Hi

i have to carry out a transient simulation on CFX ,i think that the CFX code use Implicite scheme ,so the stability is sure.(for the explicite schemes the Courant number should be aroud 1 or less).but to be sure to kept the transient features of the flow what is the suitible courant number on CFX?,does 10 good.

thanks

Hi,

You are correct in saying CFX is an implicit code and therefore does not have a Courant Number stability limit. However, to get accurate resolution of the time behaviour of a flow (and also for numerical stability reasons) you need to have a timestep small enough to resolve the relevant details.

The size of this timestep is flow dependant so you will have to do your own sensitivity analysis.

Regards, Glenn Horrocks

Hi Glenn

it's been a while.but how could i do this''own sensitivity analysis'',i'm carrying a turbomachinery flow simulation using K_eps ,on the help they advice a timestep of (0.1 to 1 / rotational spped),now this range of timestep is for steady states or it could be generalized to unsteady ones?.

thanks

Hi Amine,

The Courant number tells you nothing about the stability or variation of the flow around a control volume. For instance, a high speed steady flow can have a very high courant number, but not change at all.

The residuals, however, do tell you how the flow is changing. Therefore, if you pick a timestep that requires fewer (say 1 to 5) coefficient loops to converge within a timestep, you should be able to resolve the features of interest.

The auto-timestepping feature will allow you to do this. You can set the target min/max number of coefficient loops and the solver will adjust the timestep to acheive this. If you would prefer to use a constant timestep for your run, try running a case with the auto-timestepping on to find the optimal timestep, then re-run the case with your optimum.

-CycLone

Hi CycLone & Glenn

If you guys do not help beginners like myself, we will get no where. I want to run a simple incompressible flow through a plane channel with periodic boundaries. How can I calculate pressure drop between inlet and outlet of the channel. Thanks

Hi Ahmed,

This looks like a new thread. Please post it separately in the future.

As for your question, you can calculate the pressure drop by writing an expression in Post:

delta Pt = massFlowAve(Total Pressure)@outlet - massFlowAve(Total Pressure)@inlet

or

delta Ps = areaAve(Pressure)@outlet - areaAve(Pressure)@inlet

If your channel is periodic in the flow direction, you'll need to set it up with a periodic interface between your inlet and outlet and on the interface specify either the target mass flow rate or the pressure drop.

-CycLone

P.S. I'm assuming English is not your first language. Your statement "If you guys do not help beginners like myself, we will get no where." in English comes across as a demand for help and may be interpreted negatively since the forum is public and nobody has a responsibility to respond to posts. I'm assuming that this was not your intent, because Glenn and I, along with many other forum participants, regularly help people such as yourself. What I think you meant to say is"If it were not for the help you guys provide beginners like myself, we would get nowhere."

Hi Cyclone

Thanks for your help. You are right English is not my first language and I was not demanding you to help me. It was only a humble request.

Pressure drop that we are suppose to specify for a periodic boundary, is it a static pressure or total pressure? Thank you again. Sorry about the terrible English.

Ahmed

Hi Ahmed,

The pressure rise is a static pressure. What you are changing is essentially the reference pressure level.

-CycLone

Thank you

Ahmed

Hi guys,

I think I may have to send it into new thread but it has a sound relation with the topic in thread. Please tell me what is Courant number. I do appologize since I am an Electronics guy and I am confronting with this term for my project.

Regards

[mohamad3564]

Hello

I simulate multiphase flow by ANSYS CFX. I used o.1 for time step. How can I know about stability? can I check it with the courant number ?

[ghorrocks]

What type of stability are you referring to? Also, what about accuracy?

[mohamad3564]

Actually I have validated my results with experimental data but I want to bring some reason in the paper that the time step with value of 0.1 is acceptable. can I say this time step is appropriate for simulation by courant number= 0.6.

Best regards.

[ghorrocks]

This very thread explains why courant number is not relevant to CFX so no, you cannot justify anything based on that.

To justify your time step you need to do a time step sensitivity study where you run a range of timesteps and show that the result has converged to an accuracy you are happy with.