[x31fighter]

[QUOTE=yaseen wsu;603393]

Originally Posted by -Maxim-

My convergence criteria is MAX residuals < 10^-3 and imbalances <1%.
"Timescale Factor" here is just a multiplier of "Auto Timescale".

dear Maxim is residual < 10^-3 acceptable for academic research? I surprised because according to CFX documentation even bellow 10^-4 is only for qualitative understanding of the flow field not quantitative (I know this value depends that what is you modeled). thanks

Talking to my professors, typically 10^-5 is the bare minimum and is very case dependent. Some cases might require lower than that.

[yaseen wsu]

[QUOTE=x31fighter;603401]

Originally Posted by yaseen wsu

Talking to my professors, typically 10^-5 is the bare minimum and is very case dependent. Some cases might require lower than that.

yes, but in my view depend on the cases, for Ex. free surface simulation in spillway which is large structure 10^-4 enough only for surface height but for other variables such as velocity shear stress extra accuracy is required.

[-Maxim-]

Originally Posted by yaseen wsu

dear Maxim is residual < 10^-3 acceptable for academic research? I surprised because according to CFX documentation even bellow 10^-4 is only for qualitative understanding of the flow field not quantitative (I know this value depends that what is you modeled). thanks

Originally Posted by x31fighter

Talking to my professors, typically 10^-5 is the bare minimum and is very case dependent. Some cases might require lower than that.

I wrote MAX residuals < 10^-3. Not RMS residuals. If my case with a rotating propeller reaches MAX residuals <10^-3, the RMS residuals are below 10^-5. Some RMS residuals are even between 10^-6 and 10^-7.
Therefore my criteria is pretty strict.
Furthermore, I use my steady-state result "just" as an initial solution for the "real" transient simulation. Even if MAX residuals of 10^-3 is not reached by every residuals in every domain, the RMS residuals of 10^-4 is easily reached everywhere.

Read up on MAX residuals in the documentation in case you want to know more

[ghorrocks]

You should do a sensitivity analysis on convergence tolerance when you start a new class of simulation anyway. Different simulations require different convergence tolerances, and people have different ideas about what "accurate enough" is anyway.

[zryan civil]

Originally Posted by -Maxim-

I wrote MAX residuals < 10^-3. Not RMS residuals. If my case with a rotating propeller reaches MAX residuals <10^-3, the RMS residuals are below 10^-5. Some RMS residuals are even between 10^-6 and 10^-7.
Therefore my criteria is pretty strict.
Furthermore, I use my steady-state result "just" as an initial solution for the "real" transient simulation. Even if MAX residuals of 10^-3 is not reached by every residuals in every domain, the RMS residuals of 10^-4 is easily reached everywhere.

Read up on MAX residuals in the documentation in case you want to know more

yes you are right

[x31fighter]

I was able to get my setup to work with decent results within my acceptable range for Reynolds number up to 10^5.

I was reading "Synopsis of Lift, Drag, and Vortex Frequency Data for Rigid Circular Cylinders" By John H. Lienhard. It mentions that the boundary layer attached to the Cylinder transitions from laminar to turbulent in the range of 10^5 < Re < 5*10^5. Would this be something I need to take into account when setting up the simulation? Or would this occur when the simulation is running?

If this is something I need to take into account, how would I do this in CFX?

[ghorrocks]

You can use the SST turbulence transition model for this if you like.

[x31fighter]

In CFX, is that as simple as just selecting SST turbulence model then checking the transitional turbulence checkbox under it?

[ghorrocks]

To activate those models, yes, that is all which is required.

The skill is to get it to converge and generate appropriate mesh, time step and convergence settings so it runs accurately.

[x31fighter]

The current model I am using is SST and I did a mesh refinement for the cylinder and got a Cd of 0.98 for Re = 50000. I am expecting a value closer to 1.2 for Cd according to experimental results. My problem is "2D" with a thickness of 0.00762 m for the z direction. I was wondering if there were any physics that I could be potentially missing? The only thing I can think of is having the model extruded more for a more 3D cylinder.

Another issue, when I tried running k-epsilon I got a fatal overflow causing it to diverge as a transient case. I check the mesh and that doesn't seem to be an issue. I tried running it at Steady-State with automatic initial conditions and it seems to converge fine. I can't use automatic initial conditions for transient setup. Is there a way to determine initial conditions so that there is not a fatal overflow? Or is there another reason why it crashes?

Thanks in advance.

[ghorrocks]

FAQ: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F