[saisanthoshm88]

I was trying out a ANSYS CFX workshop - Transonic flow over a NACA 0012 Airfoil and the Mach number used in the workshop was 0.7. Everything went well when the same Mach number was used but while running the simulation for higher mach numbers it was found that the solver is struggling more to reach the convergence target (= 1E-6 R.M.S). The Reynolds number is 9e6.The SST turbulence model is used. Dynamic viscosity is 1.82e-5. The temperature for the simulation is 288 K. The image attached shows the calculations for the pressure ( which is applied at the outlet boundary) and the velocity ( which is applied at the inlet boundary). Can some one suggest the ways by which I can have a more smoother convergence trend at Mach numbers higher than 0.7 in this problem.

[ghorrocks]

Convergence is often harder as the Ma number increases, this is not unusual. Sometimes you have to significantly change the numerical approach when the shock waves start appearing so a setup which ran fine subsonic does not work with a small increase in speed.

[saisanthoshm88]

Can you recommend some changes in a focussed way so that I can try them out in CFX for acheiving convergence at the supersonic speeds. Infact I've tried these settings for Mach numbers 1.2 and 1.6 but then the solver terminated abruptly and I recieved some Notices in the third iteration some thing like:

For Mach number = 1.6:
Notice: The maximum Mach number is 2.431E+02.

For Mach number = 1.2:
Notice: The maximum Mach number is 1.208E+02.

So after giving out such notices at the end of the third iteration the solver abruptly terminated.

Can you please suggest something out of this.It would be better even if you provide some generic steps to be followed in making the settings to achieve proper convergence for the supersonic flows.

[ghorrocks]

I find local timescale factor very useful in getting these sort of flows to start converging. Once you are on the road to convergence then swap back to physical time scales.

More details here: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

[saisanthoshm88]

Thanks for the suggestion Glenn, it works. I could indeed obtain the convergence with the local time scale control itself but can you please tell me why is it not recommended to go with the local time scale alone all the way to convergence (or) why is it stressed upon to run the final few iterations necessarily with a physical time scale instead.
And then after observing a convergence trend with the local time scale control, how do we shift the solver settings to the physical time scale control. Is it done by editing the run in progress?
I don’t really have a clarity upon this as this is the first time that I’m working with such options. Can you please guide me upon this.

[ghorrocks]

Do a search of the forum, this issue has been discussed a few times. To be honest, I can't remember the reason, I just remember you should not run local timescale factor all the way to convergence.

Yes, you can do a edit run in progress to switch over. No need to stop and restart.

[saisanthoshm88]

Thanks Glenn, yep I could find such information about the Local Timescale control on these Links of the forum:

http://www.cfd-online.com/Forums/cfx...cceptable.html
http://www.cfd-online.com/Forums/cfx...le-factor.html

So now everything is fine till a Mach number = 2.5 but there was a problem in convergence when I was trying out the things at Mach number = 3. My objective is indeed to acheive convergence at Hypersonic speeds and as such I was proceeding in a step by step manner trying out different Machnumbers.

I couldn't acheive convergence at Mach 3. Inspite of using a Local Timescale Factor = 10 and even by enabling the advanced options in the solver settings like:

Global Dynamic Model control
Velocity Pressure coupling-->RhieChow option-->High resolution
Compressibility control--> High speed Numerics

The problem is especially seen with the convergence of the continuity(P-Mass) equation.

I'm using the Total energy Heat transfer model and the SST turbulence model.

Can you please help me out in resolving this issue.

[ghorrocks]

Use a lower time scale factor as the Mach number increases.

[saisanthoshm88]

Hello Glenn,

I tried out reducing the Local Timescale Factor for the Mach 3 speed but it didn’t work. The P-Mass equation seems to be highly non linear.

In the ANSYS CFX documentation on compressible flows it was mentioned that such non linearity in the P-Mass equation is natural at Mach numbers greater than 2. It was also mentioned that the CFX-Solver will take action to stabilize the solution with an inner iteration that re-linearizes the continuity equation.

But in my case no such action is taken by the solver and in spite of that I was able to achieve a convergence at Mach 2.5 speed while I had a problem at Mach 3.

[ghorrocks]

The P-Mass equation seems to be highly non linear.

Not quite. The momentum equations are the non-linear ones. But keeping mass conservation in high Mach number flows is tricky.

I think you can manually set additional P-Mass equation solves with an expert parameter.

[saisanthoshm88]

Originally Posted by
[B

From CFX documentation

Expert control parameters
[/B]
Physical Models parameters

tef numerics option

Type
Integer

Default Value
0

Description
The and SST turbulence models sometimes give convergence
difficulties in areas of extremely high gradients in , for example, at
a blunt trailing edge or sudden rearward facing surface, in
conjunction with a highly refined boundary layer grid (generally
resolved into the viscous sub-layer). The SST model is most
susceptible to this problem. Symptoms are generally a lack of
convergence with residuals stuck at regions of extremely high
gradients of omega, sometimes leading to sudden, early total failure
of the solver. In these cases, a flux limiting numerics implementation
can be used for the equation, activated by setting this parameter to
1. This setting may become the default setting in a future release.

]

I've looked into the CFX documentation on Expert solver parameters but I didn't find any information on invoking an internal P-Mass equation

However, I found an option called tef numerics the description of which was quoted above from the documentation but my problem wasn't solved even after changing this option value to 1.

It is indeed mentioned in the documentation for compressible flows that the solver takes a step by itself to invoke such internal P-Mass equation when the local mach number exceeds 2 but that isn't happening for my case.

[ghorrocks]

No, that' snot the option I was talking about. I do not have access to the software right now so cannot give you the exact name, it is something like high speed numerics, extra p-mass conservation loop or something like that. There should be a comment in the output file suggesting you activate it for the high Ma number runs.

[saisanthoshm88]

Thanks Glenn I found that option.

Originally Posted by CFX Documentation

Expert Control Parameters

Convergence-Control Parameters

max continuity loops

Type
Integer
Default Value
1
Description
Sets the maximum number of continuity loops to perform within a timestep. The continuity loop iterates on the density*velocity nonlinearity in the continuity equation. The default value of 1 is usually appropriate. For high-speed supersonic flows (Mach numbers above 2), increasing the value to 2 may help convergence.

I've set this value to two and as such invoked an internal P-Mass equation which solved the problem.

And A Happy New Year In Advance!

[ghorrocks]

Excellent, yes that was the parameter I was thinking about. Good work for finding it from my vague description.

[saisanthoshm88]

Hi Glenn

The solution converged well till Mach 3 when the max continuity loops option was used but there seemed to be a problem when I've attempted to work at Mach 6. As I've mentioned it earlier I was indeed working out these things upon a Mesh for NACA Airfoil from a Ansys workshop when I've checked the mesh quality by importing it to ICEM CFD (it was a fluent mesh file indeed) I found it to be 0.16

So to have a convergence in case of a Mach 6 speed do you suggest me to try using any relaxation factors in the solver that help in resolving some issues with a poor mesh quality and also to have more continuity loops.

By the way I'm running a steady state simulation

[ghorrocks]

Mach 6 is getting very fast. Are you sure you don't have dissociation effects? If yes then CFX cannot model this flow.

I would try to improve mesh quality. Mesh quality becomes exponentially more important the faster you go.