Question about "Motion Mach Number" in "Dynamic Mesh Definition" SU2 version3
 

Hi everyone,

I am using su2 to assist my Undergraduate Final Project, My aim is analyzing the flowfield around a quad-rotor UAV. Now I have already generated a mesh file from Pointwise, however, i got confused with how to set up the "Mach_Motion" item in "Dynamic Mesh Definition" in Configure file, it is means the mach number at the tip of rotating blade?? Maybe not.

Actually, I used to use SU2 Version2 to do this simulation, it do not requires the "Mach_Motion", instead it requires the "% Reference length (m) for computing force coefficients (e.g. rotor radius) ROT_RADIUS= " , so I usually type the radius of my blade, the resulted force coefficient always reasonable. However, when I upgrade the SU2 to version3, I try to set the "Mach_Motion" as the Mach number(calculated by angular velocity and radius of blade) at the tip of rotating blade, the resulted force coefficient is really not so reasonable, with the same mesh, same angular speed, force coefficient will become much smaller, than the Version2's force coefficient.

Of course, the calculation of lifting force generated by Blade become senseless(too small). L=Cl * 0.5 *rho*v^2 *S, reference area is=1, dimensionless rho = 1.28, V=MOTION_MACH*331 ?, Cl become much smaller, than the lifting force also become quite small.

(BTW: in some Version2's testcases, it requires the "% Reference speed (m/s) for computing force coefficients (e.g. tip speed)
ROT_VEL_REF= ", however, this option seems useless, because every time when i use the ROT_VEL_REF, there always have a Warning:unrecognized option in the config. file:ROT_VEL_REF)


Best wishes

Jin

Hi Jin,

In going to version 3.0, we made a lot of upgrades and standardized much of the dynamic mesh capabilities in the code. This included incorporating the rotating frame mode into the rest of the dynamic mesh framework (and consolidating options).

We added the motion mach number option to decouple the force coefficient calculation from the free-stream definition for moving mesh applications, as sometimes you might want to non-dim. based on a tip mach number for a rotor, for instance. It also allows you to compute force coefficients that make sense if your free-stream Mach number is zero (rotor in hover, for example).

In order to compute forces for any type of dynamic mesh simulation, see the code on lines ~3500-3525 in solution_direct_mean.cpp, or

/*--- For dynamic meshes, use the motion Mach number as a reference value
for computing the force coefficients. Otherwise, use the freestream values,
which is the standard convention. ---*/
if (grid_movement) {
Gas_Constant = config->GetGas_ConstantND();
Mach2Vel = sqrt(Gamma*Gas_Constant*config->GetTemperature_FreeStreamND());
Mach_Motion = config->GetMach_Motion();
RefVel2 = (Mach_Motion*Mach2Vel)*(Mach_Motion*Mach2Vel);
}
else {
RefVel2 = 0.0;
for (iDim = 0; iDim < nDim; iDim++)
RefVel2 += Velocity_Inf[iDim]*Velocity_Inf[iDim];
}

RefDensity = Density_Inf;
RefPressure = Pressure_Inf;

factor = 1.0 / (0.5*RefDensity*RefAreaCoeff*RefVel2);

Note also that the RefAreaCoeff is the value that set in the following config option:

% Reference area for force coefficients (0 implies automatic calculation)
REF_AREA= 1.0

Between setting the motion mach number to an appropriate value of your choice and entering the correct area, you should be able to recover the type of non-dim. for the force coefficients that you expect.

Hope this helps,
Tom

Just to keep this current, this data is now in solver_direct_mean.cpp, starting at line 4523.

su2 propellersimulation
 

Hi Jin, Hi Tom;
I am also doing a su2 cfd simulation for a propeller blade but facing some difficulties. It seems like I can get a good idea from your project. If its not a problem can you please share you pointwise mesh file and su2 configuration file?
Thank you!