[hamidciv]

hi every one
i run model as shown, I've analyzed within 4 days, finally today finished, unfortunately my result have high error with experimental data, could any one please give me advice
i used body sizing with element size=0.5 and soft behavior, then i used inflation that shown red follow(first layer heght=0.1, maximum layer=60)
in cfx pre i used k-epsilon turbulence model.
my flow as shown follow before spillway and on spillway have wawe , i dont know cause this wave?
please help me that you order Where is the problem?
i very confused.
thanks in advance

[hamidciv]

no body advise me?

[ghorrocks]

Patience, patience. You only posted the original question 3 hours ago. Don't forget this is a global forum, so people are in different time zones to you and only look at the forum from time to time.

Your upstream boundary condition is almost certainly wrong. That is causing the weirdness in the upper reservoir.

Your mesh in the runner is bad. There does not appear to be any inflation down the runner.

But really your question is a FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

[hamidciv]

hi dear glenn
your order is quite Correct , i opologize For my hasty, what your mean of inflation down in my mesh model? if your possible please explain me and any suggestion.
thanks in advance
best regards

[ghorrocks]

Please post an image of your geometry and boundary conditions and your CCL file.

Your second image shows your mesh. The inflation stops in the runner. You will want inflation in the runner section.

[hamidciv]

dear glenn , tahnks a lot for spending time for me
i sent ccl file and geometry & mesh& boundary condition.
upon your order i have changed my mesh and turbulence model(sst) , and again starting to run, if your possible please check ccl file for any problem because i used The same boundary condition for new run.
thanks in advance

[ghorrocks]

Your mesh still does not have inflation layers in the runner.

I did not say to use SST, but now you mention it that is a superior model in most respects so that is a good move.

having a look at your CCL:
* You are defining a surface tension coefficient, but you do not appear to have activated the surface tension model. You will want to make sure surface tension is off. Surface tension is not going to be significant and it will cause convergence difficulties.
* This is a transient simulation. Are you sure you are running it for long enough for a steady state to be established?
* You are not modelling this as a homogeneous multiphase model. Is this intentional?
* Are you sure your initial condition is good? If your initial condition is not good then it is better to just start with everything stationary.
* You are using CFX V14. The current version is V16. You should upgrade to the current version.

[hamidciv]

hi dear glenn
thanks for good suggestion
unfortunately i forget activate surface tension model,but upon your order with considering convergence difficult In total off surface tesnsion as you mentioned.
yes i using homogeneous multiphase model because i modeling free surface that consist water & air.
for establish steady state , i considered total time 15s , I think that is enough((in inlet i have depth=7m, velocity=1.5, my length model is about 100 m), if your think is not enough please express your opininion.
for initial condition i in time=0 assumed my voulume Filled the air , water=0, i considered u in velocity components the same of normal speed.
In your opinion what kind of mesh i used?
have another question for you, The size of the previous model that i runned about 100 gb, whether i can for prevent of fulling hard system , in any stage that i stopped running and i go to the Target file and delete it?
thanks a lot for help me
best regards

[ghorrocks]

Only activate surface tension if it plays a significant role in the physics. At the scale of a reservoir spillway it will not play a significant role so disable it.

You misread my comment on homogeneous multiphase - you are NOT doing a homogeneous multiphase model. Homogeneous is a much simpler model and you should use it if it is applicable to your physics. If the water stays as a distinct interface and foam, spray or bubbles are insignificant then use the homogeneous model.

I cannot say if 15s is long enough. Have a look at your results and see if they are still evolving in time.

I do not understand your comment about your initial velocity condition.

An inflation mesh or a structured mesh will be best in the spillway as the water is likely to exist in a thin section at the bottom.

CFX has lots of options to make the results file smaller. Have a look at the output tab.

[hamidciv]

very thanks for Follow my problem and spending time for me
thanks for hint, i checked hydraulic parameters per time, your order is correct, my flow is unsteday.
i sent one image of initial condition if your possible look at it, i have velocity and depth water in inlet , i put u in initial condition equal to normal speed in inlet boundary condition,whether this is correct? i dont know amount v&w.
i finally meshed model as shown follow with tetrahedra.
your mean of low size in output tab is selected variables or other way is exist taht main effect in lower size because size runnes is rellay high.
many thanks dear glenn

[PeMo]

Just a quick comment about your initial conditions. It seems to me that your initial conditions are poorly defined. You set a constant velocity, which will splash against the wall of your upper reservoir, flowing back and will be reflected at your inlet BC. As Glenn mentioned, I would start with a stationary flow field and let the flow develop

[hamidciv]

dear peter thanks for comment, if your possible please express me your mean of stationary flow field, unfortunately i dont understand? are you mean steady state? as your mentioned upon experimental data unfortunately i have not other data in model , only i have depth and velocity water in inlet.
thanks

[ghorrocks]

A stationary flow is where velocity = zero. Do not use the U=1.51m/s you have defined and make it U=0.

If you can do a hex mesh rather than a tet mesh that will also help a lot.

[hamidciv]

hi dear glenn
i apply all your order and now i doing run, i have runing with u=1.51, but upon your order i stopped my run and i considered u=0, unfortunately i every doing , i facing error, in during running in Timestepping Information I saw RMS Courant Number & max courant number equal to zero that due put u=0 , now What can I do? i also fine time steps but dont solve error.
thanks again

[ghorrocks]

You cannot tell anything from the workbench error messages. The useful error messages are in the output file from the CFX solver. Please post the error message from the output file.

[hamidciv]

dear glenn, i attached images of errors in cfx solver manager, that is notable Coefficient loop iteration go to 2 and than return to 1.
thanks a lot

[ghorrocks]

As I said, it is the .out file which is useful. You have not included that.

But I think I can see you have a floating point error. This is a FAQ: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

[hamidciv]

dear glenn
as your said i sent image if error in cfx solver in during running, also i read faq that your attached, in your opininion upon faq i using single phase, or using upwind in advection scheme for generating initial condition ,unfortunately i dont underestand where is the main problem, why i when u=0 this error happen?
thanks a lot

[ghorrocks]

There is something in your model which makes the initial condition you are specifying numerically unstable. We cannot tell you what it is without more detail of what you are modelling and how the error came about.

[hamidciv]

ok , thanks a lot dear glenn, i considered different initial condition and i expressed result in here, if my problem dont solved, i bothering again.
many thanks dear glenn