[Spacehorse]

Hi,

I am trying to set up a simulation of water flowing past a 3D object to solve for drag force and lift force.

This seems similar to a wind tunnel like case so I was assuming I could copy a tutorial such as simpleFoam airFoil2D and modify it to be 3D, add my geometry and change the fluid from air to water.

I am a bit stuck as to how I specify the fluid is water.

If anyone has any suggestions on a better way to set up this case I would be very grateful!

Thank you.

[Krapf]

Hi Spacehorse

in your case you have to modify the values in constant/transportProperties to change the fluid from air to water. If the solver is compressible you have to adapt constant/thermophysicalProperties.

My approach would be similar. If I don't have a project of my own that could serve as a basis, I would look for a tutorial that is as similar as possible.

Kind regards
Krapf

[Spacehorse]

Thank you for your help.

So for instance if in the transportProperties file only 'nu' was listed. I would change the kinematic viscosity.

I would also add density I've assumed? rho.

are there any other properties which are required for a fluid flow case solving for drag force?

Kind regards,

[Krapf]

Yes, you change the kinematic viscosity.
The density is not required. No idea why it is specified in airFoil2D. It also works if you delete the density and I cannot find a difference in the log file.

Take a look at the files in $FOAM_ETC/caseDicts/postProcessing/forces. You can find tutorials which calculate forces/force coefficients with "foamInfo forces"/"foamInfo forceCoeffs" (depending on which OpenFOAM version you use).

[Spacehorse]

Hi Krapf,

Thanks again for your help!

Really useful information once again.

FYI I decided to specify rho as I thought that might be needed.

So currently in the system folder I have the forceCoeffs file and if i want the forces to be solved for I will add the forcesIncompressible file which you have pointed me to?

I have actually decided to use the motorbike tutorial as my base project and have successfully made modifications to it and completed a simulation on my own geometry (3D cylinder). It seems successful but now I suppose I need to make a verification case.

Thanks again,
Spacehorse

[Krapf]

Originally Posted by Spacehorse

So currently in the system folder I have the forceCoeffs file and if i want the forces to be solved for I will add the forcesIncompressible file which you have pointed me to?

That's correct.

[Spacehorse]

So to update.

I have successfully completed the simulation with the following set up:

inlet free-stream velocity: 2.57m/s (5knots)
rho = rhoInf = 1020 (salt water)
nu = 1.04e-06
geometry is a cylinder with flat end facing the inlet
dimensions of cylinder = d=0.275m, L=0.745m

one of the next steps is to refine the mesh and make it better quality.
But first I'm not sure if the results are accurate or even in the right ball park. please see below.

end of simpleFoam string below:

forceCoeffs forceCoeffs1 execute:
Coefficients
Cd : 0.278398 (pressure: 0.273802 viscous: 0.00459598)
Cs : 0.000558303 (pressure: 0.000496108 viscous: 6.21959e-05)
Cl : -8.05953e-06 (pressure: -7.73975e-06 viscous: -3.19779e-07)
CmRoll : -6.3528e-08 (pressure: -5.72014e-08 viscous: -6.32661e-09)
CmPitch : 1.71585e-06 (pressure: 1.63512e-06 viscous: 8.0728e-08)
CmYaw : 0.00106991 (pressure: 0.00110496 viscous: -3.50432e-05)
Cd(f) : 0.139199
Cd(r) : 0.139199
Cs(f) : 0.00134907
Cs(r) : -0.000790763
Cl(f) : -2.31391e-06
Cl(r) : -5.74561e-06
forces forces write:
Sum of forces
Total : (221.184 -0.0064032 -0.443566)
Pressure : (217.532 -0.00614914 -0.394152)
Viscous : (3.65145 -0.000254061 -0.0494139)
Sum of moments
Total : (-3.76018e-05 0.633276 -0.0010156)
Pressure : (-3.38571e-05 0.654018 -0.000967819)
Viscous : (-3.74468e-06 -0.0207419 -4.77824e-05)


ensightWrite ensightWrite write: ( k omega p U )
End

So the drag coefficient looks a bit low for what I've read online.
And also what unit is the pressure output? is that the drag force or do I have to make further calculations from that?
I read in a thread somewhere that with in-compressible sims you need to multiply the outputted force with the density of the fluid?

I'm very grateful for any input on this.

[Krapf]

Force is in N, Moment in Nm
If you set the correct value for rhoInf, you do not need to multiply the output value.

What you probably read is that you have to multiply the pressure (not the pressure forces) by the density if you want to have it in Pascal.