[mejahan]

Dear experts,

I have some questions and would be gratefuller if you can answer them.
I am simulating a 25mmD internal flow using CFX with SST. As I have read some posts and the CFX manual, low Reynolds number turbulence models use automatic wall treatment in which is y+ insensitive and give the user more freedom on y+ setup. But I still see some posts that recommend y+ of 1 or 2. Can you please let me know your comment.
And I have plotted the eddy viscosity ratio in post.P, but I do not see the transition of the Eddy.V from low to high in the boundary layer, but rather I see a constant contour of this variable along the wall and the central flow, with minimum value close to zero. And the maximum value for Eddy viscosity ration is less than 1, I do not know why !!
Set ups: The y+ is less than 1 and the Re in around 6000, but this is a transient simulation that Re changes with time. Thank you for your time in advance.

[evcelica]

What are your inlet conditions? What eddy viscosity ratio did you define there? Did your flow have enough length for your flow to become developed?

[mejahan]

Hi,
I have used pressure inlet with 2D inlet length to have turbulent developed profile, eddy viscosity ratio with eddy viscosity to dynamic viscosity.

[ghorrocks]

automatic wall treatment in which is y+ insensitive

That is mixing the message up quite a bit. A better way of putting it would be "automatic wall treatment is applicable over a wider range of y+". But it will be sensitive over y+ ranges due to normal mesh size sensitivity.

[mejahan]

Hi Glenn,

Thank you for your reply. You are right it is essential to setup y+ normal to wall that first mesh falls into the viscous sublayer in order to model this region.
But still I could not resolve the problem about the eddy viscosity, it is still very low.
I used pressure inlet and velocity outlet with inlet and outlet lengths. SST RANS model, with zero gradient turbulence model at inlet. And my time step is 0.001s for transient solution.
And please let me know your comment on time stem setup in SST RANS model for transient solution, is there any consideration for time step setup?

Thank you for your time in advance.

[ghorrocks]

You are right it is essential to setup y+ normal to wall that first mesh falls into the viscous sublayer in order to model this region.

No, that is not what I am saying at all. I am saying the automatic wall function approach is applicable from y+<1 to large y+, unlike normal wall functions which are only applicable for y+>11 and integration to the wall which is only applicable for y+<5 (ish). Whether you need the first mesh in the viscous sublayer will depend on the conditions you are modelling - it is not always required.

If the eddy viscosity ratio is <1 then it means your flow is not very turbulent. If you know the flow is turbulent then are you sure you have set your model up correctly?

The best way to set the time step for most cases is to use adaptive time stepping, homing in on 3-5 coeff loops per iteration. Make sure the max and min allowable time step size are wide enough that you never reach them.

[mejahan]

Dear Glenn,



Let me offer my appreciation for your kind and useful reply. Your comments sometimes provide me a huge help.


Let me explain the numerical and BC set up then I will ask you my questions.
It is a 25mm pipe with a fixed valve at center with inlet(5R) and outlet length(17R), the mass flow rate changes with time from zero to maximum(inlet u=1m/s, Re=7000 at maximum) then zero again within the time period of 0.300s. Then I expect to have turbulent flow and detect eddy viscosity ratio (EVR) larger than 10 at maximum flow. The BC is Pressure inlet (zero gradient for momentum and turbulent) with mass flow outlet and SST turbulence model.
It converged well at steady state (U=1m/s) and I have checked the y+ and mesh generation at PP and it showed acceptable EVR range more than 10 at the center of the pipe and after the valve where there are strong recirculation zones. I gradually reduced the physical time step from 0.1 to 0.00001 and I see no oscillation in the Residuals and control points.
But when I run the transient sinusoidal flow (dt=0.001s and the residuals meeting the requirement (RMS<1e-5)), I see no eddy viscosity at the maximum flow when Re is close to 7000(opposed to SS solution). However, the profile of the velocity shows a turbulent fully developed profile at the inlet and outlet at maximum flow.
I have checked other configurations of the BC, such as Velocity inlet (profile and uniform with low turbulence intensity) with pressure outlet. And I see the same problem in EVR.
As you mentioned, it seems that the solver is not simulating a turbulent flow. I have to say that ran a laminar simulation with the same numerical setups and to my surprise, I see not considerable differences in the profile of the velocity and shear stress at maximum flow downstream of the valve.
And someone(not very expert in CFD) told me that time step of 0.001 is too large to capture the turbulent flow, but I saw turbulent flow at my steady state simulation(dt=0.1) with acceptable EVR. Please let me know you comment about this as well.
Something that I suspect is the time period of 0.15 to reach the maximum flow from zero. Maybe the flow does not have enough time to develop the turbulent flow. But in this case the unanswered question is that I capture the fully developed turbulent velocity profile at maximum flow at inlet where I set pressure BC.



I really appreciate your time for reading my post and I am looking forward to hearing your comments.

Thank you,
Mehdi

[ghorrocks]

But when I run the transient sinusoidal flow (dt=0.001s and the residuals meeting the requirement (RMS<1e-5))

Where did the dt=0.001s come from? Did you analysis to determine it? Or was it a guess? The most common newbie mistake is to use too large a time step and that smears the flow details. You should do a sensitivity analysis to determine the time step size, or use adaptive time stepping homing in on 3-5 coeff loops per iteration.

but I saw turbulent flow at my steady state simulation(dt=0.1)

Time in steady state simulations is really psuedo-time. It is not a real time, just an acceleration factor for convergence. Use it a very rough guide only.

Maybe the flow does not have enough time to develop the turbulent flow.

Yes, this is possible. Have a look at the turbulent viscosity ratio versus time and see if it is still building up.

There is a general FAQ on simulation accuracy. Have you read it? http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

[mejahan]

Dear Glenn,

Many thanks for your time and useful comments.

After reading your comments I arranged two separate simulations. One with the same time period of time (0.300s) but with adaptive time stepping as you mentioned. It takes so long sometimes for the solver to advance in time but I am waiting for the results. And another run for increased time period to 1s, to see if the problem of the low eddy viscosity is about the time that the flow is developing to turbulent flow.
As for your comment about the eddy viscosity with time during the simulation, I have assessed this aspect and what I see is that eddy viscosity ration is high at the beginning of the period when the velocity is very low, because of the eddies remaining from the previous period simulation (it is a periodic simulation). But as the simulation advances and velocity increases, these eddies are washed out and EVR decreases to very low numbers close to zero, even at the maximum flow when the Re=7000. During the deceleration phase again because of the recirculation zones and vortex shedding development, I see EVR is increasing again. I am monitoring the control points at different locations of the domain regarding this value for the Adaptive time stepping simulation and see the same results so far (I am not in the maximum flow yet).
But again another question is that how I can have turbulent fully developed velocity profile at maximum flow but zero eddy viscosity, and I see the same velocity profile even when the solver was set to laminar flow.

I would be grateful if you let me know your comments.

Thank you,

[ghorrocks]

If the adaptive time stepping model is running much slower than your original model that suggests your original transient model had time steps which are far too large. That means the results it gave you are rubbish and should be ignored.

[mejahan]

Dear Glenn,

Thank you for your comment.
Even results from the adaptive time stepping showed that the eddy viscosity ratio is very low at the maximum flow (Tperiod=0.3s, UmaxIn=1m/s). I arranged another run with extending the time of the period to 1s and still the EVR is low but better than lower period. Small eddies from the previous period are washed out and after peak flow during the deceleration these eddies begin to appear because of the vortices and separation zones, but at peak flow EVR is less than 1 that shows the flow does not develop the turbulent flow. And despite high Reynolds number=7000 at peak, flow shows almost laminar behavior at this point, because at the steady state solution flow is completely turbulent with EVR>10 in some points, and results from the laminar setup, does not show much of difference at peak flow( the discrepancies in viscous shear stress and somehow velocity vectors are not considerable.
Now the question is whether this behavior is physical or there is something wrong about the BC or numerical setup.
As turbulent intensity and velocity profile are unknown at the inlet, I am using pressure inlet with zero gradient for turbulent and momentum, and the turbulent solver is high resolution not first order. In addition, I need to have fully developed velocity profile at inlet and it is the best choice to have pressure inlet BC.
I would appreciate if you let me know your comments and suggestions.

Thank you,

[ghorrocks]

Have you read the FAQ I posted in #8? It talks about the accuracy issues you should consider.

Also you have not given much information about whether your transient run simply has not had time to build up to a steady state value or not. Have a look at the EVR versus time. Is it increasing? Then if you ran it longer with a constant flow it should increase - and this should match the steady state run you did before.

Also your choice of zero gradient for turbulence inlet boundary will mean that the flow is very slow to establish. This will slow it down even more. It will be faster if you put a pipe upstream to allow the flow to develop as modelled, with a simple fixed value of turbulence at the inlet.

[mejahan]

Dear Glenn,

Thank you for your comments.
I have read the FAQ in simulation accuracy you posted. Thank you, it was useful. I have done sensitivity analysis for mesh and y+, time step, temporal discretization (first order and high resolution), and they are working fine with my simulation.
I have done the steady state simulation (the same velocity as maximum flow velocity for pulsatile flow) to see whether it gives me acceptable eddy viscosity values for this Reynolds number. But I am modeling pulsatile flow and steady state in not my favor. However, flow does not show much of turbulent behavior at maximum flow in pulsatile flow. I was wondering to see whether it is physical and expected or I should work on the modeling setups.
About your comment on pressure inlet, I have used mass flow inlet but I have to specify the turbulence specifications at the inlet in which are unknown. And by setting the inlet to mass flow, I have to use a longer inlet length to let the flow develop the fully develop turbulent flow profile of velocity which in not favorable. In addition, the turbulence specification is changing by time the same way as mass flow and velocity do, and I could not find any value for them in literature.
Another question that I have is that whether I can set up momentum and turbulence specification in inlet with pressure inlet, because the software gives me a warning message in CFX-Pre to change them to zero gradient. And if I can do it, does it give me physical results.

I would be grateful if you let me know your comments. And please let me know if you have any question in mind.

Thank you,

[ghorrocks]

You cannot define momentum on an inlet pressure boundary. The momentum is calculated by the solver. But you can define the scalar variables of the fluid at the inlet, so that is temperature, turbulence etc.

[mejahan]

Dear Glenn,

Thank you for your reply.