CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Community Contributions (https://www.cfd-online.com/Forums/openfoam-community-contributions/)
-   -   [swak4Foam] Problem with fully developed velocity profile groovyBC in 2D axi-sym mesh (https://www.cfd-online.com/Forums/openfoam-community-contributions/139087-problem-fully-developed-velocity-profile-groovybc-2d-axi-sym-mesh.html)

harshad88 July 17, 2014 00:37
Problem with fully developed velocity profile groovyBC in 2D axi-sym mesh
 
Hello All,

I am studying a premixed jet flame using reactingFoam in a 2D axisymmetric mesh and using a groovyBC to simulate fully developed turbulent flow through the premixed inlet. The geometry has a wall beside the premixed inlet (at x=0.0075m). I am using the following code to set up my velocity profile:

Code:
Inlet
    {
        type groovyBC;
              value uniform (0 0 0);
              variables (
                "n=7;"  //power law coefficient n
                "R=0.0075;"  //pipe radius
                "Umean=7.5;"  //calculate mean velocity
                "Umax=13.2;"  //calculate max velocity
                "profile=Umax*pow(1-sqrt(pow(pos().x,2)+pow(pos().z,2))/R,(1/n));"
                //calcucate power law velocity profile Umax*(1-r/R)^(1/n)
                );
              valueExpression "normal()*-profile";
              //apply to boundary, normal() is surface normal vector and minus is needed for inflow
    }
However, when I extract the velocities using the sampleDict utility I do not see my velocities going to 0 at the intersection with the wall.
Code:
x        y        z        u(m/s)                v(m/s)                w(m/s)
0        0        0        0                13.097                0
0.00105        0      0      1.8e-2          12.9125        -7.34282e-06
0.0021        0        0        0.000278988        12.5902                -8.95149e-06
0.003        0        0        -0.00146174        12.2672                -2.48713e-07
0.00375        0        0        -0.00351349        11.9474                -2.31918e-05
0.0039        0        0        -0.00399891        11.8788                -9.06154e-06
0.0042        0        0        -0.00526191        11.7293                -3.19546e-05
0.0045        0        0        -0.00667307        11.5738                -1.0456e-06
0.0051        0        0        -0.0111364        11.2036                -3.2705e-05
0.00555        0        0        -0.0147763        10.8722                5.90284e-06
0.0057        0        0        -0.0148122        10.7366                2.19331e-05
0.006        0        0        -0.0149064        10.4634                -4.21239e-07
0.00645        0        0        -0.0167839        9.89666                -2.98323e-06
0.0066        0        0        0.00138561        9.61408                0.000813393
0.00675        0        0        0.0273102        9.29285                0.00173083
0.0069        0        0        0.0532349        8.97162                0.0006639
0.00705        0        0        0.0728419        8.32117                0.000127202
0.0072        0        0        0.0820423        7.12842                0.000463938
0.00735        0        0        0.0912427        5.93567                0.000299331
0.0075        0        0        0.0918162        4.74207                -0.0003617
Can anyone please help me out and tell me what have I done wrong here? Why aren't my velocities 0 at the endpoint?? :confused:

gschaider July 22, 2014 17:07
Quote:
Originally Posted by harshad88 (Post 501873)
Hello All,

I am studying a premixed jet flame using reactingFoam in a 2D axisymmetric mesh and using a groovyBC to simulate fully developed turbulent flow through the premixed inlet. The geometry has a wall beside the premixed inlet (at x=0.0075m). I am using the following code to set up my velocity profile:

Code:
Inlet
    {
        type groovyBC;
              value uniform (0 0 0);
              variables (
                "n=7;"  //power law coefficient n
                "R=0.0075;"  //pipe radius
                "Umean=7.5;"  //calculate mean velocity
                "Umax=13.2;"  //calculate max velocity
                "profile=Umax*pow(1-sqrt(pow(pos().x,2)+pow(pos().z,2))/R,(1/n));"
                //calcucate power law velocity profile Umax*(1-r/R)^(1/n)
                );
              valueExpression "normal()*-profile";
              //apply to boundary, normal() is surface normal vector and minus is needed for inflow
    }
However, when I extract the velocities using the sampleDict utility I do not see my velocities going to 0 at the intersection with the wall.
Code:
x        y        z        u(m/s)                v(m/s)                w(m/s)
0        0        0        0                13.097                0
0.00105        0      0      1.8e-2          12.9125        -7.34282e-06
0.0021        0        0        0.000278988        12.5902                -8.95149e-06
0.003        0        0        -0.00146174        12.2672                -2.48713e-07
0.00375        0        0        -0.00351349        11.9474                -2.31918e-05
0.0039        0        0        -0.00399891        11.8788                -9.06154e-06
0.0042        0        0        -0.00526191        11.7293                -3.19546e-05
0.0045        0        0        -0.00667307        11.5738                -1.0456e-06
0.0051        0        0        -0.0111364        11.2036                -3.2705e-05
0.00555        0        0        -0.0147763        10.8722                5.90284e-06
0.0057        0        0        -0.0148122        10.7366                2.19331e-05
0.006        0        0        -0.0149064        10.4634                -4.21239e-07
0.00645        0        0        -0.0167839        9.89666                -2.98323e-06
0.0066        0        0        0.00138561        9.61408                0.000813393
0.00675        0        0        0.0273102        9.29285                0.00173083
0.0069        0        0        0.0532349        8.97162                0.0006639
0.00705        0        0        0.0728419        8.32117                0.000127202
0.0072        0        0        0.0820423        7.12842                0.000463938
0.00735        0        0        0.0912427        5.93567                0.000299331
0.0075        0        0        0.0918162        4.74207                -0.0003617
Can anyone please help me out and tell me what have I done wrong here? Why aren't my velocities 0 at the endpoint?? :confused:
How are you sampling? Because the values are strange anyway (I guess the x and the z component should be exactly zero if the patch has a normal (0,1,0) ).

To check which values groovyBC sets I usually
a) have a look at the written field file
b) open the case in paraview. Deselect internalField, select the patch in question and inspect it in PV

harshad88 July 24, 2014 01:19
Hello Bernhard. Thanks for your reply . I am sampling using the "uniform" technique in the sample utility, however I have deleted a couple of columns of my data to keep it short.

I was wondering if my problem has something to do with the mesh. My axisymmetric domain has the axis in the vertical - Y direction , whereas most of the problems I have seen have their axis in the horizontal X direction. Will my mesh be still consistent with the OpenFoam format? Please let me know. Thanks!

gschaider July 24, 2014 06:58
Quote:
Originally Posted by harshad88 (Post 502906)
Hello Bernhard. Thanks for your reply . I am sampling using the "uniform" technique in the sample utility, however I have deleted a couple of columns of my data to keep it short.
Use "midPoint" and the interpolation scheme "cell" if you want to know the real value in the cells. "uniform" and any kind of interpolation is for preparing the data for presentations etc but not for finding problems. Because you might as well have a problem with the interpolation.

Quote:
Originally Posted by harshad88 (Post 502906)
I was wondering if my problem has something to do with the mesh. My axisymmetric domain has the axis in the vertical - Y direction , whereas most of the problems I have seen have their axis in the horizontal X direction. Will my mesh be still consistent with the OpenFoam format? Please let me know. Thanks!
Don't think so. If you think the orientation is a problem you can always use the transformPoints-utilitiy to rotate the mesh

harshad88 July 24, 2014 12:02
1 Attachment(s)
Hi Bernhard,

So instead of having a groovyBC i just put in a fixedValue bc (0.0 13.0 0.0) for my inlet. The domain next to the inlet is a wall (0.0 0.0 0.0). I used the "midpoint" sampling technique with 'cell' interpolation and the following in the output I got for velocity at inlet after 0.01 seconds.

Code:
distance, Ux, Uy, Uz
0.000124881, -0.000182222, 13.0002, 6.40391e-14
0.000374643, -0.000366104, 13.0002, 1.46322e-13
0.000624405,-0.000569023, 13.0001, 2.17518e-13
0.000874167, -0.000749703, 13, 1.79184e-13
0.00112393, -0.000908129, 12.9999, 1.23171e-13
0.00137369, -0.00105632, 12.9999, 1.11654e-13
0.00162345, -0.00120575, 12.9998, 1.72996e-13
0.00187322, -0.00136315, 12.9998, 3.27864e-13
0.00212298, -0.00153432, 12.9998, 5.30865e-13
0.00237274, -0.00172296, 12.9998, 4.06978e-13
0.0026225, -0.00193339, 12.9997, 3.88529e-13
0.00287226, -0.00217462, 12.9997, 4.72995e-13
0.00312203, -0.00245306, 12.9997, 2.78539e-13
0.00337179, -0.00277999, 12.9997, 1.41409e-13
0.00362155, -0.00318224, 12.9997, 6.0643e-14
0.00387131, -0.00367517, 12.9997, 6.17558e-15
0.00412107, -0.00431001, 12.9998, -4.18723e-14
0.00437084, -0.00515109, 12.9998, -8.86959e-14
0.0046206, -0.00625099, 12.9999, -1.175e-13
0.00487036, -0.00772528, 12.9999, -8.92134e-14
0.00512012, -0.00974374, 13, -5.14688e-14
0.00536988, -0.012564, 13.0001, -2.47128e-14
0.00561965, -0.0165905, 13.0004, -9.6174e-15
0.00586941, -0.0225386, 13.0008, -1.10196e-15
0.00611917, -0.0317697, 13.002, 4.90887e-15
0.00636893, -0.0458528, 13.0047, 8.50871e-15
0.00661869, -0.0621625, 13.0074, 7.54421e-15
0.00686846,-0.0489905, 12.9861, 3.24075e-14
0.00711822, -0.202212, 12.8795, 8.25841e-14
0.00736798, 0.487566, 12.1117, 2.76338e-14
The velocity drops to 12.11 m/s even before reaching the wall. The Ux is also non-zero in this domain. Not able to fathom why this is happening :confused:

I have attached an image of the closeup of mesh (the highlighted part is my inlet)

gschaider July 24, 2014 13:30
Quote:
Originally Posted by harshad88 (Post 503020)
Hi Bernhard,

So instead of having a groovyBC i just put in a fixedValue bc (0.0 13.0 0.0) for my inlet. The domain next to the inlet is a wall (0.0 0.0 0.0). I used the "midpoint" sampling technique with 'cell' interpolation and the following in the output I got for velocity at inlet after 0.01 seconds.

Code:
distance, Ux, Uy, Uz
0.000124881, -0.000182222, 13.0002, 6.40391e-14
0.000374643, -0.000366104, 13.0002, 1.46322e-13
0.000624405,-0.000569023, 13.0001, 2.17518e-13
0.000874167, -0.000749703, 13, 1.79184e-13
0.00112393, -0.000908129, 12.9999, 1.23171e-13
0.00137369, -0.00105632, 12.9999, 1.11654e-13
0.00162345, -0.00120575, 12.9998, 1.72996e-13
0.00187322, -0.00136315, 12.9998, 3.27864e-13
0.00212298, -0.00153432, 12.9998, 5.30865e-13
0.00237274, -0.00172296, 12.9998, 4.06978e-13
0.0026225, -0.00193339, 12.9997, 3.88529e-13
0.00287226, -0.00217462, 12.9997, 4.72995e-13
0.00312203, -0.00245306, 12.9997, 2.78539e-13
0.00337179, -0.00277999, 12.9997, 1.41409e-13
0.00362155, -0.00318224, 12.9997, 6.0643e-14
0.00387131, -0.00367517, 12.9997, 6.17558e-15
0.00412107, -0.00431001, 12.9998, -4.18723e-14
0.00437084, -0.00515109, 12.9998, -8.86959e-14
0.0046206, -0.00625099, 12.9999, -1.175e-13
0.00487036, -0.00772528, 12.9999, -8.92134e-14
0.00512012, -0.00974374, 13, -5.14688e-14
0.00536988, -0.012564, 13.0001, -2.47128e-14
0.00561965, -0.0165905, 13.0004, -9.6174e-15
0.00586941, -0.0225386, 13.0008, -1.10196e-15
0.00611917, -0.0317697, 13.002, 4.90887e-15
0.00636893, -0.0458528, 13.0047, 8.50871e-15
0.00661869, -0.0621625, 13.0074, 7.54421e-15
0.00686846,-0.0489905, 12.9861, 3.24075e-14
0.00711822, -0.202212, 12.8795, 8.25841e-14
0.00736798, 0.487566, 12.1117, 2.76338e-14
The velocity drops to 12.11 m/s even before reaching the wall. The Ux is also non-zero in this domain. Not able to fathom why this is happening :confused:

I have attached an image of the closeup of mesh (the highlighted part is my inlet)
This is OK: you set a zero-velocity BOUNDARY CONDITION. This is only valid in the boundary faces. In the boundary cell the velocity is calculated from that BC and the other cells and for low velocities may be as high as you show it

The sample utility is good for looking at cell values. If I want the face values on a patch I usually have a look at the field-file or check it in ParaView

harshad88 July 24, 2014 13:50
But shouldnt atleast the Ux be 0 because my velocity is only in the y-direction?

The Ux seems to be pretty signicant and not close to zero unlike the Uz.

gschaider July 24, 2014 14:28
Quote:
Originally Posted by harshad88 (Post 503034)
But shouldnt atleast the Ux be 0 because my velocity is only in the y-direction?

The Ux seems to be pretty signicant and not close to zero unlike the Uz.
Well: the wall is slowing the fluid down but the BC pushes from the back. To preserve conservation it has to go somewhere. In your case: left


All times are GMT -4. The time now is 09:28.