[swak4Foam] Problem with fully developed velocity profile groovyBC in 2D axi-sym mesh

harshad88 · July 17, 2014, 01:37

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??

gschaider · July 22, 2014, 18:07

Quote:

Originally Posted by harshad88

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??

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, 02:19

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, 07:58

Quote:

Originally Posted by harshad88

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

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, 13:02

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

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

gschaider · July 24, 2014, 14:30

Quote:

Originally Posted by harshad88

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

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, 14:50

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, 15:28

Quote:

Originally Posted by harshad88

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

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
sliding mesh problem in CFX	Saima	CFX	46	September 11, 2021 08:38
Patch fully developed velocity and turbulence profile over full domain	Teumde	FLUENT	2	June 29, 2015 14:47
[swak4Foam] problem with Velocity Profile with groovyBC	ssss	OpenFOAM Community Contributions	1	August 7, 2014 15:44
Fully developed temperature profile for laminar/turbulent flow in FLUENT	raghu.tejaswi	FLUENT	10	November 7, 2012 10:57
A girl fail to plot velocity profile when mesh changes + Wall function	asherah	STAR-CCM+	0	February 19, 2010 18:45

July 24, 2014, 02:19		#3
harshad88 New Member Harshad Lalit Join Date: May 2013 Posts: 26 Rep Power: 13	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!

July 24, 2014, 14:50		#7
harshad88 New Member Harshad Lalit Join Date: May 2013 Posts: 26 Rep Power: 13	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.