Dear all I am using macro Turbo_Perform. How can I calculate the rotating "wetted" surface region?

Thank!

Here a copy of macro from TASCFLOW

Define Macro TURBO_PERFORM

-- Define Parameter quiet=on define parameter _liquid=off -- -- -- Print menu to select machine type -- echo echo DISCLAIMER: The following macros have been supplied to assist in the echo performance estimation of several types of turbomachines. The equations echo were obtained from available literature, however some equations may have echo alternate definitions. echo echo It is YOUR RESPONSIBILITY to verify the accuracy of these definitions. echo echo echo MACHINE TYPE echo ============ echo echo 1.) Liquid Pump echo 2.) Liquid Turbine echo 3.) Compressor echo 4.) Gas Turbine echo echo Enter the number indicating the machine type: --

input MACHINE

Define parameter MACHTYPE=$MACHINE -- -- Check for the existence of multiple reference frames --

mfr_check -- -- Prompt the user for an inlet region and an outlet region -- echo echo Enter the inlet region: --

input _X_INLET

Define region REGION_1=$_X_INLET -- if (existparameter 'MFR_CHECK') echo echo Enter the number of blades or sectors for this region: --

input IN_BLADENUM endif -- echo echo Enter the outlet region: --

input _X_OUTLET

Define region REGION_2=$_X_OUTLET -- echo echo Enter the rotating "wetted" surface region. This region must not echo have duplicate nodes if multiple subregions are specified. --

input _X_BLADE

Define region REGION_3=$_X_BLADE -- echo echo Enter the number of rotor blades: --

input BLADENUM if (existparameter 'MFR_CHECK') else

define parameter IN_BLADENUM = $BLADENUM endif -- calc PI=4.0*atan(1.0) --

The rotating "wetted" surface region is used in the macro to calculate the torque and thrust values. It is the surface(s) in the rotating part of your grid (i.e. impeller) that are in contact with the fluid (generally - hub, shroud and impeller blades).

Hope this helps

Roy

Thank you very much for your advise. Hence I can use region manager to correct a blade regions. I am not sure this region include hub with it and all blade region or not for example pressure side or suction side only because this parameter not appear again in macro source code.

If your blade grid was generated through Turbogrid there should be blade regions generated for your blade that detail pressure/suction, leading edge and trailing edge surfaces (if present). This will depend on the template used - but generally I think the region is simply named blade_# (where # goes from 1 to the number of blades present in your model). The blade_bo named regions are 3D blade regions and not the surfaces. Find out which regions you are interested in - create a new region and use the "add" region facility to add in all the regions you want to your new region that will then contain all the wetted surfaces of your impeller. Then go through your regions removing the duplicate nodes.

Roy

I used single block grid template of Turbogrid and put "blade" as a wetted surface region in macro but output show me Output:

Torque (one blade) = 0

Torque (all blades) = 0

Power (all blades) = 0

Thrust (one blade) = 0

Thrust (all blades) = 0 so I think the problem came form a wetted surface region. How do you think about this problem?Why torque equal zero? This macro was used to analyze performance of axial flow pump diameter 10 cm Head 1.8 M Q 4.5 kg/s design by vortex theory, used NACA airfoil .

Regards

Have you viewed the "blade" region to check that it is indeed the surfaces on the impeller blade. Also check that the region is not blade_#gridname where #gridname is whatever you have called the impeller grid.

Yes, I did indeed.When I use show in Tasctool and then select 5 to show parameter for make sure blade region name = blade and display it in GUI mode again to make sure this region is blade surface. I am not clear about blade_#gridname, what do you mean? could you please explain again or show me anothre example.

If I append an impeller to an existing TASCflow model I often give it the name "IMP", which would mean my blade region name would become blade_imp.

If you can see the region and are happy with it - then it is unlikely to be the region that is at fault.

The next thing to check is that your scalar fields includes the following scalars:

area_wall_y area_wall_z

These fields must be present for the macro to calculate the Torque/Power/Thrust. If they do not exist you will receive a zero output from your calculation. These scalars must be output at the time of the analysis - when the rso is written.

To output the required data the following commands must be placed in the prm file.

BCINFO = t

You can do this manually (just type and save)or you can switch it on via the Solver Monitor and selecting

Parameters/Additional Solver Parameters/I/O Control

and looking in Boundary Data and check the BCINFO box.

You will then have to continue your analysis from where you completed it before, for only a single iteration. When the rso is re-written this time the above command will write the required scalars to your rso file. Once this is done - re-run the macro as before.

I hope this helps

Roy

I hope so, thank you very much for your lecture, I will try and show you again what I get.

Thank you, this can help me, now I can calculate torque.

Regards C-CARE #