[aras]

Hi,

I have an internal flow inside a pipe. the pipe has many small details inside it in a way that 85% of the flow path inside the pipe is blocked with details.

the operating pressure inside the pipe is high (10 Mpa). I have used K-w turbulence model and the solution is steady state.

I am using pressure-based solver with PISO velocity-pressure coupling. spatial discretization is 1st order momentum and pressure is PRESTO.

I have set the URFs to 0.7 density, 0.3 pressure, and 1 drag force

I am getting continuity divergence right from the 4th or 5th iteration.

can anybody give me a hint what might has gone wrong?

thx alot

[CosmicRay]

Have you tried refining the mesh?!!

[aras]

that's the thing. I have around 4 million mesh right now and I am near my machine capacity.

But how can I be sure that this is the mesh issue?

[CosmicRay]

check the Y+ values around the walls in Fluent. check the skewness of the cells in the preprocessor. Try to use parallel solver if you are not using it to increase your machine capacity

[CFDtoy]

Hi,
are you running compressible flow here? reduce p relax to 0.1, use SIMPLE scheme, upwind settings for all variables.

mesh issues are definitely worth a look but first check your settings. I will also pay attention to initialization of k,w etc..start with high turb energy and dissipation rates to stabilize flow..

Check turb model - start with k-e and then move to k-w. k-e is very dissipative and see if you attain convergence.

Does your pipe have several steps, potential recirculation zones or simply pipe?

Cheers,

CFDtoy

[k_k]

hi,

The obstacle in the flow domain can severely affect convergence. To attain a converged solution place the inlet/outlet boundaries atleast 5-10 times the height of the obstacle. Start the solution with a small under-relaxation factor.

Cheers

[aras]

Originally Posted by CFDtoy

Hi,
are you running compressible flow here? reduce p relax to 0.1, use SIMPLE scheme, upwind settings for all variables.

mesh issues are definitely worth a look but first check your settings. I will also pay attention to initialization of k,w etc..start with high turb energy and dissipation rates to stabilize flow..

Check turb model - start with k-e and then move to k-w. k-e is very dissipative and see if you attain convergence.

Does your pipe have several steps, potential recirculation zones or simply pipe?

Cheers,

CFDtoy

thx for the response.


by high turbulence energy and dissipation, how much you mean? when I am initializing the flow from inlet, it has some values calculated from the inlet, should I make them higher? if yes, roughly how many times?

I tried with k-e instead of k-w with smaller URFs and now I am getting an OK(not excellent) convergence. since my pipe has many walls in there with many obstacles, do you suggest k-e with wall function or k-w?

[aras]

and do you suggest SIMLE or SIMPLEC?

by the way when I change the outlet from pressure outlet to outflow, I am having difficulty to get convergence for the same case, any suggestion on that?

[madhuvc]

@aras,

if you have a pressure inlet I guess its advisable to use pressure outlet BC. Trying using SIMPLE scheme for coupling, STANDARD for pressure scheme, you can change schemes and methods accordingly later.

[aras]

I have a mass flow inlet. do you think which one should I use? outflow or pressure outlet?

[madhuvc]

http://www.cfd-online.com/Forums/flu...condition.html ..hope this helps..

[aras]

but I am getting divergence with outflow while it converges with pressure outlet, any specific reason, you think of?

[satyendra]

hi cosmicRay,

i am trying to solve an incompressible ideal gas problem having two mass flow inlet conditions and two pressure outlet conditions ( i cannot use outflow BC since according to chapter 7, fluent user guide this is not allowed ). hence I have set target mass flow at outlet. But the continuity is not converging. any idea where i am going wrong.

rana

[k_k]

hi,

In my experience, mass flow boundary conditions always show slower convergence. The divergence in you case, I suspect is because the pressure is not explicitely specified in atleast one boundary. I suggest you the following,

1. Try using velocity inlet boundary conditions rather than mass flow inlet. As you are simulating an incompressible flow, it doesnt make a difference as density is fixed.

2. Use pressure outlet at one of the outlet boundary and outflow in the other (if that is allowed in Fluent)

Try these and let us know what happens.

Cheers

[ghafarimahsa]

Hi all,

My system has 3 inlet and several outlets. I measured the flow for inlet and outlet.
I'm using the velocity inlet boundary condition and outflow for outlets. I faced following problem in my simulation.
1. My simulation doesn't converge properly. The lowest continuity is about 10e-2!!! Which is not good at all.
2. My pressure results sounds ridiculous it change from a very high value to a very low value I don't know how can I fix it.

Thank you

[rmn_990]

Hi.
I had this problem and it was solved in this way:
you should "reorder" your mesh until achieving this notice in the command bar :

>> Reordering domain using Reverse Cuthill-McKee method:
zones, cells, faces, done.
Bandwidth reduction = 372525/670 = 556.01
Done.

>> Reordering domain using Reverse Cuthill-McKee method:
zones, cells, faces, done.
Bandwidth reduction = 670/670 = 1.00
Done.


after that you can initialize and run

*reorder :
in Ansys Fluent 17---> menu bar--->setting up domain--->reorder--->domain

Good Luck
Ramin

[oozcan]

should do it twice or one time ?

you have done it twice as bandwidth reduction equal to 1

[bhushanvelis]

Hi,
Thanks CFDtoy, your suggestions worked for me...

[Amir Reza]

Hi.
Thank you rmn_990 it worked for me