Laminar , steady state pipe flow
 

I would like to solve steady state, laminar flow of newtonian fluid in cylindrical pipe. Can you please suggest which solver would be more appropriate.

Thank a lot

Sam

laminar solver
 

hi sam ,
the simple and the most basic solver for a laminar and incompressible flow is icoFoam.

Hi Sudharshan,

Thank you for your reply.

icofoam solver solves transient, laminar and incompressible newtonian flow. But I am looking to solve for steady state, laminar and incompressible newtonian flow.

Can I use simplefoam to solve laminar flow by changing code?

Hi,

To use simpleFoam for laminar flow, you have to edit constant/RASProperties of your case and change RASModel to laminar.

Regards,
Jose Santos

You can also use icoFoam. Although the solver is transient, you will get an steady-state solution after some time, since the flow itself becomes steady-state. as far as I know, a steady-state solver does exactly the same, it solves the equations with the time derivatives and the solution proceeds in time until a steady-state is reached. I did this for a rectangular channel flow and it worked well.

hi sam,
you can use simpleFoam for your case but need to edit RAS properties before using. Good luck.

regards,
sudharsan

Thank you to all.

I will solve the my problem using simplefoam. I will let u know if I face any difficulty.

Thank you.
Sam

Dear Sam

I am trying to solve a steady state incompressible laminar flow for a pipe with circular cross section, but I didn't get the fully developed parabolic shape for velocity profile.
I am using simpleFOAM (OF-2.1.0) where I have changed the RAS properties to laminar and set the turbulent off. Could you please suggest me, where is the problem? Do you able to solve this simple problem?

If you give me your email ID, I can send you the files.

Thanks

Goutam

Hi Sam,
I have used icoFoam for this problem and nonNewtonianicoFoam for the corresponding non-Newtonian case. Both work very well, it is also easy to cross check with the analytical values.
Regards,
Lachlan

switch off turbulence , use laminar in the RAS file of /const floder

Hi,

I would like to know, if it is possible to solve a laminar flow in a cylindrical pipe using 2d simulations in openfoam. If so, please can anyone let me know, how to construct the geometry. Further, should we change anything in the icoFoam solver.

Thanks

Regards
Vishal

2D simulations - Reg
 

Dear Nandhigana Vishal,

You can create 2D simulations by considering a wedge shaped geometry as shown in Figure 5.3 in OpenFOAM manual 2.0.0.

For creating wedge refer Figure 5.7 in the same manual.

Dear Kannan,

Thanks for your reply. I had a chance to go through the manual earlier, but could not exactly follow how the geometry and boundary conditions are incorporated using the wedge BC. For instance, I would like to create a cylinder of length 8 m and diameter 0.1 m. The inlet of the cylinder has a uniform velocity and the walls have no slip. How do we create this geometry and what angle should be specified for the wedge. Can you please illustrate this with an example along with the patch definitions.

Thanks for the help

Vishal

Simple solution
 

Dear Vishal,

1. Create an wedge (Angle of 5 Degree). Simply a hex collapsed to form a wedge as shown in manual.
2. Axis is type empty
3. Front and back face type wedge
4. For velocity use type uniform and fixed value

Go through Cavity and pitzdaily examples in OpenFOAM tutorial once for understanding and kindly follow the above.
Of course you will find difficulty. But try once then you will get it.

Hi Kannan,

Thanks for your reply. I got an understanding on the geometry construction for a simple cylinder. However, I would like to construct a concentric pipe type geometry. I would like to know if the same angle (=5 degree) should be specified for the inner cylinder too. In the manual, it says the angle should be less than 5 degrees to construct 2d axis symmetric cylinder type geometries. Could you explain why this should be the case.

Thanks

Regards
Vishal

Dear Vishal,

For 2D simulations we must have one cell thickness for FVM. I guess this may be the reason (or) OpenFOAM defines 2D when the angle is less than 5 degrees with one cell in thickness.

Hi Kannan,

Thanks for the reply. I have constructed the wedge geometry for a simple laminar pipe flow.

I wanted to simulate a laminar flow with inlet velocty = 1m/s in a cylindrical pipe of Diameter = 0.2 m and length = 8 m. I have considered kinematic viscosity = 2e-3 Pa.s and density = 1kg/m^3.

I have tried using both SimpleFoam (switching off turbulence) and icoFoam. However, the code does not converge. I am attaching the files. Please let me know, if the geometry construction is accurate, considered (theta = 5 degree).

Thanks

Regards
Vishal

Dear Vishal,
The geometry is fine but there are errors in grid. Kindly check the mesh using ""checkMesh"" and correct it. What I found is
***Number of non-orthogonality errors: 19800.
***Error in face pyramids: 59900 faces are incorrectly oriented.
Failed 2 mesh checks.

Kindly correct these errors and submit the grid for solution.

Thanks, very much Kannan. I found the bug. I had changed the direction of z axis in my new blockMesh file and that did the trick. Now the solver works. I would now like to check the solution and would then move on to making a concentric pipe geometry. Is there anything I should make a note of while constructing the concentric pipe geometry. Let me know.

Thanks

Vishal

Hi Kannan,

As we have created a wedge whose faces are not aligned to the cooridnate plane. So the maximum height in the radial direction now corresponds to (r*cos(theta/2)) and not exactly "r". Should we rescale the values obtained for the velocity and pressure in the radial direction ? Please let me know.

Thanks

Regards
Vishal

Dear Vishal,

We are assuming wedge as an approximation to simplify the domain.

Radius is R

{because R*0.999 is approximately equals R only right ??};)

--
KANNAN

You are right :P... was just curious why it was thought about to construct the geometry in this manner :). The geometry works fine. Thanks for your tips.

Hi Kanan,

I am now modeling a concentric pipe geometry. I have difficulty in understanding which faces I should generate the mesh. I would like to give boundary conditions on both the surface of inner pipe and on the outer pipe. Here is the sample blockmesh dict file that I have generated.

// length of pore = 36 nm and diameter: 10.2nm , theta = 2 deg (consider this as outer pipe)
// length of DNA = 36 nm and diameter of DNA: 2.2nm , theta = 2 deg (consider this as inner pipe)
//r_DNA*cos(theta/2) = 1.1*cos(0.0349/2 radians) = 1.0998
// r_DNA*sin(theta/2) = 1.1*sin(0.0349/2 radians) = 0.0192
//r_pore*cos(theta/2) = 5.1*cos(0.0349/2 radians) = 5.0992
//r_pore*sin(theta/2) = 5.1*sin(0.0349/2 radians) = 0.0890
vertices
(
(0 0 0) // vertex 0
(36 0 0) // vertex 1
(36 1.0998 -0.0192) // vertex 2 (L,r_DNA*cos(theta/2),-r_DNA*sin(theta/2))
(0 1.0998 -0.0192) // vertex 3 (0,rcos(theta/2),-rsin(theta/2))
(36 5.0992 -0.0890) // vertex 4 (L,r_pore*cos(theta/2),-r_pore*sin(theta/2))
(0 5.0992 -0.0890) // vertex 5 (0,r_pore*cos(theta/2),-r_pore*sin(theta/2))


(0 0 0.0192) // vertex 6 (0, 0,r_DNA*sin(theta/2))
(36 0 0.0192) // vertex 7 (L, 0,r_DNA*sin(theta/2))
(36 1.0998 0.0192) // vertex 8 (0, r_DNA*cos(theta/2),r_DNA*sin(theta/2))
(0 1.0998 0.0192) // vertex 9 (L, r_DNA*cos(theta/2),r_DNA*sin(theta/2))
(0 0 0.0890) // vertex 10 (0, 0,r_pore*sin(theta/2))
(36 0 0.0890) // vertex 11 (L, 0,r_pore*sin(theta/2))
(36 5.0992 0.0890) // vertex 12 (L,r_pore*cos(theta/2),r_pore*sin(theta/2))
(0 5.0992 0.0890) // vertex 13 (0,r_pore*cos(theta/2),r_pore*sin(theta/2))
);

Please let me know if the vertices are correct. If so, how to generate the mesh for the same.

Thanks

Regards
Vishal

hi thanks every one for posting the reply. i have a question i would like to simulate a steady state simulate in ico foam so i changed to
ddtScheme
{
type steadystate;
}

Then i got this error

FOAM Warning :
From function gaussConvectionScheme
in file finiteVolume/convectionSchemes/gaussConvectionScheme/gaussConvectionScheme.H at line 123
Reading "/home/yathuru/task1steady/system/fvSchemes.divSchemes.div(phi,U)" at line 31
Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.
To remove this warning switch off 'boundedGauss' in "/opt/OpenFOAM-2.3.0/etc/controlDict".


can some one help me.. i m lost.

Hi,

icoFoam is a transient solver. If you need steady state, simpleFoam is probably what you need.

Regards,
Jose

Dear Naresh,

It's just a warning I guess you can run your case with that.

OR, you can remove the warning as follows:

-
Best Regards!

Thank you so much for your reply santos and tushar. I knew i can do it in simple foam but just out of curiosity i wanted to try it in ico foam. I ran the simulation in simple foam its working well then i changed the case to turbulent simulation its is also working well now. :) however i have some issues with the convergence. i will try to figure it out.:) if not i will get back again .

Dear Naresh,

Please refer my previous post again. I said that you can run your icofoam solver using the steady state command. Anyways I am writing these again:

Best Luck!

Thanks once again Tushar. I m afraid if i can post this question here.

could you please give me some tips for which solver to use for this case below:

Geometry : a room with a box inside. the room has a inlet and outlet.

I want to simulate the flow through this room with some velocity and temperature at the inlet, the roof is maintained at a low temperature (20 C) and the box inside is maintained at a temperature (35C).


could you please suggest a solver. :)

Dear Naresh,

I will prefer you to go for "BuoyantBoussinesqPisoFoam", this will do the job. Wish you Good Luck for your work.

-
Best Regards!

Thank you once again for your continuous support. U have no idea how much this tipp mean to me. thanks.:)

Welcome :)

-
Best Luck!