[Mfaizan]

Hi all,

Please suggest me the difference between Physical timescale, Local timescale factor and Auto timescale?

first I tried my cfd project with auto timescale, then local timescale factor and then physical timescale.

The problem I am having with physical timescale is that it is finishing before the suggested iterations. I set 1000 iterations but with physical timescale the solver stopped after 141 iterations. WHY? I do not understand. Please anyone know the reason then please reply to this post............Humble request.....

Thanks in advance

[Antanas]

Originally Posted by Mfaizan

Hi all,

Please suggest me the difference between Physical timescale, Local timescale factor and Auto timescale?

Physical timescale - you set fixed time scale to be used over the entire flow domain;

Auto timescale - CFX determines time step automatically based on the boundary conditions, flow conditions, physics, and domain geometry;

Local timescale factor - enables different time scales to be used in different regions of the calculation domain. The value you enter is a multiplier of a local element-based time scale.

Why don't you use CFX help?

Originally Posted by Mfaizan

The problem I am having with physical timescale is that it is finishing before the suggested iterations. I set 1000 iterations but with physical timescale the solver stopped after 141 iterations. WHY? I do not understand. Please anyone know the reason then please reply to this post............Humble request.....

Thanks in advance

It doesn't related to physical timescale. The solver finishes either when convergence criteria (residuals target, conservation target (imbalances)) are met or when max number of iterations are reached. Max number of iterations is just limiter. If solver finishes before max number of iteration then it means that your residuals became less than residual target and your imbalances are less than 1% (if you activated conservation target checkbox in solver control).

[Mfaizan]

Thanks Antanas,

What do u suggest that which timescale shud I use for my model.

I am modelling a supersonic convergent-divergent nozzle. The gas in nozzle is nitrogen with 1.4MPa total pressure and 550C total temperature inlet boundary condition.

I enclosed the nozzle in cylindrical surrounding domain filled with nitrogen gas too with opening boundary condition.

Please suggest if physical timescale is OK with my entire flow domain.

[Antanas]

Originally Posted by Mfaizan

Thanks Antanas,

What do u suggest that which timescale shud I use for my model.

I am modelling a supersonic convergent-divergent nozzle. The gas in nozzle is nitrogen with 1.4MPa total pressure and 550C total temperature inlet boundary condition.

I enclosed the nozzle in cylindrical surrounding domain filled with nitrogen gas too with opening boundary condition.

Please suggest if physical timescale is OK with my entire flow domain.

My suggestions:
1. Use auto-timescale.
2. Set appropriate initial distribution. It's more important IMO. You may use gas-dynamic functions for that.
3. Use Upwind scheme to get approximate solution.
4. Use results of step 3 as initial guess and set High Resolution scheme to get final results.

You may try to use dt = C * dl / (abs(u)-a), where C <= 1, dl - smallest mesh element dimension, u - characteristic streamwise velocity component, a - characteristic speed of sound.

[Mfaizan]

Thanks Antanas,

Such a comprehensive response.

Sure I would try as u instructed.

Cheers,