[krihamm]

Hi,

I am doing a transient simulation at Mach 1 to determine drag. I have added a monitor point to monitor the progression of drag. Time step is set to <delta x / u, upwind advection scheme, first order backward Euler transient scheme, first order turbulence numerics.

The monitor point is so far (after approx 11 hour simulation) smooth and still decreasing, although not converged yet. The residual profile is however showing no signs of smoothing out (see attachment).

How important is it that the residual profile is smooth when determining the accuracy of a simulation? If the monitor point eventually converges, is that enough to conclude good results, or should I troubleshoot and see if I can improve the residual profile?

Thanks!

[AtoHM]

I would give it a bit more time, does not seem converged yet.

Also, you should check for MAX Residuals rather than RMS. The RMS can "cover up" higher residuals somewhere in the domain if they are low on the majority of the cells. I am using MAX res of 1E-3 for my steady runs, which is hard to get from the transient ones. If you are not able to get to this value (or some other you want to achieve) you should print a trn result step with the residuals and check where the highest residuals are in the domain in Post.

Residuals are not gonna smooth like your drag monitor for example, but they should lay below of some level you have to define.

[Gert-Jan]

- why do you use upwind (default high resolution) and first order in time (default 2nd order)?
- you only have 70 iterations. That is nothing. 200-500 is quite normal. So continue the calculation.
- did your computer take 11 hours to complete 70 iterations? How many nodes do you have?

[krihamm]

Originally Posted by AtoHM

I would give it a bit more time, does not seem converged yet.

Also, you should check for MAX Residuals rather than RMS. The RMS can "cover up" higher residuals somewhere in the domain if they are low on the majority of the cells. I am using MAX res of 1E-3 for my steady runs, which is hard to get from the transient ones. If you are not able to get to this value (or some other you want to achieve) you should print a trn result step with the residuals and check where the highest residuals are in the domain in Post.

Residuals are not gonna smooth like your drag monitor for example, but they should lay below of some level you have to define.

Thank you for your reply, I will check for max residuals instead! Is it possible to pause the simulation and change from RMS to max in setup and then continue the simulation, or do I need to restart the whole thing?

[Gert-Jan]

you can do it on the fly. Just click inside the graph on the right mouse button and select "Switch Residual Mode"

[krihamm]

Originally Posted by Gert-Jan

- why do you use upwind (default high resolution) and first order in time (default 2nd order)?
- you only have 70 iterations. That is nothing. 200-500 is quite normal. So continue the calculation.
- did your computer take 11 hours to complete 70 iterations? How many nodes do you have?

I recall that upwind is more robust than high resolution. Am I mistaken? I have approx 2 600 00 nodes. Smallest node size 8.3433e-2 m and a flow speed of 343 m/s gives a very small time step in order for time step < delta x / u to be fulfilled. Max coefficient loops set to 4.

[Gert-Jan]

Using upwind should be forbidden in CFX, since you have high Resolution. Especially around Mach 1.
Upwind and first order in time may be more stable, but inappropriate when it comes to accuracy. This is really a waste of time.

You could use upwind as a start to come to an initial condition in steady state. But even that is really unnecessary. I haven't used upwind in CFX for more than 12 years. Just stick to the defaults.

[krihamm]

Originally Posted by Gert-Jan

Using upwind should be forbidden in CFX, since you have high Resolution. Especially around Mach 1.
Upwind and first order in time may be more stable, but inappropriate when it comes to accuracy. This is really a waste of time.

You could use upwind as a start to come to an initial condition in steady state. But even that is really unnecessary. I haven't used upwind in CFX for more than 12 years. Just stick to the defaults.

Thank you for your reply! I will change to high resolution and second order and compare. What is your recommendation for transient scheme? Second order also?

[Gert-Jan]

Sure. Use second order in time.

[AtoHM]

Originally Posted by Gert-Jan

you can do it on the fly. Just click inside the graph on the right mouse button and select "Switch Residual Mode"

That was a bit misleading on my part. Yes as Gert wrote, you can directly switch to MAX in solver manager.
I was actually going for printing the residuals to a file so you can check where your mesh generates high values of it and improve it there if possible. That would be only required if you have high max residuals of course. IF it is: you have to define transient output in Pre -> Output Control -> Trn Results and there you can create an trn result item with "output equation residuals". If you dont want a hugh amount of data, take only selected variables output, not full and define some timesteps you are interested in, maybe 10,20,30,40,...