anyone get me out of the confusion, or give me any advice/comment on my process? Many THX in advance.

Tim

Hi,,
I think mesh problem is right, too..

"1. a vortex happen at the pressure openings;" is just extend your inlet or outlet locetion. - I mean make fully developed flow -

"2. supersonic flow blah blah dv/V=0.71541; Please turn on the High Mach Number." check your model and mesh is right.
If your setting is right, many cases disappear that message without high Mach option.
Between rotating region boundary and immovable bodies, there should be mode then 2~3cells..
tim_shute likes this.
kimmj is offline   Reply With Quote

Old   January 27, 2012, 22:46
Default
  #4
New Member
 
Tim Shute
Join Date: Jan 2012
Posts: 9
Rep Power: 6
tim_shute is on a distinguished road
Hi Boris:
I am sincerely grateful for your detailed description of trouble-shooting process, including providing meshing preference and diagnostics. I'll try it later. And "It can happen occasionally if the cell is at the wrong time at a wrong place" is really thought-provoking but I am not sure if "at the wrong time" is related to the trainsient term in the governing equations. In other word, the timing of mesh is irrelevant to the solutions of steady-state problem?

Regards
Tim
tim_shute is offline   Reply With Quote

Old   January 27, 2012, 22:54
Default
  #5
New Member
 
Tim Shute
Join Date: Jan 2012
Posts: 9
Rep Power: 6
tim_shute is on a distinguished road
Quote:
Originally Posted by kimmj View Post
Hi,,
I think mesh problem is right, too..

"1. a vortex happen at the pressure openings;" is just extend your inlet or outlet locetion. - I mean make fully developed flow -

"2. supersonic flow blah blah dv/V=0.71541; Please turn on the High Mach Number." check your model and mesh is right.
If your setting is right, many cases disappear that message without high Mach option.
Between rotating region boundary and immovable bodies, there should be mode then 2~3cells..
Hi, M_Jin:
THX for your advice of "more than 2~3 cells". I'll try it. Just feeling the orthogonal mesh in adaptive meshing is kinda inconvenient.
tim_shute is offline   Reply With Quote

Old   January 28, 2012, 06:04
Default
  #6
Senior Member
 
Boris Marovic
Join Date: Jul 2009
Posts: 464
Rep Power: 15
Boris_M will become famous soon enough
Hi Tim,
no of course the time you meshed the model is irrelevant, I just used this phrase. It's just about the size and position of this cell.
Boris_M is offline   Reply With Quote

Old   January 31, 2012, 21:06
Default
  #7
New Member
 
Tim Shute
Join Date: Jan 2012
Posts: 9
Rep Power: 6
tim_shute is on a distinguished road
Right, I got you.
tim_shute 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
Can I solve this problem by Fluent? Kai_kc FLUENT 1 October 27, 2010 05:29
convergence problem in the turbomachinery problem. u k jha CFX 1 September 7, 2010 18:41
centrifugal casting problem therockyy FLOW-3D 3 August 22, 2010 16:41
Adiabatic and Rotating wall (Convection problem) ParodDav CFX 5 April 29, 2007 19:13
boundary condition impeller centrifugal pump mino2006 FLUENT 2 December 28, 2006 19:07


All times are GMT -4. The time now is 01:16.