# Residual graph issue

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 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 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

 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
Attached Images
 Capture1222.jpg (123.4 KB, 40 views) Capture22.PNG (185.8 KB, 24 views)

 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
Attached Images
 Capture33.PNG (107.4 KB, 25 views)

 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 Courant-number, 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 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 10, 2020, 13:25
#11
New Member

Emmanuel Sarpong
Join Date: Dec 2019
Posts: 10
Rep Power: 5
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

March 11, 2020, 11:37
#12
Senior Member

Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,112
Rep Power: 60
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.

 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
Attached Images
 Capture6.PNG (138.5 KB, 20 views)

 Tags meshing, residal, residuals every iteration, star ccm+

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 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 OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 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 AlmostSurelyRob OpenFOAM Running, Solving & CFD 33 September 25, 2018 18:45 Tommy Floessner OpenFOAM Running, Solving & CFD 4 April 22, 2018 13:30 mbay101 OpenFOAM Running, Solving & CFD 13 December 28, 2013 14:12 nileshjrane OpenFOAM Running, Solving & CFD 8 August 26, 2010 13:50

All times are GMT -4. The time now is 23:38.

 Contact Us - CFD Online - Privacy Statement - Top