[raptorishungry]

Hello all,

I am trying to implement a swirling flow at the inlet of my geometry (inlet is a circular cross-section) for a 3-D steady, turbulent case. I am varying u(z) and u(theta) for a u(r) = 0, for a fixed resultant Umag (0.6 m/s in all my cases). I have tried the following methods:

1. swirlFlowRateInletVelocity - https://github.com/OpenFOAM/OpenFOAM...hVectorField.H

2. cylindricalInletVelocity - https://github.com/OpenFOAM/OpenFOAM...hVectorField.H

For the aforementioned methods, I am having an unusual spike in the velocity, where the Umag exceeds its actual intended value at the inlet. I am pasting my inlet BC for U folder for both the methods.

//swirlFlowRateInletVelocity
INLET
{
type swirlFlowRateInletVelocity;
flowRate constant 1.69e-05; // based on Umag
rpm constant 8486; // for Utheta = 0.4243 m/s
value uniform (0 0 0);

//type fixedValue;
//value uniform (0 0.6 0);
}


//cylindricalInletVelocity
INLET
{
type cylindricalInletVelocity;
axis (0 1 0);
centre (0 10e-03 0);
axialVelocity constant 0.4243;
radialVelocity constant 0;
rpm constant 8486; // for Utheta = 0.4243 m/s
value uniform (0 0 0);
}


3. I have also tried implementing through coordinate transformation method using groovyBC for the same inlet condition using the following code

INLET
{

type groovyBC;
variables
(
"zp=pos().z;"
"xp=pos().x;"
"r=sqrt(pow(xp,2)+pow(zp,2));"

"U_theta=0.4243;" // inputs
"U_axial=0.4243;" //inputs
"U_radial=0;" // inputs
"theta=atan(zp/xp);"
"U_x=U_radial*sin(theta)+U_theta*cos(theta);" // conversion to cartesian
"U_z=U_radial*cos(theta)-U_theta*sin(theta);" // conversion to cartesian
);
valueExpression "vector ( U_x, U_axial, U_z )"; // the cylindrical axis is along Y

}

For this case, the contour seems wrong and the stream lines do not seem to indicate the swirling motion.

I have attached all the plots for your kind perusal. It would be very helpful if anyone could elucidate me on this issue. Thanks in advance.

OpenFOAM version: 3.0.1

[Scram_1]

Hi Adithya!
Even I'm facing a similar issue.
I'm getting unphysical results with regards to u(r). I've tried the swirl velocity inlet BC. It would be helpful if someone could post a solution to this problem.

[raptorishungry]

Could someone please shed some light on this issue?


Thanks,

Adithya Gurumurthy

[Pravin Kadu]

I used this
[Note - my cylinder center is at (0,0,0)]

inlet2
{
type groovyBC;
variables
(
"yp2=pos().y;"
"zp2=pos().z;"
"r2=sqrt(pow(zp2,2)+pow(yp2,2));"

"U_ax2=0.5496*pow((1-mag(r2-0.0095)/(1.001*0.0035)),(1/7));"
"U_t=0.15*(1-pow((mag(r2-0.0095)/(1.001*0.0035)),2));"

"U_tz=-U_t*yp2/r2;"
"U_ty=U_t*zp2/r2;"
);
valueExpression "vector ( U_ax2, U_ty, U_tz )";
value uniform (0 0 0);
}

[raptorishungry]

Thank you Pravin! I am getting realistic results now

[HappyS5]

Originally Posted by Pravin Kadu

I used this
[Note - my cylinder center is at (0,0,0)]

inlet2
{
type groovyBC;
variables
(
"yp2=pos().y;"
"zp2=pos().z;"
"r2=sqrt(pow(zp2,2)+pow(yp2,2));"

"U_ax2=0.5496*pow((1-mag(r2-0.0095)/(1.001*0.0035)),(1/7));"
"U_t=0.15*(1-pow((mag(r2-0.0095)/(1.001*0.0035)),2));"

"U_tz=-U_t*yp2/r2;"
"U_ty=U_t*zp2/r2;"
);
valueExpression "vector ( U_ax2, U_ty, U_tz )";
value uniform (0 0 0);
}

Pravin,

I am new to CFD but I am learning the best I can.

In the near future, I will be modeling a nozzle that has significant swirl at the inlet. So, I found your discussion useful.

Sadly, I am ignorant to the code that you use in your post. Can you explain each step for me? I know it is a lot to ask, but I will benefit greatly from your tutorial.

[Krao]

Hi Chris

Originally Posted by HappyS5

Pravin,

I am new to CFD but I am learning the best I can.

In the near future, I will be modeling a nozzle that has significant swirl at the inlet. So, I found your discussion useful.

Sadly, I am ignorant to the code that you use in your post. Can you explain each step for me? I know it is a lot to ask, but I will benefit greatly from your tutorial.

I am also trying to simulate a propeller with swirl at the inlet. As I am planning to implement parabolic swirl at the inlet, it would be great if I know the expansion of the code too. If you have already found the explanation please post that here. Else, I would also request other members to give us some hint where we can find the theory of all these GroovyBCs.

Thank you all in advance

Krao

[Krao]

Originally Posted by HappyS5

Pravin,

I am new to CFD but I am learning the best I can.

In the near future, I will be modeling a nozzle that has significant swirl at the inlet. So, I found your discussion useful.

Sadly, I am ignorant to the code that you use in your post. Can you explain each step for me? I know it is a lot to ask, but I will benefit greatly from your tutorial.

I have got a better understanding now although not completely! I still don't know the meaning of the numerical values in the equation. If you have not gone through these links then it may help you as well, https://openfoamwiki.net/images/d/db...mReference.pdf, https://openfoamwiki.net/images/7/7a...icTraining.pdf

[Alizarei]

Thank you friend for your help
I was trying for Swirlvelocity inlet boundary condition and every time it showed an error for essentioaly " value " and when i added the last line of your description it worked.thank you so much man