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

CFX-Post Query

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 5, 2007, 19:06
Default CFX-Post Query
  #1
Dip
Guest
 
Posts: n/a
Small question A report of centrifugal compressor in CFX-Post shows a distribution of "alpha" and "beta" flow angles (in degrees) at leading/trailing edges vs. Span Normalized.

How are "alpha" and "beta" flow angles defined? (Not refering to any blade angles here).

Thank you.

  Reply With Quote

Old   September 6, 2007, 11:32
Default Re: CFX-Post Query
  #2
Dothan
Guest
 
Posts: n/a
Hi alpha and beta are angles between absolute velocity vector (alpha) or relative velocity vector (beta) with the axial direction (for inlet) or with the radial direction (outlet). The sign(+ or -) of angle depend where cfx put the zero of coordinate system, but I don't think this is a problem. by the way, if your question is about signs, I think cfx consider negative angles that open wide from axial/radial direction to right (looking the impeller from the inlet), and vice versa.

Regards
  Reply With Quote

Old   September 7, 2007, 09:02
Default Re: CFX-Post Query
  #3
sravani
Guest
 
Posts: n/a
Hi i am facing problem in pasing dimensionless variables.how to pass dimensionless variables during the creation of boundary conditions?
  Reply With Quote

Old   September 7, 2007, 13:58
Default Re: CFX-Post Query
  #4
d
Guest
 
Posts: n/a
Dothan thanks !

Did you get response/answer to why can you use only In Pressure - Out Pressure as boundary conditions? I have the same problem in my centrifugal compressor.
  Reply With Quote

Old   September 11, 2007, 07:05
Default Re: CFX-Post Query
  #5
Dothan
Guest
 
Posts: n/a
quoteothan thanks !

I finded this forum because I was beating my head into the wall, and if I can help someone else I'm very happy. I know how feel like when someone have a CFD problem...but this is the soul of forum.

OT: 4 days far from this forum and when I come back what I find? What are these topic about Cigarette???? Someone stop that retarded,please.

Anyway, my compressor model converge only with inlet/outlet Pressure BCs, and with mass flow rate @outlet or @inlet the mach number literally explodes. The tutorial 23 of CFX is a low pressure compressor, and converge very well with outlet mass flow rate...we can add a new Murphy's Law: tutorials always work, but all your identical applications won't.

besides self-irony, there must be a reason. What are the differences between my and CFX impeller? My impeller has a main blade and a splitter blade, runs faster and it has a greater pressure ratio. So it is problably that the complicated flow field causes boundary layer separation that don't help the convergence. furthermore, I think Mach number explodes because if I force the mass flow rate@outlet, and inside the impeller happens what I said before, during the initial 20 iteration CFX rises the velocity@outlet to keep the mass flow rate@outlet BC...and diverge. Mayebe, if we try to start te solutor with a lower mass flow rate@outlet and increase this value only when the solution reachs convergence,step by step ...

but CFX suffers the starts or it implement some trick for initial transitory?

another thing: Computed value of CFX-post are very unreliable. I mean, Polytropic efficiency for example changes value by moving the outlet surface. 5mm of variation produces a change in Pol-Eff from 90% to 85%. I'm not looking for the actual value, clear, but for a value that can be confronted with another impeller, generally with different mesh... discouraging.

Regards

  Reply With Quote

Old   September 11, 2007, 21:18
Default Re: CFX-Post Query
  #6
Dip
Guest
 
Posts: n/a
Dothan, I believe you must have done it already, but I would calculate the isentropic and polytropic efficiency numbers as seen both from plots and well as the report. Mine makes sense for the first run, kind of, but never did I vary the outlet. I have to see. But,can't resolve the b.c issue yet. They say Press-Mass flow b.c's are more robust than Press-Press.
  Reply With Quote

Old   September 12, 2007, 10:10
Default Re: CFX-Post Query
  #7
CycLone
Guest
 
Posts: n/a
Hi Dothan,

I assume you have a total pressure specified at the inlet, right?

The solver is probably blowing up because the flow is initially choked and you are trying to pull more mass through than the choked condition allows. Near choke it is best to specify a pressure outlet (with a total pressure inlet). Near stall you are better off specifying a mass flow outlet. These issues are discussed in the turbomachinery best practices guide in the CFX documentation.

With regards to efficiency, state point queries, which are needed to calculate polytropic and isentropic efficiency when the Cp is variable, are not yet available within Post. If you are comparing impellers, just make sure you place the inlets in the same location. You can then calculate the efficency at any location in the domain, I suggest creating a turbo surface aligned with the blade trailing edge (there is a nice feature that can automatically do this for you).

The outlet location will only matter in terms of the boundary condition you are applying. Moving it up may put it too close to the impeller, for instance, and changing the static pressure at different radial locations will also change the operating point, because the vaneless space beyond the blade is a diffuser.

-CycLone
  Reply With Quote

Old   September 13, 2007, 10:29
Default Re: CFX-Post Query
  #8
Dothan
Guest
 
Posts: n/a
Hi Cyclone, I agree with you, I had read best pratices in CFX. I'll check again. Last week I did this test: with the same model mesh, I have run 6 cases, changing the outlet pressure.so I have built 2 charts, polytropic vs mass flow rate and pressure ratio vs mass flow rate. After that, I have moved the outlet surface (not the last, but the surface between TE and Outlet) and I have run the new model. clear, moving close or far from TE,change the operating point, but this point must be near the previous charts. And this don't happen.

anyhow I'm studing your advice, and I'll create a new surface for comparing different impellers. If I align a surface with the TE, Isn't it too close to the vane wakes?

Problably, I fail when I try to undestand how CFX calculate the summary values, like pol. efficinecy. Any your observation will help me. tnx

Dothan

  Reply With Quote

Old   September 13, 2007, 10:37
Default Re: CFX-Post Query
  #9
Dothan
Guest
 
Posts: n/a
Hi Dip,

if I understand you want plot Pol.Efficiency vs mass flow rate, or pressure ratio vs mass flow rate ecc, i.e. plot the characteristic charts of your compressor. well, I have done this by 6-7 different cases, changing the outlet pressure, keeping the impeller rpm costant. I plot point by point with Openoffice Calc, or if you like you can do this with Excel.

Dothan
  Reply With Quote

Old   October 9, 2007, 08:12
Default Re: CFX-Post Query
  #10
madhao
Guest
 
Posts: n/a
Hi,i dont know its correct or wrong but ucan try ... create new material in material library then try to give the boundary conditions.
  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
CFX post legend modification mactech001 CFX 3 December 25, 2011 23:12
How to get reynolds stress values in POST CFX syler3321 CFX 5 March 17, 2011 01:23
CFX post - graph kmgraju CFX 0 July 22, 2010 11:59
Chart Generation in CFX Post Vadim Baines-Jones CFX 2 August 28, 2007 09:14
Tecplot for CFX post processing pantangi goud CFX 2 August 24, 2005 16:42


All times are GMT -4. The time now is 13:21.