CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Angular Velocity Ramp for Axial Turbine (http://www.cfd-online.com/Forums/cfx/114688-angular-velocity-ramp-axial-turbine.html)

viniciusgm March 15, 2013 10:22

Angular Velocity Ramp for Axial Turbine
 
Hi,

I am beginner in Ansys CFX, and I have problem to acheive to converge in a axial turbine 3D case. I am trying with a angular velocity ramp each 25 interation, but to do this manualy is bothering. So I would like to know if someone has some tips or a place that I can find a good manual that I can learn to do this.

Thank you for your attention.

ghorrocks March 16, 2013 05:57

What do you mean by "axial velocity ramp each 25 iterations"? Why are you doing this?

You could use a CEL expression to automatically link the axial velocity to iteration number but I cannot see why you would want to do this... maybe as a way to gently start an unstable simulation?

viniciusgm March 17, 2013 11:07

Quote:

Originally Posted by ghorrocks (Post 414351)
What do you mean by "axial velocity ramp each 25 iterations"? Why are you doing this?

You could use a CEL expression to automatically link the axial velocity to iteration number but I cannot see why you would want to do this... maybe as a way to gently start an unstable simulation?

---------------------------------------------------------------------

Exactly. The simulation is very unstable in the begin. I noted if the simulation begin without rotational velocity the simulation not diverge, in this way I don't have problem with overflow. But I need some way to make this rotational velocity ramp. I can't find good documentation that learn this process. Intuitively I tried build a rotational ramp with this expression: RotationalSpeed +Current Iteration Number*10[rev min^-1], once I defined the RotationalSpeed as zero for first interation. But this method is a little bit agressive. I need a method softer to avoid the overflow in the simulation.

Thank you for the help.

ghorrocks March 17, 2013 18:26

If your existing citer*10[rev min^-1] is too agressive then isn't the solution simply to reduce the coefficient, maybe citer*1[rev min^-1] or whatever works?

Note that this equation is unbounded so this simulation will never converge. You should put a limiter on it so it eventually reaches the speed to are trying to simulate. Maybe something like min(citer*10[rev min^-1],100[rev min^-1])... assuming 100rpm is your intended speed.

Have you tried all the normal ways of starting difficult simulations?
* Using an initial condition which better represents the flow.
* Using local time stepping
* Using a small time step to start off

viniciusgm March 18, 2013 12:28

The citer*1[rev min^-1] is a good start point, but I need a lot of interaton to stabilize my solution and achieve the design rotational speed. Maybe there is another way.

Yes, my equation is unbounded because I was only observing the residual. I did a test to verify the stability of my solution on each iteration.

I have tried all the normal ways, as you mentioned. In all these ways, I had problem with overflow.

I observed that the solution converge when my rotational speed is zero. So, I suspect that I should find a way to gradually increase the rotational speedy.

Now, I will modify acceleration ramp using some Expressions and User Functions, as suggested to me.

As soon as possible I will return to discuss if this method worked.

Thanks.

ghorrocks March 19, 2013 05:42

Of course ramping the speed like this causes its own convergence difficulties. It is not an ideal way of doing it.

A much preferable way is to have the impeller running at the constant full speed, and use the zero speed result as an initial condition. Use very small time steps to start the simulation, and maybe local time stepping instead.

What is unusual about this simulation to make it so unstable? Either this is a devilishly difficult flow, or you have an error in the setup.

viniciusgm March 21, 2013 10:37

I reviewed all my settings, and I used the converged zero rotational velocity solution as initial condition using very small time step. It worked!
Thanks for your attention.


All times are GMT -4. The time now is 05:20.