basics for unsteady simulation
 

hello, I'm going to run my first 3D unsteady simulation with fluent and I have some doubts with settings.. Usually I simulate wing profile, but this case is a rectangular chamber whit slot cut along over side and pulsed pressure imposed through connection tube (circular) at the bottom side, I'd like to know:

1) which is the more suitable turbulence model for this kind of situation (for steady simulation for profile usually I use SA..)

2)I'm interested to study the phase and amplitude difference between input pressure and exit slot pressure, so how much importance I should take for meshing (I do not care about boundary layer on wall for example, but is same important to have right refinement on wall?)

3)When I perform unsteady simulation is important to start from a steady solution or I can run directly with used defined function with unsteady pressure?

any other advace for unsteady settings is very appreciated.. bye

Re: basics for unsteady simulation
 

Dear Ernani,

this is a very good set of questions since unsteady CFD simulations are becoming more common place. I am actually working on one right now with Fluent which involves a very wide range of time scales, chamber filling (slow) conducting solids (slow), flow and heat transfer in narrow channels (fast), phase change to vapor (fast) etc.

So the overall issue to get a handle on are the spatial and temporal (time) scales of the problem. And how much of these we can reasonably simulate.

In an ideal world we would run the simulation though the exact same start-up sequence as the experiment and resolve all the time and space scales. Today this is impractical so we must:

1.use a turblence model (simplified combustion model, radiaton model etc)

2.reasonable meshes and time steps (actually all that counts is the Courant number....see below)

3.start-up from some reasonable place that captures the aspects of the problem of interest so we do not waste computer time on things like tank filling or opening valves, winding up rotors, etc

very interesting how your questions number out the same as my issues here ;-)

1. Most of the standard RANS turbulence models were not really tuned for unsteady simulations. That said they all can be applied to transient flows although they imply some "steadyness" in the flow. The real issue is whether the unsteadyness of interest to your problem and the unsteadyness of turbulence of your real experiement are well separated processes. If they are complex and interacting then you have to move to something like LES, DES, etc.

An example is the unsteady interaction of turbulent separated flow on a stalled wing with changes of angle of attack AOA. In the experiment of looking at lift (and/or drag) as a function of AOA there will be a hysterisis loop as one increases angle of attack to stall and then decreases. These loops of the dynamic AOA response change as one increases or decreases the rate of change of AOA. With a standard RANS model you will not capture most of this properly.

So look at your problem and decide or experiment with various turbulence models to see what you get...most people use SA or k-e versions for even very complex unsteady phenomena like flutter, rotor-stator interaction. I think a lot of this is since they are so stable and running transient already is a huge increase in complexity of the simulation.

2. You must resolve the features of interest with the mesh. Something on the order of 20 cells per feature is a good starting place. So say you have a sine wave then you have to get atleast 20 cells across it. Some call this N_lambda....or number per wave? Then you have to run a time step that maintains a reasonable Courant number. Cr should be 1 or less and this is the primary factor for accuracy. I have seen people who set-up a simulation with a certain mesh run it at a reasonable time step. Then refine the mesh, run at the same time step....and the results are garbage....why... Cr was too high...remember locally Cr = U/(dt/dx) ie physical velociy/numerical velocity based on info going one cell/timestep. This is your key to accuracy. There are books, papers, etc which show the behaviour of various schemes for various problems as a function of Cr. Check out Fletcher's book, Hirsch, Ferziger and Peric (chapter on unsteady problems and error control).

3. In terms of where to start the problem as I said above it would be nice to do the same start-up as the experiment but as a rule ONLY do as much of the transient as you NEED.

So for a wind tunnel doing one loop of aoa the start up is probably:

a. wind up the fan...maybe 1 minute b. steady out the flow in the tunnel maybe even temp...few minutes c. monitor static forces for steadyness...1 min d. begin aoa loop....30 s e. repeat d. f. top the equipemtn

all the numbers above are just guesses??? but you can see that an order or magnitude of the simulation could be wasted. Obviously f above is unnecessary since there is no influence on earlier events from later.

Of course if there is some developing cycle that you need then you may have to go through a couple of cycles from steady state. In turbo work this is usually several full revs. Try and see what is important. Here you also have to be careful off multiple solutions with different start-ups.

4. Other issues of note: always run 2nd order in time and space. You can use 1st order for the start-up if necessary and if it is not important. Be careful as well there are flags for getting the correct transient terms in Rhie Chow treatment. There is an rpsetvar for this but I forgot it now...check with support...or I can dig it out for you. Another issue is how to run transient: nita or iterative. Check the manual for guidelines on this. With iterative you want to get a couple of orders of residual reduction per time step but not waste your life on it. If you have to go to smaller time steps so convergence of the non-linear iterations is easier in say 5-10.

Ok that is lots to think about...I trust this is of help. Let us know how it goes.

Best Regards,

Bak_Flow

Re: basics for unsteady simulation
 

thank you very much for your advice... I will put it in action bye:)

Dear Bak_Flow,
I am interested in the phase change about water from liquid to vapor. I have done some investigation, it seems that VOF model in FLUENT software cannot simulate the phase change phenomenon, i wonder if there is a proper tool that can gain the phase change simulation.
Regards,
Bill

problem of the drag's convergence for a circular cylinder with a synthetic jet (udf)
 

please can you help me i'm runing an unsteady flow around a circular cylinder with a diameter 15 mm for a REYNOLDS number =150 .
first of all when i run this problem without a jet actutator i got DRAG coefficeint =1.45 and LIFT (max = 0.6 ) which is a little bit near to published results before.
but now i'm tryin to restart my calculation after introducing a jet actutator as an oscilatting orifice ic the cylinder using a user defined function ( velocity inlet )
/************************************************** ********************/
/* unsteady.c */
/* UDF for specifying a transient velocity profile boundary condition */
/************************************************** ********************/

#include "udf.h"

DEFINE_PROFILE(unsteady_velocity, thread, position)
{
face_t f;

begin_f_loop(f, thread)
{
real t = RP_Get_Real("flow-time");
F_PROFILE(f, thread, position) = 5.0*sin(10.*t);
}
end_f_loop(f, thread)
}

the grid is chown bellow in the attached file and also the non convergence of drag and lift coeefiecient :confused: .
the velocity inlet is 0.1460735 ms-1
walls
cylinder = stationnary wall .
the small part introduced in cavity of the cylinder is the synthetic jet moving with the sinusoidal velocity ( mentionned up (udf ))
i don't nkow what is the problem :'( i'm really stuck there :( .
i've used as descritisations schemes :
pressure -velocity coupling : simple
pressure : standrad
momentum : first order
please help meeeeeeee

What is the best way to check the unsteady simulation ?

The simulation I've studied on have 2,5 E-5 s of time step and 0,12 s of total time. The simulation has been running for 24 hours but just the half of the steps were completed. (there are 24000 steps completely).
I want to see whether the analysis is correct or not. What should I do ? Should I reduce the time step or total time ? Could you please give me information about this matter ?