
[Sponsors] 
March 9, 2020, 13:48 
Residual graph issue

#1 
New Member
Emmanuel Sarpong
Join Date: Dec 2019
Posts: 10
Rep Power: 5 
I am running a simulation for flow over 2d cylinder. I ran a laminarturbulent case at from re=100 to Re=10K. I was comparing the drag values to a paper and most values were similar. I could visualise vortex shedding and vector scene. However, i was told that my residual graph is wrong and so the solver is not stable. I don't know what part of my setup is wrong and i need to apply this case to several bridge deck sections. If anyone has any solutions please help.
SetUP Domain: 4m by 6m(hxL) Radius of cylinder:0.05m Meshing: Surface Wrapper, Polyhedral, Surface Meshing Values: base size:20cm thn 2 volumetric controls of 2cm and 1cm aruond the wake of the cylinder Physics: air (Standard), coupled flow, implicit unsteady, kepsilon, velocity is 0.2m/s Time step is 0.05s (second order discretisation) courant number 0.5 

March 9, 2020, 16:34 

#2 
Senior Member
Matt
Join Date: Aug 2014
Posts: 929
Rep Power: 16 
It is necessary for us to see your residual plot in order to diagnose issues with it. Can you upload a copy?


March 9, 2020, 17:48 

#3 
New Member
Emmanuel Sarpong
Join Date: Dec 2019
Posts: 10
Rep Power: 5 
the residual and mesh are attached. Actually the re=10K is definitely wrong


March 10, 2020, 06:08 

#4 
New Member
Marco Riedel
Join Date: Apr 2011
Location: Germany
Posts: 25
Rep Power: 13 
The residual plot shows per default the normalized residuals. If I understood it right, Star divides the actual iteration through the average value of the first 6 iterations. Sometimes the residuals look better, if you switch the normalization option to off.


March 10, 2020, 07:22 

#5 
New Member
Emmanuel Sarpong
Join Date: Dec 2019
Posts: 10
Rep Power: 5 
thank you for your feedback. It has improved the graph and looks within the range but the spiking seem abnormal to me


March 10, 2020, 07:23 

#6 
New Member
Emmanuel Sarpong
Join Date: Dec 2019
Posts: 10
Rep Power: 5 
heres the graph


March 10, 2020, 07:53 

#7 
New Member
Marco Riedel
Join Date: Apr 2011
Location: Germany
Posts: 25
Rep Power: 13 
Phew, as a next step I would look at the solver settings. But first of all I would try to solve the case with the segregated solver. If you don't see problems in that case, you know that you have to work on the (coupled) solver settings .Something like Courantnumber, Underrelaxation factor or the convergence accelerator. Also a good initialization may help you.


March 10, 2020, 08:08 

#8 
New Member
Emmanuel Sarpong
Join Date: Dec 2019
Posts: 10
Rep Power: 5 
yh i will try the segregated solver and see what i need to do with the coupled solver. I will let you know what happens


March 10, 2020, 11:08 

#9 
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,112
Rep Power: 60 
Make a report of a solution value (velocity, pressure, temperature, etc.) and also make a monitor and report of it and check that it is asymptotically converging.
Isn't this a transient simulation? In which case the residuals makes 100% sense. 

March 10, 2020, 13:24 

#10 
New Member
Emmanuel Sarpong
Join Date: Dec 2019
Posts: 10
Rep Power: 5 
i tweaked the underrelaxation factor. this 2 Capture4.PNG and the other is 0.5Capture5.PNG. but i turned the normalisation on again to see if it was similar to what was happening before.


March 10, 2020, 13:25 

#11 
New Member
Emmanuel Sarpong
Join Date: Dec 2019
Posts: 10
Rep Power: 5 
someone said it was wrong but they were comparing to OpenFOAM residuals which i am pretty sure uses a PISO solver


March 11, 2020, 11:37 

#12  
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,112
Rep Power: 60 
Quote:
The reason it spikes is because the 1st iteration of the new timestep uses the final solution of the previous timestep as the initial guess. The solution to the previous timestep will always be different than the new timestep unless your flow is completely stationary. So you are always guaranteed to see a spike. PISO if done the PISO way is iterationless (1 iteration) so of course the residual plot will look very different. 

March 12, 2020, 07:43 

#13 
New Member
Emmanuel Sarpong
Join Date: Dec 2019
Posts: 10
Rep Power: 5 
thank you for explaining the residual graphs to me. I will try and improve on the setup to see if anything changes


March 13, 2020, 11:48 

#14 
New Member
Emmanuel Sarpong
Join Date: Dec 2019
Posts: 10
Rep Power: 5 
i was able to obtain sufficient results for the cylinder case however now i am applying the same setup to the a bridge deck do you think these are acceptable residuals or should edit the setup further


Tags 
meshing, residal, residuals every iteration, star ccm+ 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
[solids4Foam] How to calculate drag coeff when using solids4Foam  amuzeshi  OpenFOAM CC Toolkits for FluidStructure Interaction  15  November 7, 2019 13:50 
Suppress twoPhaseEulerFoam energy  AlmostSurelyRob  OpenFOAM Running, Solving & CFD  33  September 25, 2018 18:45 
Segmentation fault when using reactingFOAM for Fluids  Tommy Floessner  OpenFOAM Running, Solving & CFD  4  April 22, 2018 13:30 
Unstabil Simulation with chtMultiRegionFoam  mbay101  OpenFOAM Running, Solving & CFD  13  December 28, 2013 14:12 
Error while running rhoPisoFoam..  nileshjrane  OpenFOAM Running, Solving & CFD  8  August 26, 2010 13:50 