User Variable Plot and Oscillating Convergence

marcel_jay · August 21, 2014, 11:11

Hello CFD Community,

I am experience some convergence problems and that's why want to observe user variables in my simulation.
At first I just plotted pressure loss, which worked fine, but now additionally I want to plot average inlet velocity and mass flow.
The issue is, it is all plotted in one graph, so I see the velocity converging, but the other two are displayed just as a line next to the x-axis. I think it's because the values are to far from each other.
Any hint how to fix this?

Secondly, I wanted to ask what you think about a converging solution that is not monotonic, means oscillation. It reaches the residual target after about 170 timesteps though.
Is the non-monotonic behaviour inaccurate even if the result is below my residuals?

Cheers

Marcel

marcel_jay · August 21, 2014, 11:18

Okay, for the first issue, I just found out you can right click the plotted graph (Monitor Properties) and deselect single variables!

ghorrocks · August 21, 2014, 20:52

The residual is not a total measure of convergence. The variation on your inlet velocity suggests that in your case, even though the residuals are tight the flow has not converged. So in your case I would add imbalances to your convergence requirement. Then you will continue until the global balances are good too.

This is a sign that your physical time scale is probably too short. You would converge faster if you used a larger physical time scale.

marcel_jay · September 5, 2014, 11:20

First of all, thanks a lot for you answer.

I now understand my user variables as my main convergence criteria.
RMS Targets were after about 100 timesteps very close to 1E-4, but all my user variables very diverging (almost linear). And that even after 500 timesteps, whilst Momentum and Mass were oscillating at the same level.

As I think my mesh is pretty good (min orthogonal quality = 0.25 and max skewness = 0.8) I might have to fix the timescale.
Imbalances were set to 1% and the results were 0.05% to 1.7% which is not even too bad I suppose.

I used automatical timescale (conservative, factor 1.0) so far.

In the CFD-Online Tutorial it says I need the average residence time, don't know how to get that. In the streamline it tells me that 0,00013s is the max value.
Do you know how to find the right physical time scale?
Also shouldn't I use the residence time of previous converging models (similar), as with diverging velocitys the timescale changes. In my previous solutions the max residence time was 10 times higher.

An ANSYS video tutorial said you should use a physical timescale of about 1/3 of the velocity scale or 1/ω when the domain rotates. Mine rotates with 30k rpm.
As I've seen people using timescales of about 2 seconds... mine would be a million times smaller, isn't that bad?

Cheers
Marcel

ghorrocks · September 6, 2014, 07:48

In a steady state simulation the exact value of the time step is not important. All the suggestions of residence time or functions of the rotation speed are really just starting guesses. You need an approximate time step just to get started.

If it diverges then restart with a smaller time step. If it converges slowly then use "edit run in progress" to increase the time step. You can probably edit it a few times as the simulation converges you should be able to use larger time steps. But if it starts to go wobbly you have gone too far so back it off again.

So all the time step sizes you quote are just a starting point, and it does not really matter which one you choose. You then run it and adjust it as you go.

August 21, 2014, 11:18	Found a solution	#2
marcel_jay Member Marcel Jay Join Date: Jun 2014 Location: Berlin Posts: 52 Rep Power: 11	Okay, for the first issue, I just found out you can right click the plotted graph (Monitor Properties) and deselect single variables!

August 21, 2014, 20:52		#3
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,719 Rep Power: 143	The residual is not a total measure of convergence. The variation on your inlet velocity suggests that in your case, even though the residuals are tight the flow has not converged. So in your case I would add imbalances to your convergence requirement. Then you will continue until the global balances are good too. This is a sign that your physical time scale is probably too short. You would converge faster if you used a larger physical time scale. rgd likes this.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Oscillating residuals and no convergence!	Sherlock_1812	OpenFOAM Running, Solving & CFD	7	August 20, 2014 09:39

September 5, 2014, 11:20		#4
marcel_jay Member Marcel Jay Join Date: Jun 2014 Location: Berlin Posts: 52 Rep Power: 11	First of all, thanks a lot for you answer. I now understand my user variables as my main convergence criteria. RMS Targets were after about 100 timesteps very close to 1E-4, but all my user variables very diverging (almost linear). And that even after 500 timesteps, whilst Momentum and Mass were oscillating at the same level. As I think my mesh is pretty good (min orthogonal quality = 0.25 and max skewness = 0.8) I might have to fix the timescale. Imbalances were set to 1% and the results were 0.05% to 1.7% which is not even too bad I suppose. I used automatical timescale (conservative, factor 1.0) so far. In the CFD-Online Tutorial it says I need the average residence time, don't know how to get that. In the streamline it tells me that 0,00013s is the max value. Do you know how to find the right physical time scale? Also shouldn't I use the residence time of previous converging models (similar), as with diverging velocitys the timescale changes. In my previous solutions the max residence time was 10 times higher. An ANSYS video tutorial said you should use a physical timescale of about 1/3 of the velocity scale or 1/ω when the domain rotates. Mine rotates with 30k rpm. As I've seen people using timescales of about 2 seconds... mine would be a million times smaller, isn't that bad? Cheers Marcel

September 6, 2014, 07:48		#5
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,719 Rep Power: 143	In a steady state simulation the exact value of the time step is not important. All the suggestions of residence time or functions of the rotation speed are really just starting guesses. You need an approximate time step just to get started. If it diverges then restart with a smaller time step. If it converges slowly then use "edit run in progress" to increase the time step. You can probably edit it a few times as the simulation converges you should be able to use larger time steps. But if it starts to go wobbly you have gone too far so back it off again. So all the time step sizes you quote are just a starting point, and it does not really matter which one you choose. You then run it and adjust it as you go.