Dear anyone who can help,

I am currently using cfx 5.7, and modelling laminar flow in a 2D domain over a bluff body. I run the simulation at a timestep of 0.05 seconds for about 50 seconds real time. The solution is quite poor but however the velocity and pressure profile looks OK.

Using the same setup as above, Here's the problem when I decrease the timestep to 0.001 sec. the solution becomes weird, at about 10 sec of real time the solution is fine, but after that I seem to get massive recirculation at the upward stream of the bluff body and near the inlet and also at the outlet. Looking at the pressure profile, the pressure is sectioned into rectanglar shapes of the domain and goes from a positive pressure to a negative or vice versa, or sometimes negative pressure throughout.

Please could someone help me on this problem, is it my setup, global initialisation etc?

James

James,

How did you specify your inlet and outlet boundary conditions. What fluid definition did you use?

-Robin

Hi Robin,

Inlet conditions; 8 m/s, normal to the boundary, Outlet; Static pressure, relative 0 Pa,

Ideal Gas @ temperature 293 K; isothermal. Fluid domain reference pressure: 101325 Pa

James

James,

How long is your domain and your bluff body?

-Robin

Robin,

Domain is 250 m Bluff body 31 m

James

Hi James,

What you are seeing are probably pressure waves. Note that the pressure variable is a gauge pressure, relative to the domain pressure you specified. So a negative pressure is just below your reference pressure.

First of all, I think your timestep is way too small, but you may have a reason for this. Assuming the temperature is around 20 C, the speed of sound is about 343 [m/s]. That means it will take .73 [s] for a pressure wave to move across your domain, or 730 timesteps! In short, you are definitely running with a timestep small enough to resolve pressure waves. The wave propegation may not be exactly correct, since you are probably not solving the total energy equation.

The pressure waves arise from your velocity specified boundary because the mass flow and density of fluid at the boundary are responding to the back pressure. Air Ideal Gas will still have a density that depends on pressure, even though you may have specified the energy as isothermal. You might have fewer problems if you were to change the inlet to a total pressure instead. You could specify the total pressure to be 1/2*Density*Velocity^2 and set your outlet pressure to zero. Or you could just change your outlet to a mass flow specification.

At 8 m/s though, I would recommend using "Air at 25 C" or creating your own general fluid. There are no compressibility effects and you can run with a constant density. This will get rid of most of your problems.

As for your initial guess, I recommend solving a steady state solution first, then restarting the transient from there.

Regards, Robin

Robin,

Thankyou for your response, I will let you know how I get on!

Regards

James

Robin, Is there a rule of tumb in terms of time steps for RANS models ? like using the SST, if a domain is 1m long and the fluid is 1m/s.

Do you mean URANS (ie transient)? For transient simulations, the timestep will depend on how rapidly the solution is changing. Generally, if your timestep is small enough, you can converge the linear solution within 3 coefficient loops.

For a steady state simulation you should use as big a timestep as you can get away with. Don't be shy. A large timestep will get you through the startup transients quickly. If there are sharp variations in the residuals later, you can reduce the timestep to drive the residuals in.

A good check of the timestep is the write a backup file and create streamlines from an inlet colored by time. A big timestep would be 10x the lenght averaged time on the streamlines, a small timestep would be 1/10th of the average time.

Also have a look at the tech tip on the CFX Community Site titled "Monitoring and Improving Convergence" (http://www-waterloo.ansys.com/cfxcom...onvergence.htm).

Regards, Robin