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

Flow solver crashes abruptly in Fine/Turbo

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

Like Tree1Likes
  • 1 Post By Hamidzoka

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 17, 2022, 14:23
Default Flow solver crashes abruptly in Fine/Turbo
  #1
New Member
 
OH
Join Date: Apr 2022
Posts: 1
Rep Power: 0
saugat is on a distinguished road
Hello All!
I am using Cadence Autogrid/Fineturbo to work on a case of SCO2 compressor. I cannot share much details due to the sensitivity of the project but the issue I am having is: After running around 200 - 300 iterations, I get 'negative density' in multiple domains in run log and residuals shoot up and the flow solver crash abruptly.
The mesh is not as per the best criteria but the mesh generation window looks good enough enough overall and doesnot produce any warnings.

I am looking for a way to pinpoint exaclty what is causing the flow solver to crash. I have seen some suggestions in different forums to look at the residuals but I am not sure what is the best way to do this. Any suggestions would be very helpful.

Thanks,
Saugat
Attached Images
File Type: jpg mesh_details1.jpg (121.6 KB, 6 views)
File Type: jpg r1.jpg (76.4 KB, 5 views)
File Type: jpg mf2.jpg (88.4 KB, 4 views)
saugat is offline   Reply With Quote

Old   June 21, 2022, 04:18
Default Cause of divergence
  #2
Senior Member
 
Colinda
Join Date: May 2012
Location: Brussels
Posts: 144
Rep Power: 12
colinda1 is on a distinguished road
Hi,

When a computation diverges in such way, I would relaunch it with a number iterations such that the simulation ends just before the divergence.
Then you can look in post processing where in the domain something unphysical happens: are there unphysical temperatures somewhere in the domain? Look at the minimum and maximum pressure and temperature ranges to see whether that could be the case. Then an iso-surface can help to locate these unphysical values. A velocity vector plot or streamlines throughout the domain may also help to identify the cause of trouble.

Best regards,
Colinda
colinda1 is offline   Reply With Quote

Old   July 19, 2022, 03:06
Default
  #3
Senior Member
 
Hamid Zoka
Join Date: Nov 2009
Posts: 277
Rep Power: 17
Hamidzoka is on a distinguished road
Hi;
According to the attached picture, divergence takes place after termination of coarser grids iterations. Possible reasons can be: turbulent model, mesh quality and improper initial conditions. Try to locate the point at which divergence starts. This can normally be found through post-processing the case at 1 or 2 iterations prior to divergence. This may give an insight to origins of divergence. Also try more stable turbulence models like SA. More sophisticated turbulence models like SST are more sensitive to mesh quality.
One more thing that needs attention is that achieving a converged solution in case of multi-stage compressors can be an issue and needs a precise setting of initial solution. Improper setting of flow directions, temperature and pressure levels will definitely result in divergence which is not the case in turbines.
Maybe you need a mean-line quick calculation of flow directions as well as P and T, to find a proper initial solution prior to CFD simulation.
You also need to check your material properties.

Regards
colinda1 likes this.
Hamidzoka is offline   Reply With Quote

Old   August 10, 2022, 00:29
Default
  #4
New Member
 
Join Date: Aug 2022
Posts: 4
Rep Power: 2
gsgt07 is on a distinguished road
But how is your mass flow rate is so much different at inlet and outlet
gsgt07 is offline   Reply With Quote

Old   August 11, 2022, 04:30
Default
  #5
Senior Member
 
Hamid Zoka
Join Date: Nov 2009
Posts: 277
Rep Power: 17
Hamidzoka is on a distinguished road
Quote:
Originally Posted by gsgt07 View Post
But how is your mass flow rate is so much different at inlet and outlet
Inlet and outlet mass flow rates are quite different since the solution is diverging. Divergence is generally associated with unrealistic values in pressure, velocity, density and consequently the mass flow rate.
Hamidzoka is offline   Reply With Quote

Old   August 11, 2022, 05:04
Default Hi
  #6
New Member
 
Join Date: Aug 2022
Posts: 4
Rep Power: 2
gsgt07 is on a distinguished road
The flow basically is diverging because of implementation of wrong boundary condition or either may be you are using some bad quality mesh.
The selection of turbulence model I think so have no concerned with divergence of solution because in turbulence modeling we are modelling the turbulent viscosity that can be further used in NS equation if you are getting wrong velocity & pressure field that may be because of wrong implementation of BC's or IC's.
If you have any doubt on turbulence model in that case you can run your simulation by excluding the turbulence model means as DNS.
gsgt07 is offline   Reply With Quote

Old   August 17, 2022, 02:35
Default
  #7
Senior Member
 
Hamid Zoka
Join Date: Nov 2009
Posts: 277
Rep Power: 17
Hamidzoka is on a distinguished road
Quote:
Originally Posted by gsgt07 View Post
The flow basically is diverging because of implementation of wrong boundary condition or either may be you are using some bad quality mesh.
The selection of turbulence model I think so have no concerned with divergence of solution because in turbulence modeling we are modelling the turbulent viscosity that can be further used in NS equation if you are getting wrong velocity & pressure field that may be because of wrong implementation of BC's or IC's.
If you have any doubt on turbulence model in that case you can run your simulation by excluding the turbulence model means as DNS.
From physical point of view you are right. However, note that solver tries to handle a system of equations with different levels of complexity and non-linearity. Different turbulence models, depending on their assumptions and formulations, have terms with different levels of non-linearity. It means that simpler models with less sophisticated source terms will have a better chance to converge while the more complex models engaging different combinations of flow parameters have issues in convergence.
Just as an example, there exist different vesrions for RSM turbulence models. some uses eddy viscosity to model the diffusion term while others use Reynolds stress components instead. The former definitely has less convergence issues, while the later models are prone to divergence. Thus, technically turbulence model has an impact on convergence

Regards
Hamidzoka is offline   Reply With Quote

Old   August 17, 2022, 03:43
Default Hi
  #8
New Member
 
Join Date: Aug 2022
Posts: 4
Rep Power: 2
gsgt07 is on a distinguished road
In such case you have to check that at which point (location) the maximum divergence has taken place but in Fidelity how to locate that point either may be in log file or even if you know that point then how to find that location in computational domain
gsgt07 is offline   Reply With Quote

Reply

Tags
fine/turbo, residual, solver crash

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Buoyancy-driven flow eclipsed by solver noise? JayDeeUU OpenFOAM Running, Solving & CFD 1 May 3, 2022 05:40
Buoyancy-driven flow eclipsed by solver noise? JayDeeUU OpenFOAM Running, Solving & CFD 0 March 7, 2021 17:53
PEMFC model with FLUENT brahimchoice FLUENT 22 April 19, 2020 16:44
Maximum words supported by the flow solver exceeded rae CFX 3 June 6, 2013 07:49
laminar pipe flow with buoyantSimpleRadiationFoam and janafThermo crashes Fabian OpenFOAM 1 September 29, 2010 12:38


All times are GMT -4. The time now is 23:47.