CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Mach number Vs Convergence trend

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 14, 2010, 06:07
Default Mach number Vs Convergence trend
  #1
Senior Member
 
---------
Join Date: Oct 2010
Posts: 302
Rep Power: 8
saisanthoshm88 is on a distinguished road
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.
Attached Images
File Type: jpg Calculations.JPG (30.6 KB, 88 views)
__________________
Best regards,
Santhosh.
saisanthoshm88 is offline   Reply With Quote

Old   December 14, 2010, 06:49
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,662
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   December 14, 2010, 08:41
Default
  #3
Senior Member
 
---------
Join Date: Oct 2010
Posts: 302
Rep Power: 8
saisanthoshm88 is on a distinguished road
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.
__________________
Best regards,
Santhosh.
saisanthoshm88 is offline   Reply With Quote

Old   December 14, 2010, 17:33
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,662
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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
ghorrocks is offline   Reply With Quote

Old   December 15, 2010, 03:46
Default
  #5
Senior Member
 
---------
Join Date: Oct 2010
Posts: 302
Rep Power: 8
saisanthoshm88 is on a distinguished road
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 donít really have a clarity upon this as this is the first time that Iím working with such options. Can you please guide me upon this.
__________________
Best regards,
Santhosh.
saisanthoshm88 is offline   Reply With Quote

Old   December 15, 2010, 05:57
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,662
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   December 18, 2010, 14:16
Default Hypersonic flow - reg...
  #7
Senior Member
 
---------
Join Date: Oct 2010
Posts: 302
Rep Power: 8
saisanthoshm88 is on a distinguished road
Thanks Glenn, yep I could find such information about the Local Timescale control on these Links of the forum:

Convergence on Local Time Scale Acceptable
Local Timescale Factor

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.
__________________
Best regards,
Santhosh.

Last edited by saisanthoshm88; December 18, 2010 at 21:37.
saisanthoshm88 is offline   Reply With Quote

Old   December 19, 2010, 17:05
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,662
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Use a lower time scale factor as the Mach number increases.
ghorrocks is offline   Reply With Quote

Old   December 22, 2010, 01:33
Default
  #9
Senior Member
 
---------
Join Date: Oct 2010
Posts: 302
Rep Power: 8
saisanthoshm88 is on a distinguished road
Hello Glenn,

I tried out reducing the Local Timescale Factor for the Mach 3 speed but it didnít 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.
__________________
Best regards,
Santhosh.
saisanthoshm88 is offline   Reply With Quote

Old   December 22, 2010, 07:15
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,662
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
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.
ghorrocks is offline   Reply With Quote

Old   December 28, 2010, 12:26
Default
  #11
Senior Member
 
---------
Join Date: Oct 2010
Posts: 302
Rep Power: 8
saisanthoshm88 is on a distinguished road
Quote:
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.
__________________
Best regards,
Santhosh.
saisanthoshm88 is offline   Reply With Quote

Old   December 28, 2010, 16:39
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,662
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   December 29, 2010, 02:49
Default
  #13
Senior Member
 
---------
Join Date: Oct 2010
Posts: 302
Rep Power: 8
saisanthoshm88 is on a distinguished road
Thanks Glenn I found that option.

Quote:
Originally Posted by CFX Documentation View Post

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!
__________________
Best regards,
Santhosh.
saisanthoshm88 is offline   Reply With Quote

Old   December 29, 2010, 06:46
Default
  #14
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,662
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Excellent, yes that was the parameter I was thinking about. Good work for finding it from my vague description.
ghorrocks is offline   Reply With Quote

Old   December 31, 2010, 02:03
Default
  #15
Senior Member
 
---------
Join Date: Oct 2010
Posts: 302
Rep Power: 8
saisanthoshm88 is on a distinguished road
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
__________________
Best regards,
Santhosh.

Last edited by saisanthoshm88; January 12, 2011 at 23:59.
saisanthoshm88 is offline   Reply With Quote

Old   January 13, 2011, 01:59
Default
  #16
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,662
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Mesh Refinement Luiz Eduardo Bittencourt Sampaio (Sampaio) OpenFOAM Mesh Utilities 41 January 17, 2013 03:43
Unaligned accesses on IA64 andre OpenFOAM 5 June 23, 2008 10:37
Abt: Mach number.. Help! Plz! jinwon park Main CFD Forum 0 February 5, 2008 14:57
The Far-field Pressure Boundary & Low Mach Number Saif-Deen Akanni FLUENT 1 March 5, 2007 06:05
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15


All times are GMT -4. The time now is 15:18.