
[Sponsors] 
September 22, 2009, 17:33 
Centrifugal compressor mass flow error

#1 
Senior Member
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 9 
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 compressordiffuser 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 

September 22, 2009, 18:22 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,638
Rep Power: 98 
http://www.cfdonline.com/Wiki/Ansys...gence_criteria
You will have to give more details before we can help you. 

September 23, 2009, 04:42 

#3 
New Member
Join Date: Sep 2009
Posts: 1
Rep Power: 0 
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. 

October 24, 2009, 15:30 

#4 
Senior Member
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 9 
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 steadystate 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 PR3.0PR3.4 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 04:37. 

October 25, 2009, 06:15 

#5 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,638
Rep Power: 98 
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. 

October 25, 2009, 07:26 

#6 
Senior Member
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 9 
I've made it by using the interpolation function and the "aitern" expression, it' works.
Thank you! Best regards, Attesz 

May 19, 2011, 16:25 
go to http://parsturbine.com

#7  
New Member
Jamshid
Join Date: May 2011
Posts: 1
Rep Power: 0 
Quote:


May 22, 2011, 07:01 

#8  
Super Moderator

Quote:


May 25, 2011, 04:24 

#9 
Senior Member
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 9 
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 

May 25, 2012, 05:29 

#10 
Member
jk
Join Date: Jun 2009
Posts: 64
Rep Power: 9 
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.* 

May 25, 2012, 05:30 

#11 
Member
jk
Join Date: Jun 2009
Posts: 64
Rep Power: 9 
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.* 

May 25, 2012, 14:41 

#12  
Senior Member
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 9 
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:
__________________
CFD= Cleverly Formatted Data 

May 26, 2012, 09:24 

#13 
Member
jk
Join Date: Jun 2009
Posts: 64
Rep Power: 9 
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 

May 26, 2012, 09:25 

#14 
Member
jk
Join Date: Jun 2009
Posts: 64
Rep Power: 9 
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 

May 27, 2012, 05:58 

#15 
Senior Member
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 9 
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?
__________________
CFD= Cleverly Formatted Data 

May 27, 2012, 06:51 

#16 
Member
jk
Join Date: Jun 2009
Posts: 64
Rep Power: 9 
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 

May 27, 2012, 06:51 

#17 
Member
jk
Join Date: Jun 2009
Posts: 64
Rep Power: 9 
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 

May 27, 2012, 10:17 

#18 
Member
jk
Join Date: Jun 2009
Posts: 64
Rep Power: 9 
Hi,
I am getting the following warning for some time step. Warning: Wall distance limited to 1e06 in 2 cells in region 02_wheel Warning: Wall distance limited to 1e06 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 

May 27, 2012, 10:17 

#19 
Member
jk
Join Date: Jun 2009
Posts: 64
Rep Power: 9 
Hi attesz,
I am getting the following warning for some time step. Warning: Wall distance limited to 1e06 in 2 cells in region 02_wheel Warning: Wall distance limited to 1e06 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 

Tags 
centrifugal, compressor, mass flow, pressure ratio 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Integrated conjugate heat transfer solver in OpenFOAM  hjasak  OpenFOAM Running, Solving & CFD  170  March 2, 2016 05:20 
Installation of Netgen in SuSE Linux 92  edvardsenpriv  Open Source Meshers: Gmsh, Netgen, CGNS, ...  23  January 16, 2009 07:12 
OpenFoam 14 installation problem  gfcoppola  OpenFOAM Installation  20  November 2, 2007 14:38 
Installation problem with GCC  Norma McKee (Mckee)  OpenFOAM Installation  10  March 4, 2007 08:09 
Problems of Duns Codes!  Martin J  Main CFD Forum  8  August 14, 2003 23:19 