# Angular Velocity Ramp for Axial Turbine

 Register Blogs Members List Search Today's Posts Mark Forums Read

 March 15, 2013, 10:22 Angular Velocity Ramp for Axial Turbine #1 New Member   vinicius Join Date: Mar 2013 Posts: 4 Rep Power: 6 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.

 March 16, 2013, 05:57 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,336 Rep Power: 110 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?

March 17, 2013, 11:07
#3
New Member

vinicius
Join Date: Mar 2013
Posts: 4
Rep Power: 6
Quote:
 Originally Posted by ghorrocks 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.

 March 17, 2013, 18:26 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,336 Rep Power: 110 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

 March 18, 2013, 12:28 #5 New Member   vinicius Join Date: Mar 2013 Posts: 4 Rep Power: 6 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.

 March 19, 2013, 05:42 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,336 Rep Power: 110 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.

 March 21, 2013, 10:37 #7 New Member   vinicius Join Date: Mar 2013 Posts: 4 Rep Power: 6 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.

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post padmanathan FLUENT 0 May 4, 2011 07:18 vanni Main CFD Forum 1 May 18, 2009 11:03 vanni FLUENT 1 April 23, 2009 02:44 rr123 FLUENT 0 July 21, 2008 09:35 learning_never_ends FLUENT 0 June 30, 2008 17:04

All times are GMT -4. The time now is 23:03.