You do not need to do a time step independance check for a steady state simulation. The residuals, imbalances and/or the stability of variables of important to you (eg drag coefficient, pressure loss) are the way to judge convergence.

* Convergence difficulty on refining mesh - you are correct, it is caused by the reduction in dissipation in finer meshes. So that means you might have to use a few tricks to get the finer mesh to converge.

* Not converging beyond 1e-5 - this is an FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Thank you Glenn for your reply,

But why should I refine the mesh and get divergence problem with very fine mesh when with y+ .5 to 1 I can get the convergence , I mean what is the criteria for mesh refinement ?

And , I have used some output points to check the convergence like velocity , they get to a constant level and residuals goes to their minimum , but what it means when the residual goes to a number and keep constant or fluctuate ?

And please tell me what the physical time step means , does it define the numerical time step?

The criteria for mesh refinement is until the variables of interest to you have converged sufficiently to an accuracy you are happy to accept. Any convergence issues which come up you just have to figure out a way to resolve.

Your question about the convergence flat line is answered in the FAQ.

Physical time step is the psuedo-time step used to advance the equations. For further details see the software documentation.

Thanks Glenn for your reply,

I would appreciate if you tell me what is "imbalance in the domain" and how I can check it on the CFX ?

have a look at the imbalances under the solver manager. Get the available variables up by right clicking on a graph window and select imbalances.

Thank you for your reply,

I found them , but what is the imbalance in the domain? and I have read that it should be less than 1% , why?

It is the global conservation of that variable. The residual is the accuracy the equations are being solved in that specific control volume.

No, there is not a general rule that 1% is good enough. You need to do a sensitivity study on this to find the conservation tolerance your simulation requires.

I really appreciate your helps and useful comments,

I have some questions that needs the idea of CFD experts ,

I have simulated incompressible flow in a simple duct with different boundary conditions , turbulence and laminar , attached .
The Reynolds number is not so high,Re=3000-3500 then I used SST with y+<1 or laminar .

- is it correct to have the pressure inlet and mass flow outlet instead of mass flow inlet pressure outlet ? the profile of the velocity is different as the mass flow inlet imposes constant velocity profile at inlet ,
- at the Mass flow inlet BC , the profile of the velocity shows that the velocity is not maximum at the center far away from the inlet, is it correct .
- What is the exact procedure for the solving other variables when I set the pressure inlet at the boundary, is it zero gradient , is it more physical ?
- for the laminar condition , the velocity profile at the middle of the pipe is lower than some pints of the corner , is it physical ?

They are converged and mesh independent .

Thank you in advance

Sorry for the low quality picture ,
this might be better,

Thanks

1) Mass flow at inlet or outlet - put it where it best represents the flow you are modelling. You can correct in saying that by default it assumes a constant velocity across the section so that will require additional upstream space for the boundary layers to develop.

Your other questions really focus on what is important for you to model. If you are interested in the fully developed flow then you need to ensure your domain is long enough for the fully developed flow to form. That length will be different for a pressure and mass flow boundary (mass flow will be longer). And as for whether the laminar result is realistic - again, if the real flow is laminar then yes. If the eral flow is turbulent then no. CFD is about reproducing the results of the experiment, so you match the models to what happens in the experiment.

Thanks Glenn for your reply,

I am not really concerned about the fully developed as I am doing this as a pilot study for my final simulation, but as far as I know , the velocity should be maximum at the middle , but I see some results for mass flow inlet SST or Laminar , as I discussed before not conforms with this fact ,
And I have another question , should I get the flat velocity profile at the inlet with laminar flow and pressure inlet BC , or generally is it possible to have the flat profile at the inlet with the pressure inlet BC?

Thank you ,

If you start a flow with plug flow (ie constant velocity across the whole section) and allow it to develop into fully developed flow, have a think about how it progresses through the development. You will find that during the development of the flow you will get regions away from the centre which are the maximum flow.

The pressure inlet should allow a flow closer to fully developed.

Thanks Glenn

I really appreciate your comments as an expert .

My question is , how the flow develop such a way that has not maximum velocity at center? Because of the effect of the zero velocity at the wall and the viscous flow then as we go further from the walls we should have highest velocity , I am a little bit confused
And It seems not to be physical ?? Do we have some condition like this in experiment ?

Thank you

Have a think about it - the flow in the centre needs to go faster than the initial plug flow in the fully developed flow. So how does it "know" it needs to accelerate?

If the thought experiment does not explain it for you, do a simulation and have a look at how the flow evolves from plug flow to fully developed.

As it can be seen from the image ,Velocity in the core of the flow outside the boundary layer increases with increasing distance from entrance. This is due to the fact that through any cross section same amount of fluid flows, and boundary layer is growing.
It is exactly the mass flow inlet with inlet uniform velocity profile , but the way that flow develops by the numerical solution is different from what it is seen from the image.
I can not justify the numerical result that center line velocity is not maximum ,

:) The diagram you show is wrong. The person who drew that diagram does not understand the details of how fully developed flow forms.

You haven't thought about it yet - how does the flow in the middle accelerate? What is required to make it accelerate?

Here the reason that can accelerate the fluid is the effective area reduction because of the BL . And as the fluid outside the BL can be assumed inviscid then it should have a flat profile outside BL.
Then I do not understand the cause of non flat profile outside of the BL with the maximum velocity on the corner. I have seen an experimental result showing this issue.
Please refer me to any article that discusses this issue , I need to know about it.

Thanks

Hi again ,

I have attached the experimental result for flow profile development in a pipe.
Please let me know your idea about my previous post.

Thanks

Hi ,

I would appreciate if you can help me out,
As It can be seen from the experimental result(previous post image) , the velocity profile after the BL is somhow flat and in some points in the center a little higher than the corner outside of the BL.
But as previously discussed , if the mass flow inlet is set as BC then we do not see this profile , but after BL , on the corner is higher than the center .
But if we use Pressure inlet as BC then the profile is something that is expected like explained , before Fully developed length it is flat after BL and we can get to fully developed profile after considerable shorter length compared to mass flow inlet.
Then my question are ,
- is the Mass flow inlet a wrong BC because I do not see the correct velocity profile , or I am wrong in the theory or simulation?please explain for me.

The answer to this question is important for me and I hope you help me out.

Thank you in advance.

Do a simulation of flow in a laminar pipe, at say Re=500 (so well laminar) and have a look at how the flow develops.

In turbulent flows it is hard to see the details as it is lost in the turbulence, so the image you posted is not clear.