# convergence rate with steady state simulations

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

July 4, 2017, 04:39
convergence rate with steady state simulations
#1
Member

Join Date: Jun 2017
Posts: 39
Rep Power: 5
Hi,

I know this might be discussed previously, and am sorry to bring this up again, but I could not solve my problem based on the previous posts.

I am solving a steady flow problem, say flow in a simple tube with "flux in" boundary conditions on the some portions of the walls for some of the "additional variables".

From physical point of view, the problem should reach steady state when the rate by which the additional variables are washed from the wall are equal to the rate by which the additional variables are released at the wall.

I have this "flux in" boundary conditions for three additional variables (i.e., AP, RP, and CF), while kinematic diffusivity of CF is 1000 times greater than AP and RP.

I get the solution converged for AP and RP after around 3500 iterations (automatic timescale) but the variable with higher diffusivity has a much slower convergence rate (far above the convergence criteria) even after 3500 iterations. Note, the velocity and pressure converged really fast at less than 100 iterations.

I am attaching a snapshot of the convergence curves, the convergence criteria is MAX RMS < 0.0005.

I was wondering if anyone can advise how I can get faster convergence.

Thanks a lot.
Attached Images

 July 4, 2017, 14:51 #2 Senior Member   Join Date: Jun 2009 Posts: 1,285 Rep Power: 25 You should read the documentation section titled: "Controlling the Timescale for Each Equation" You should probably set the timestep for the specific additional variable to a larger value than it is currently using. The CCL snippet you need is similar to Code: ```FLOW: Flow Analysis 1 SOLVER CONTROL: EQUATION: CF CONVERGENCE CONTROL: Length Scale Option = Conservative Timescale Control = Auto Timescale Timescale Factor = 1000 END END END END``` Please keep us posted on your progress with the above

July 6, 2017, 05:37
#3
Member

Join Date: Jun 2017
Posts: 39
Rep Power: 5
Quote:
 Originally Posted by Opaque You should read the documentation section titled: "Controlling the Timescale for Each Equation" You should probably set the timestep for the specific additional variable to a larger value than it is currently using. The CCL snippet you need is similar to Code: ```FLOW: Flow Analysis 1 SOLVER CONTROL: EQUATION: CF CONVERGENCE CONTROL: Length Scale Option = Conservative Timescale Control = Auto Timescale Timescale Factor = 1000 END END END END``` Please keep us posted on your progress with the above
Hi,

Thanks a lot. I followed your advice and observed that an increase in CF timescale can remarkably increase the convergence rate of this equation. Thanks.

However, a new problem raised. As the additional variable AP, which already met the convergence criteria, is affected by CF (they are coupled), the increase in CF timescale affected AP and I saw a sudden increase in AP MAX RMS which turned into sustained oscillations far above the convergence criteria after some iterations.

Now the CF MAX RMS is monotonically decreasing (and is below convergence criteria) but AP MAX RMS is oscillating at a level above convergence criteria.

I would appreciate any advice on that.

Thanks a lot.
Best

 July 6, 2017, 07:28 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 16,460 Rep Power: 128 There are many possible ways forward: * Put a slower time scale on the AP equation * Reduce the CF time scale * Just continue on and converge CF and the others tighter and see what AP does - it might converge after a while. cardioCFD likes this.