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

Centrifugal compressor mass flow error

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 22, 2009, 17:33
Unhappy Centrifugal compressor mass flow error
  #1
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Location: Munich
Posts: 368
Rep Power: 17
Attesz is an unknown quantity at this point
Hi all,
I'm modelling a micro gas turbine engine(for RC airplanes). It has a centrifugal compressor wheel, a diffuser, combustion chamber, axial turbine and a nozzle. The compressor pressure ratio is 3.4. I want to reach it from 2.2 step by step, to get the compressor characteristic. I'm modeling the compressor wheel and the diffuser. Inlet: air ideal gas 300K 1bar opening pressure, outlet: far from the outlet of the diffuser, opening, 2.2bar opening pressure and dirn, 350K. Rotation speed of the impeller is 120000RPM. At this rotation speed, the compressor-diffuser has 3.4 pressure ratio. My simulation converges at 2.2 pressure ratio, but at higher pressure ratios not. I' think, in the simulation the 3.4p.ratio will be above the surge line, but it's not the reality. I've checked the geometry, made a good quality mesh. I'm using SST turbulence model.

Any idea? It can be caused by the solver settings(I dont think)?

Thanks!

Best regards,
Attila
Attesz is offline   Reply With Quote

Old   September 22, 2009, 18:22
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,828
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
http://www.cfd-online.com/Wiki/Ansys...gence_criteria

You will have to give more details before we can help you.
ghorrocks is offline   Reply With Quote

Old   September 23, 2009, 04:42
Default
  #3
New Member
 
Join Date: Sep 2009
Posts: 1
Rep Power: 0
Ally is on a distinguished road
To begin with solver settings are unlikely to be the source of your problem - seeing as the model converges at lower PR this is more likely to be an issue with the physical set up. Do the mass flow v PR predictions line up with the map at lower pressure ratios?

Although you say your boundaries are placed well upstream and downstream, particularly at diffuser outlet these need to be FAR downstream (particularly important at high PR) - you should really be able to use an outlet boundary. Unless handled correctly this wil give you unrealistic PR vs mass flow results and shift your surge line.
Ally is offline   Reply With Quote

Old   October 24, 2009, 15:30
Default
  #4
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Location: Munich
Posts: 368
Rep Power: 17
Attesz is an unknown quantity at this point
Thank you!

I've modified the boundary conditions, try a lot of modifications in geometry, without results.

But I've found some information about simulation of compressors in this document:

http://www.ansys.com/events/proceedings/2006/PAPERS/252.pdf

At page 7 we can read:

"The initial conditions within the compressor are estimated automatically by CFX based on the boundary
conditions. However when the compressor was simulated at operating conditions, the numerical solution
was found to diverge. Therefore, a rotational velocity ramping function was used at start up.
The impeller rotational velocity at start up was set such that the initial velocity is about 25% of the desired
velocity and it was increased to the desired velocity over the next 75 iterations. This allows the flow to
develop at slower rotational velocities such that when the desired rotational velocity is reached, the flow
properties within the compressor are much closer to the desired steady-state solution.
This technique
generates improved estimates for the initial data, which was necessary because of the aggressive time steps
(1/rotational velocity) used in order to quickly reach convergence. As a comparison, this time step is over
10 times larger than the one automatically estimated by CFX based on mesh dimensions."

My compressor velocity speed is high (120000RPM), and I started the simulation at this speed. From the document I think, it can be also a possible problem. I note, my simulation at 120000 RPM and PR3.0-PR3.4 doesn't converge!

Could someone help, how to use this "ramping function" in my simulation? I can't program in CEL, but I would like to

Thank you very much!
Attesz

Last edited by Attesz; October 25, 2009 at 03:37.
Attesz is offline   Reply With Quote

Old   October 25, 2009, 05:15
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,828
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
If you want to write a CEL expression use the step or if functions (If is only available in V12). Have a look in the CEL Expression reference guide for how to write these functions.

Alternately you can use a 1D interpolation function to ramp it up.
ghorrocks is offline   Reply With Quote

Old   October 25, 2009, 06:26
Default
  #6
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Location: Munich
Posts: 368
Rep Power: 17
Attesz is an unknown quantity at this point
I've made it by using the interpolation function and the "aitern" expression, it' works.

Thank you!

Best regards,
Attesz
Attesz is offline   Reply With Quote

Old   May 19, 2011, 16:25
Smile go to http://parsturbine.com
  #7
New Member
 
Jamshid
Join Date: May 2011
Posts: 1
Rep Power: 0
Jamshid is on a distinguished road
Quote:
Originally Posted by Attesz View Post
Hi all,
I'm modelling a micro gas turbine engine(for RC airplanes). It has a centrifugal compressor wheel, a diffuser, combustion chamber, axial turbine and a nozzle. The compressor pressure ratio is 3.4. I want to reach it from 2.2 step by step, to get the compressor characteristic. I'm modeling the compressor wheel and the diffuser. Inlet: air ideal gas 300K 1bar opening pressure, outlet: far from the outlet of the diffuser, opening, 2.2bar opening pressure and dirn, 350K. Rotation speed of the impeller is 120000RPM. At this rotation speed, the compressor-diffuser has 3.4 pressure ratio. My simulation converges at 2.2 pressure ratio, but at higher pressure ratios not. I' think, in the simulation the 3.4p.ratio will be above the surge line, but it's not the reality. I've checked the geometry, made a good quality mesh. I'm using SST turbulence model.

Any idea? It can be caused by the solver settings(I dont think)?

Thanks!

Best regards,
Attila
go to http://parsturbine.com
Jamshid is offline   Reply With Quote

Old   May 22, 2011, 07:01
Default
  #8
Far
Senior Member
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,557
Blog Entries: 6
Rep Power: 54
Far has a spectacular aura aboutFar has a spectacular aura about
Send a message via Skype™ to Far
Quote:
Originally Posted by Jamshid View Post
I am afraid that the thread is more than one year old!
Far is offline   Reply With Quote

Old   May 25, 2011, 04:24
Default
  #9
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Location: Munich
Posts: 368
Rep Power: 17
Attesz is an unknown quantity at this point
Hi Jamshid,

Your website contains few information about your turbine, if you could, please share with us (or only with me ) more information. I'm very interested in your developments because in a few months I will start my RC turbine company.

Regards,
Attesz
Attesz is offline   Reply With Quote

Old   May 25, 2012, 05:29
Default
  #10
Member
 
jk
Join Date: Jun 2009
Posts: 64
Rep Power: 17
jyothishkumar is on a distinguished road
Hi Attesz,

Currently I am working in unsteady flow analysis of centrifugal compressor (of turbochargers).* I have started my unsteady analysis with a converged steady state results.* I am using the moving mesh method to include the rotation.* When the impeller makes about 270 degrees of rotation, the mass flow starts decreasing at the volute exit.* It continuously decreases further to a very small value.* I have monitored the mass flow for about 6 revolution of the wheel.* My time step size is around 1deg. and the speed of compressor is 6702.06rad/s (64000 rpm).* Also I have taken a point away from surge (i.e. within the operating range). Is this physically possible.* whether I should wait and see for some more rotations.*
jyothishkumar is offline   Reply With Quote

Old   May 25, 2012, 05:30
Default
  #11
Member
 
jk
Join Date: Jun 2009
Posts: 64
Rep Power: 17
jyothishkumar is on a distinguished road
Hi Attesz,

Currently I am working in unsteady flow analysis of centrifugal compressor (of turbochargers).* I have started my unsteady analysis with a converged steady state results.* I am using the moving mesh method to include the rotation.* When the impeller makes about 270 degrees of rotation, the mass flow starts decreasing at the volute exit.* It continuously decreases further to a very small value.* I have monitored the mass flow for about 6 revolution of the wheel.* My time step size is around 1deg. and the speed of compressor is 6702.06rad/s (64000 rpm).* Also I have taken a point away from surge (i.e. within the operating range). Is this physically possible.* whether I should wait and see for some more rotations.*
jyothishkumar is offline   Reply With Quote

Old   May 25, 2012, 14:41
Default
  #12
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Location: Munich
Posts: 368
Rep Power: 17
Attesz is an unknown quantity at this point
Hi, sounds like you have reached the surge. Take into account that RANS simulations usually underpredict the performance curve, but URANS are closer to the real operation, meaning that you have higher pressure ratio/lower mass flow that is you are closer to surge. If you know your surge pressure ratio keep bigger distance, if not decrease the pressure ratio or increase the massflow whatever you use as BC. Also look at the results if they are correct or not. Are you using outlet or opening at the exit of the volute? Give more details,

Cheers

Quote:
Originally Posted by jyothishkumar View Post
Hi Attesz,

Currently I am working in unsteady flow analysis of centrifugal compressor (of turbochargers).* I have started my unsteady analysis with a converged steady state results.* I am using the moving mesh method to include the rotation.* When the impeller makes about 270 degrees of rotation, the mass flow starts decreasing at the volute exit.* It continuously decreases further to a very small value.* I have monitored the mass flow for about 6 revolution of the wheel.* My time step size is around 1deg. and the speed of compressor is 6702.06rad/s (64000 rpm).* Also I have taken a point away from surge (i.e. within the operating range). Is this physically possible.* whether I should wait and see for some more rotations.*
__________________
I am doing CFD Consulting Services.
Ich biete CFD Strömungssimulationen an.
Attesz is offline   Reply With Quote

Old   May 26, 2012, 09:24
Default
  #13
Member
 
jk
Join Date: Jun 2009
Posts: 64
Rep Power: 17
jyothishkumar is on a distinguished road
Hi,

Thanks for your reply. Actually i am using mass flow inlet and static pressure outlet bc. But I have taken a point away from the surge (taken from the map). If this is the case how come surge will happen. Any ideas
jyothishkumar is offline   Reply With Quote

Old   May 26, 2012, 09:25
Default
  #14
Member
 
jk
Join Date: Jun 2009
Posts: 64
Rep Power: 17
jyothishkumar is on a distinguished road
Hi,

Thanks for your reply. Actually i am using mass flow inlet and static pressure outlet bc. But I have taken a point away from the surge (taken from the map). If this is the case how come surge will happen. Any ideas
jyothishkumar is offline   Reply With Quote

Old   May 27, 2012, 05:58
Default
  #15
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Location: Munich
Posts: 368
Rep Power: 17
Attesz is an unknown quantity at this point
Did you measure the parameters of the perf. map or just calculated? If you trust in your data, then check the mesh maybe. What it the PR of surge and your PR?


Quote:
Originally Posted by jyothishkumar View Post
Hi,

Thanks for your reply. Actually i am using mass flow inlet and static pressure outlet bc. But I have taken a point away from the surge (taken from the map). If this is the case how come surge will happen. Any ideas
__________________
I am doing CFD Consulting Services.
Ich biete CFD Strömungssimulationen an.
Attesz is offline   Reply With Quote

Old   May 27, 2012, 06:51
Default
  #16
Member
 
jk
Join Date: Jun 2009
Posts: 64
Rep Power: 17
jyothishkumar is on a distinguished road
Hi attesz,

I have taken the value from the experimental datas. Pressure ratio of surge is around 1.62 and mass flow is around 0.104kg/s. Whereas my mass flow is around 0.27 kg/s and PR is 1.5
jyothishkumar is offline   Reply With Quote

Old   May 27, 2012, 06:51
Default
  #17
Member
 
jk
Join Date: Jun 2009
Posts: 64
Rep Power: 17
jyothishkumar is on a distinguished road
Hi attesz,

I have taken the value from the experimental datas. Pressure ratio of surge is around 1.62 and mass flow is around 0.104kg/s. Whereas my mass flow is around 0.27 kg/s and PR is 1.5
jyothishkumar is offline   Reply With Quote

Old   May 27, 2012, 10:17
Default
  #18
Member
 
jk
Join Date: Jun 2009
Posts: 64
Rep Power: 17
jyothishkumar is on a distinguished road
Hi,

I am getting the following warning for some time step.

Warning: Wall distance limited to 1e-06 in 2 cells in region 02_wheel
Warning: Wall distance limited to 1e-06 in 2 cells in region 03_shroud
corrections limited in 9 cells in region 02_wheel

Also the same is not coming if the mesh is very coarse. In case if it is a mesh problem i got my steady case without having any convergence issue with the same mesh. Your comment is appreciable
jyothishkumar is offline   Reply With Quote

Old   May 27, 2012, 10:17
Default
  #19
Member
 
jk
Join Date: Jun 2009
Posts: 64
Rep Power: 17
jyothishkumar is on a distinguished road
Hi attesz,

I am getting the following warning for some time step.

Warning: Wall distance limited to 1e-06 in 2 cells in region 02_wheel
Warning: Wall distance limited to 1e-06 in 2 cells in region 03_shroud
corrections limited in 9 cells in region 02_wheel

Also the same is not coming if the mesh is very coarse. In case if it is a mesh problem i got my steady case without having any convergence issue with the same mesh. Your comment is appreciable
jyothishkumar is offline   Reply With Quote

Reply

Tags
centrifugal, compressor, mass flow, pressure ratio

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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Integrated conjugate heat transfer solver in OpenFOAM hjasak OpenFOAM Running, Solving & CFD 172 April 13, 2023 00:42
[Netgen] Installation of Netgen in SuSE Linux 92 edvardsenpriv OpenFOAM Meshing & Mesh Conversion 23 January 16, 2009 06:12
OpenFoam 14 installation problem gfcoppola OpenFOAM Installation 20 November 2, 2007 13:38
Installation problem with GCC Norma McKee (Mckee) OpenFOAM Installation 10 March 4, 2007 07:09
Problems of Duns Codes! Martin J Main CFD Forum 8 August 14, 2003 23:19


All times are GMT -4. The time now is 16:40.