Residual graph issue

estar · March 9, 2020, 13:48

I am running a simulation for flow over 2d cylinder. I ran a laminar-turbulent 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, k-epsilon, velocity is 0.2m/s
Time step is 0.05s (second order discretisation)
courant number 0.5

fluid23 · March 9, 2020, 16:34

It is necessary for us to see your residual plot in order to diagnose issues with it. Can you upload a copy?

estar · March 9, 2020, 17:48

the residual and mesh are attached. Actually the re=10K is definitely wrong

MRI · March 10, 2020, 06:08

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.

estar · March 10, 2020, 07:22

thank you for your feedback. It has improved the graph and looks within the range but the spiking seem abnormal to me

estar · March 10, 2020, 07:23

heres the graph

MRI · March 10, 2020, 07:53

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 Courant-number, Underrelaxation factor or the convergence accelerator. Also a good initialization may help you.

estar · March 10, 2020, 08:08

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

LuckyTran · March 10, 2020, 11:08

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.

estar · March 10, 2020, 13:24

i tweaked the under-relaxation 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.

estar · March 10, 2020, 13:25

Quote:

Originally Posted by LuckyTran

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.

someone said it was wrong but they were comparing to OpenFOAM residuals which i am pretty sure uses a PISO solver

LuckyTran · March 11, 2020, 11:37

Quote:

Originally Posted by estar

i tweaked the under-relaxation factor. this 2 Attachment 75474 and the other is 0.5Attachment 75476. but i turned the normalisation on again to see if it was similar to what was happening before.

These look fine. There is a spike in the residual at the begining of the time-step followed by reduction in residuals. You can complain that the level of residuals it not enough and you want more (i.e. smaller than 5e-05 blah blah blah) but this is the expected behavior. If it doesn't spike then you're doing it wrong.

The reason it spikes is because the 1st iteration of the new time-step uses the final solution of the previous time-step as the initial guess. The solution to the previous time-step will always be different than the new time-step unless your flow is completely stationary. So you are always guaranteed to see a spike.

PISO if done the PISO way is iteration-less (1 iteration) so of course the residual plot will look very different.

estar · March 12, 2020, 07:43

thank you for explaining the residual graphs to me. I will try and improve on the setup to see if anything changes

estar · March 13, 2020, 11:48

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

March 9, 2020, 13:48	Residual graph issue	#1
estar New Member Emmanuel Sarpong Join Date: Dec 2019 Posts: 10 Rep Power: 7	I am running a simulation for flow over 2d cylinder. I ran a laminar-turbulent 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, k-epsilon, velocity is 0.2m/s Time step is 0.05s (second order discretisation) courant number 0.5

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[solids4Foam] How to calculate drag coeff when using solids4Foam	amuzeshi	OpenFOAM CC Toolkits for Fluid-Structure 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

March 9, 2020, 16:34		#2
fluid23 Senior Member Matt Join Date: Aug 2014 Posts: 947 Rep Power: 18	It is necessary for us to see your residual plot in order to diagnose issues with it. Can you upload a copy?

March 10, 2020, 06:08		#4
MRI New Member Marco Riedel Join Date: Apr 2011 Location: Germany Posts: 25 Rep Power: 15	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
estar New Member Emmanuel Sarpong Join Date: Dec 2019 Posts: 10 Rep Power: 7	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, 07:53		#7
MRI New Member Marco Riedel Join Date: Apr 2011 Location: Germany Posts: 25 Rep Power: 15	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 Courant-number, Underrelaxation factor or the convergence accelerator. Also a good initialization may help you.

March 10, 2020, 08:08		#8
estar New Member Emmanuel Sarpong Join Date: Dec 2019 Posts: 10 Rep Power: 7	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
LuckyTran Senior Member Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,761 Rep Power: 66	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
estar New Member Emmanuel Sarpong Join Date: Dec 2019 Posts: 10 Rep Power: 7	i tweaked the under-relaxation 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 12, 2020, 07:43		#13
estar New Member Emmanuel Sarpong Join Date: Dec 2019 Posts: 10 Rep Power: 7	thank you for explaining the residual graphs to me. I will try and improve on the setup to see if anything changes