[urosgrivc]

I think that you must try to run it in stedy state.
that way you will get time averaged results of pressures and forces acting on a wing.
Than you can simply go to mechanical and import and aply these [time averaged] presures to your wing.->(one way FSI)
(quite simple and robust if you make the CFD simulation well enough)
-I do recomend independace studies->(mesh size, and domain size) must not influence your results.
What I meen by that is, let say your simulation has converged perfectly but you have an extremly corse mesh, than results are not good dispite that it has converged. (mesh influenced your results) it must not.
search the forum independance study or something like that.
-sst model is good for this tipe of simulation dont use k-epsilon alone as you need modeling in near wall zone.

If you would be doing a transient CFD than you should somehow make a transient FEM but than the shape changes and the flow changes so that is a twoway analisis)
With two way coupling you could predict the frequency of wing woble becouse of air acting on it (but it is wery complex and you probably dont need it)

I think that you should be able to converge the solution in steady state becouse you have 5deg AOE (no seperation). If you would go abbove 10deg (depends which naca profile you have) then things get wery complicated and computationaly time consuming (transient), I would not recomend that to you yet.
It is interesting but predicting airfoil stall acuratley is much harder than it looks (becouse of flow seperation and transient efects).
But you are not near stall zone so you are good.

[ghorrocks]

I think that you must try to run it in stedy state.
that way you will get time averaged results

No, this is wrong. A steady state simulation does not give you time averaged results. If the actual flow is transient then it won't converge. You only use a steady state simulation when the actual flow is steady state.

Note that the turbulence model will return a time averaged result, as that is the result of the Reynolds/Fauve averaging. But the velocity, pressure and temperature fields are not time averaged.

dont use k-epsilon alone as you need modeling in near wall zone.

We don't know for this case whether wall functions are a problem or not. So I would not write off wall functions out of hand. However, if you use the SST model it can automatically handle wall functions and integration to the wall, so it can handle both cases.

[urosgrivc]

yes I ment the RANS aproach.
and thank you for the other words.

This is in general now it does not apply to this wing simulation->..:
I thought that temperature field is time averaged as it is turbulence dependant isnt it,
(or is it just the velocity profile near wall that is responsible to obtain heat transfer coefficient and temperature profile near wals?).

[ghorrocks]

Sorry, let me more precise in my terminology. The additions are in CAPITAL LETTERS:

A steady state simulation does not give you time averaged results OF THE SIMULATION VARIABLES (U,V,W,P ETC). IT GIVES YOU THE TIME AVERAGED RESULT OF THE TURBULENT FLUCTUATIONS. If the SIMULATION VARIABLES is transient then it won't converge. You only use a steady state simulation when the SIMULATION VARIABLES ARE steady state.

***********

So the simulation variables u,v,w,temperature/enthalpy are Reynolds Averaged from the turbulent fluctuations. But for a steady state simulation u, v, w or temperature/enthalpy must not vary with time.

I don't know if that makes things any clearer

And to answer you direct question: yes, the temperature/enthalpy equation is Reynolds Averaged.

[frossi]

So I ran a steady state simulation. First, a ran a one-way FSI steady state for the 5 deg angle of attack. It converged with a RMS tolerance of 1E-6. But the results were very similar to the transient results. Is that normal?

Then, I ran a one-way FSI steady state for the same wing at 35 deg angle of attack. The simulation converged with a tolerance of 1E-5 (I didn't conduct more tolerance independence studies, I just wanted to see reasonable convergence). How is this possible? What you guys said before made perfect sense, because the flow separation is a transient effect. So how could I get a steady convergence with such a high angle of attack? I attached an image from CFX post. So should I always try a steady state first (and keep it in case it works), even though the phenomenon I want to observe is clearly transient?

Thank you

[ghorrocks]

If the steady state simulation converges then you are fine.

Steady state similar to transient? If the transient simulation settles down to a steady state configuration, then that final configuration should be the same as if you had done a steady state simulation.

Separation transient? Yes, it should be. It is possible it is not but that is unusual. Reasons why a transient simulation can fail to show expected transient behaviour include:
* Mesh too coarse
* Using first order advection differencing (need second order or higher)
* Using first order time differencing (need second order)
* Inlet turbulence conditions have too high turbulence level.
* These are the main ones, there are others.

[urosgrivc]

Try a diferent mesh size with fine inflation layers y+=1 at AOE=35°.
Do you get same results for lift and drag?
Becouse you have set vectors to equaly spaced we dont have any idea of what your mesh is like.

Becouse you have very high speed air flow, your mesh near walls will have to be extremly thin to achive y+ of 1 as wall functions are not aplicable for your
35aoe flow - wall functions do not predict flow seperation or high inverse presure gradients corectly.

I bet it is a mesh size problem. just refine it a and try again. As I have vriten in previous posts mesh size might fool you into thinking you have correct results - corse mesh converges weel as it just lefts out most of important data of the flow.

Is this a 2D problem now? werent you talking about 3D one? how are you going to make a usefull 2D FSI?

What do you meen by (First, a ran a one-way FSI steady state for the 5 deg angle of attack) Are you coupling analisis together or what .
Just do a simple CFD first (solution in mechanical is nothing compred to CFD solution).

[ghorrocks]

Becouse you have very high speed air flow, your mesh near walls will have to be extremly thin to achive y+ of 1 as wall functions are not aplicable for your
35aoe flow - wall functions do not predict flow seperation or high inverse presure gradients corectly.

Are you sure this is correct? At AOA=35 deg you get very clear separation points at the leading and trailing edges, as his image shows. This is not a borderline separation which boundary layer effects are important, this AOA is so far into separation that it is not required. Wall functions will model obvious separation points like this just fine. I suspect that you will get the separation just fine with wall functions and a much coarser mesh.

Your comments seem to apply to cases where the airfoil is only just separating (for instance AOA=10 degrees), and full integration of the boundary layer is required there to correctly predict the separation.

I am no expert in airfoil modelling so if I am wrong please tell me why. But from what I know I see no reason to insist on integration to the wall in this case.

[urosgrivc]

Yes I agree totaly .
35 is quite past stall point
And I have never tried Angles of attack higher than 25 so I dont know what happens than either.
But it it was suprisingly hard to get usefull lift and drag data at (9-18)deg airfol in my case.

My prevoius AOEs are ment AOAs, (sory but english is not my first language)

[frossi]

it is still a 3D problem. The picture you saw in my previous post is just a plane in the fluid domain that I used to show the turbulence.

urosgrivc,

What do you meen by (First, a ran a one-way FSI steady state for the 5 deg angle of attack) Are you coupling analisis together or what .

I am doing a CFX coupled with a static structural. So, once the CFX solver is done, I import the pressure from CFX to Mechanical and compute the stress on the wing.



urosgrivc, when you say

Do you get same results for lift and drag?

I believe you refer to CFX POST results. I am computing lift and drag from the CFX POST "calculator" tab, assuming x-force on the wing as drag, and y-force as lift (see picture). For what concerns moment, am I correct if I assume the function "torque" to be the moment of the wing about an axis? What I can't figure out is how to calculate moment about a specified moment center on my wing root axis. In fact, I want to calculate moment of the wing about the quarter chord of the wing root, but I can't find any options to specify the moment center. Can you guys please tell me how to do this?

I used 35 AOA 35 deg because I wanted to observe separation. Surely this was an exageration. I want to perfect my technique, and I saw you guys mentioned wall functions and y+. I found on different sources that y+ is a non-dimensional quantity used to capture near-wall boundary layer phenomena. But what is y+ exactly? What is the difference between y+ and wall functions? Also, where can I visualize the value of my y+? What is the ideal y+ value?

[ghorrocks]

y+ is explained in the CFX documentation. Also a good turbulence modelling textbook like "Turbulence Modelling for CFD" by Wilcox is highly recommended.

[urosgrivc]

there is some usefull data about Y+ and inflation layers here also;

http://www.computationalfluiddynamic...hing-in-ansys/
http://www.computationalfluiddynamic...oundary-layer/
http://www.simutechgroup.com/CFD/cfd-tips-do-dont.html

and you can find lots of data here on the forum asveal

You are able to evaluate torque in cfx post.
If your global cordinate frame is already in the center where you want it to be, than just go to Function calculator and use the torque function.
If you want to move the center to where you want it, you can make a new coordinate frame and than evaluate torque around this one not the global one.

With (same results); I ment if you refine the mesh and solve again if results of lift and drag, torque, etc. stay the same?
or they change? If these change a lot than your results are not mesh independant and are useles so you must change the mesh and try agian till you reach mesh independancy.

[hwangpo]

Originally Posted by ghorrocks

This is not correct for CFX for most simulations. CFX does not require CFL = ~1. This requirement applies to explicit solvers and CFX is implicit. The approaches I described in the previous post are applicable to CFX.

(Small note: the only exception I am aware of in CFX is surface tension modelling. In CFX this behaves in an explicit manner and does require Courant/CFL =~1. But this only applies to surface tension modelling)

Courant number and CFL are not very useful in CFX as it is not a good predictor of whether the time step will be numerically stable or accurate. Therefore I do not recommend using it.

By 'surface tension modelling' do you mean surface-tension-dominant flows? OR all of the problems including surface tension?

thanks.

[ghorrocks]

I meant simulations where the surface tension force has a significant effect on the flow, and is directly modelled using a free surface model. So this is things like inkjet printer droplet ejection, drops on surfaces, spray breakup and things like that.

It does not apply to eularian or lagrangian particle tracking, or particle based spray breakup models.

[hwangpo]

Originally Posted by ghorrocks

I meant simulations where the surface tension force has a significant effect on the flow, and is directly modelled using a free surface model. So this is things like inkjet printer droplet ejection, drops on surfaces, spray breakup and things like that.

It does not apply to eularian or lagrangian particle tracking, or particle based spray breakup models.

Thank you. I'm working on some projects of air-water flow where the surface tension may be significant. By the way, considering the air as ideal gas maybe need the timestep far smaller than incompressible one to converge, at least in my case this is true.

[ghorrocks]

If the compressible gas is significant then yes, it is likely to reduce the required time step compared to an incompressible simulation.

[Goenitz]

Originally Posted by ghorrocks

If the compressible gas is significant then yes, it is likely to reduce the required time step compared to an incompressible simulation.

can we set the time step and simulation time in CFX?

"For a transient simulation, the multi-field timestep and time duration are also used by CFX-Solver; that
is, you cannot specify the CFX Time Steps and Time Duration independently"

But I cannot find any of the option but a convergence residual criteria or wall clock time.

[ghorrocks]

Yes, of course you can. That is very basic stuff. It is in the "analysis type" setup in CFX-Pre.

Note that for a coupled simulation you need to have the CFD and FEA (or whatever you are coupling to) solvers work together, so this will place some restrictions on time stepping. But for stand-alone CFD simulations you can set what ever time step and simulation time you like.

[Goenitz]

Originally Posted by ghorrocks

Yes, of course you can. That is very basic stuff. It is in the "analysis type" setup in CFX-Pre.

Note that for a coupled simulation you need to have the CFD and FEA (or whatever you are coupling to) solvers work together, so this will place some restrictions on time stepping. But for stand-alone CFD simulations you can set what ever time step and simulation time you like.

Really excuse me sir for the trouble. Actually, has been using fluent lately, so totally forgot that those time settings are declared in the Analysis Type.

[Martin_Sz]

monitors which u define in solver is the best way to estimate total time and tipe step size ( if u plot imbalances )