# gas turbine simulation setup

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 August 15, 2004, 12:22 gas turbine simulation setup #1 Petr Guest   Posts: n/a Hello folks, I wonder how to setup material properties for flow simulation for gas turbine stage. As I learn from friends, who successfully did it in TASCflow, there are separate options for Cp and Cv values in material properties window. For a while I see that in CFX 5.7 I can select only one of it Cp or Cv. Appreciate Your suggestions and advice in advance. BR Petr

 August 18, 2004, 14:05 Re: gas turbine simulation setup #2 Ian Guest   Posts: n/a CFX uses Cp and molecular weight. Cv and gamma can be derived from these 2 quantities.

 August 18, 2004, 16:27 Re: gas turbine simulation setup #3 Petr Guest   Posts: n/a Thanks Ian. I understand it. My core problem is that I can't duplicate in CFX 5.7 gas turbine stage simulation ( accomplished early in TASCflow 2.11). I get flow rate about 12% higher in CFX than calculated in TASCflow. The results obtained in TASCflow are well correlated with experimental data, so I'd like to believe in its. I found that sole problem is the difference in working fluid density. The settings for fluid in TASCflow were: "Air at STP", Turbulence, Compressible. When I set fluid in CFX 5.7 as "Air at STP", I get the density at inlet 1.284 kg/m^3 (P=830000Pa), despite that "Density depends on pressure" flag was set as YES. When I set fluid in CFX 5.7 as "Air as Ideal Gas", I get the density at inlet 2.55 kg/m^3, while TASCflow shows this value 12% less. Thanks in advance to anyone for any suggestions. Petr

 August 19, 2004, 12:07 Re: gas turbine simulation setup #4 Robin Guest   Posts: n/a Are you using the same grid that was used in TASCflow?

 August 19, 2004, 12:47 Re: gas turbine simulation setup #5 Petr Guest   Posts: n/a Hello Robin, Yes, thanks to CFX guys I can import the very same model as was used for TASCflow early. Today I found other odd thing : I have estimated gas costant (R) on inlet and outlet and obtained odd values 253/225. This values was checked in TASCflow and was OK - 287/287. Working fluid for CFX was Air Real Gas. Does anybody have positive experience of turbine stage simulation in CFX 5.7 ? Thanks Petr

 August 19, 2004, 13:09 Re: gas turbine simulation setup #6 Robin Guest   Posts: n/a Hi Petr, We've had a lot of success with CFX-5.7 for this kind of calculation. Have you discussed this with technical support? -Robin

 August 19, 2004, 13:23 Re: gas turbine simulation setup #7 Robin Guest   Posts: n/a Do you mean Air Ideal Gas?

 August 19, 2004, 14:50 Re: gas turbine simulation setup #8 Petr Guest   Posts: n/a Sorry. Sure it is Air Ideal Gas.

 August 19, 2004, 16:55 Re: gas turbine simulation setup #9 Robin Guest   Posts: n/a Hi Petr, A couple things worth noting here. The "Density depends on pressure" flag in the materials properties only has an effect if you have defined the density as an a function of pressure. If you have not modified the density accordingly, it will have no effect and your density will be constant. Which is what you are seeing. Air at STP is the wrong fluid property to use, in any case, since the flow you are interested in is clearly compressible. You should probably define your own fluid, rather than simply using Air Ideal Gas, since the exhaust from your combustor will not have the same properties. That said, if you are using Air Ideal Gas and the flow is compressible, make sure you select the "Total Energy" option in your Domain set up. Thermal Energy and Isothermal will not include the necessary terms in the energy equation. If you have the same grid, boundary conditions, fluid properties, and your solution is converged, you should get almost exactly the same result with CFX-5 as CFX-TASCflow. The only major numerical difference between the two codes is with the advection scheme. CFX-TASCflow does not have the same higher order schemes as CFX-5, but if you run them both with 1st order upwind, you should get the same results. If you still don't get the same results, I suggest contacting CFX support and sending them your cases. It is most likely a set-up problem, but if it is indeed a numerical issue, they will be interested in resolving it. Best regards, Robin

 August 21, 2004, 15:22 Re: gas turbine simulation setup #10 Petr Guest   Posts: n/a Hi Robin Thanks for explanation. It solve some my doubts. BTW: I TRY TO RUN THE EXAMLE FROM Tutorial 12 Flow in an Axial Rotor/Stator. I don't like BC suggested in Tutorial: total pressure on inlet and MFR on outlet. At my humble experience it often leads to wrong results for tubine stage. I run tutorial "as is" and then switch BC to total pressure on inlet and static pressure on outlet. Regrettably any time I can't get correct R(gas constant) on inlet and outlet. Next week I'll write to CFX support. Thanks and Best Regards Petr

 August 27, 2004, 11:42 Re: gas turbine simulation setup #11 Ian Guest   Posts: n/a Create your own user defined fluid in each. That way you can be sure they are using exactly the same fluid properties. We do this and our results are identical.

 August 28, 2004, 12:38 Re: gas turbine simulation setup #12 Petr Guest   Posts: n/a Thanks Ian, You are very helpful. BTW: couple a weeks before, we came to idea to export from our turbine design tool AxSTREAM to CFX/TASCflow not only geometry ,as we do now, but a fluid tabeles too. Your advice solves any doubts. Petr

 September 1, 2004, 08:19 Problem with tutorial sample #13 Petr Guest   Posts: n/a I try to check problem with samples from CFX tutorials. So I took Tutorial 12 ( Axial stator/rotor) and run it. I run it "as is" - using BC as was difined in tutorial ( pressure on inlet and MFR on outlet) and for other case (total pressure on inlet and static on outlet). Simulation ran smoothly and finished normaly (E-04). Then I try to calculate gas constant on inlet and outlet and obtain different values. How it can be explained ? I'm sure that it is the main reason of problems discussed in this topic. Thanks Petr

 September 1, 2004, 10:18 Re: Problem with tutorial sample #14 Juan Carlos Guest   Posts: n/a I am late in this discussion, but would you mind explaining how you are estimating the gas constant from the CFX-5.7/TASCflow results? With that information, others could run the tutorial and try to reproduce your observations. Thanks Juan Carlos

 September 7, 2004, 15:20 Re: Problem with tutorial sample #15 Petr Guest   Posts: n/a In case of tutorial 12 data was as below : fluid - as defined in tut12- Air Ideal Gas inlet BC - total pressure 400000Pa, temp= 1000K, outlet - static pressure 200000Pa, rotor rotating 523.6 rad/sec. Gas constant was calculated as R = Pressure/ (Temperature * Density) Results for inlet / outlet were: Pressure (stat) = 388631Pa / 200000Pa Temperature (stat) = 993.5K / 884K Density = 1.718 / 1.187 Gas constant(R)= 227.7 / 190 Pressure, Temperature and Density were calculated with Calculator ( function MassFlowAve) ------------------------------------------------------- Thanks Petr

 September 8, 2004, 15:02 Problem solved ! #16 Petr Guest   Posts: n/a Problem with gas constant is solved. I missed reference pressure. When ref. pressure = 100000Pa was added to values calculated from simulation results, gas constant become OK. Sorry for false alarm. Thanks to all Petr

 September 27, 2004, 06:08 Re: gas turbine simulation setup #17 selvarani Guest   Posts: n/a

 November 11, 2004, 16:37 Re: gas turbine simulation setup #18 said Guest   Posts: n/a please sent me gas turbine model

 December 11, 2004, 11:04 Re: gas turbine simulation setup #19 Andhika Wiraswastika Guest   Posts: n/a please sent me gas turbine model n also the program listing in simulink MATHLAB......... thankz...

 January 8, 2005, 08:53 Re: gas turbine simulation setup #20 Bouam Guest   Posts: n/a je cherche un logiciel de simulatioin d'une turbine à gaz

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Andy QUB FLUENT 5 September 19, 2015 06:38 baobaochong Main CFD Forum 0 October 10, 2009 04:44 saii CFX 2 September 18, 2009 08:07 ahourri FLUENT 0 November 14, 2005 10:23 Abdul Hafid Main CFD Forum 1 September 14, 1998 09:39

All times are GMT -4. The time now is 18:43.

 Contact Us - CFD Online - Top