# Oscillating Residuals (with picture)

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

 March 22, 2013, 09:12 Oscillating Residuals (with picture) #1 New Member   Pete Drum Join Date: Sep 2012 Posts: 6 Rep Power: 6 Sponsored Links Hi guys, iam doing a wind flow velocity analysis around a building as a project for college (->external flow). As I said in the title, i have an issue with oscillating residuals. I meshed the system with tets and generated 10 boundary layers around the building. Number of elements is about 1.8 *10^6. I made the enveloping body as big as described in the ANSYS tutorials. As Inlet andOutlet I used velocity inlet and pressure outlet. The turbulence model is a k-epsilon with realizable and enhanced wall treatment. The wind velocity at the inlet is 8 m/s. furhtermore, I defined SIMPLE and everything alse as second-order. Y+ is about 200. I didnt change any of the URF's. There are no mesh warnings, if I check the mesh in the solver. solver is pressure-based and I defined steady state. thats how it looks after 5000 iterations: Uploaded with ImageShack.us any ideas how to solve this problem? thank you! regards

 March 22, 2013, 10:26 #2 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,490 Rep Power: 25 Some things you can try: check the turbulence values at the inlet make sure your model has the right dimensions lower under relaxation factors for pressure and momentum deactivate the realizable option of the k-epsilon turbulence model use first order interpolation schemes use a mesh with lower Y+ post a picture of the setup here ... many other things ... run a LES instead of the RANS approach because of the dominant transient influence on the flow

 March 22, 2013, 10:35 #3 New Member   Pete Drum Join Date: Sep 2012 Posts: 6 Rep Power: 6 Hey flotus1, thanks for your answer.I will try that for sure. But I have two questions about your suggestions: 1. Why would you deactivate the realizable option? I thought it generates more accurate results than the other options. 2. Could you explain how I can check the turbulence values at the inlet in a more detailed way? thank you : ) regards

 March 22, 2013, 10:44 #4 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,490 Rep Power: 25 The realizable option may produce better approximations of the flow in some cases. But if the solution doesnt converge with this option, then in my opinion the standard k-epsilon formulation still is better. We experienced similar convergence problems for the external flow around blunt bodies with the realizable option. The k-omega SST model might also be an alternative worth trying. Since you get warnings about the turbulent viscosity ratio limited in many cells, you should make sure that you didnt set unreasonably high values at the inlet. Yet it is more probable that the warning comes from cells in the wake region of the building.

 March 22, 2013, 11:09 #5 Super Moderator     Ghazlani M. Ali Join Date: May 2011 Location: Tokyo, Japan Posts: 1,382 Blog Entries: 23 Rep Power: 22 if you can provide us with some picture of your mesh ... __________________ Regards, New to ICEM CFD, try this document --> https://goo.gl/KAOIwm Ali

 March 22, 2013, 11:37 #6 New Member   Pete Drum Join Date: Sep 2012 Posts: 6 Rep Power: 6 Thanks for your answers. I will upload some pictures of my mesh wehn Im at home. regards

 March 25, 2013, 06:24 #7 New Member   Pete Drum Join Date: Sep 2012 Posts: 6 Rep Power: 6 Hi again, I gave it another try with the recommended options (realizable off, reduced URFs (momentum from 0.7 to 0.6 and pressure from 0.3 to 0.2), started with frist order then switched to second order when it converged, ) Result is looking way better than before, but there are still some jumps in the residuals. Another problem is the area weighted average velocity. It is oscillating very much. Any Ideas what I could do to obtain good results? Picture: Uploaded with ImageShack.us thank you! PS:Sorry for not uploading a picture of the mesh. I will do that today evening.

 March 25, 2013, 07:05 #8 Member   Thiagu Join Date: Oct 2012 Location: India Posts: 59 Rep Power: 6 Good progress. But need the picture of your setup. comments # Area weg. avg velocity @ which location ? # how about the overall mesh distribution # mesh distribution in wake region (where the velocity gradients are more) # for extenal flow one equation (spalart allmaras) model is preferred , but i'm not sure check in fluent recommendation. # how close the BCs and object (buliding)

 March 25, 2013, 13:26 #9 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,490 Rep Power: 25 Since you could afford 5000 Iterations in the first run, you can decrease the URFs further (0.7 to 0.6 doesnt make much difference). I recommend 0.3-0.2 for momentum and 0.1 for pressure. Additionally, you should use a first order upwind scheme for the momentum discretization. If the solution converges, you can still switch to second order from this initialization.

March 27, 2013, 11:52
#10
Senior Member

OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 13
Quote:
 started with frist order then switched to second order when it converged
Are you sure this is converged? I see a lot of fluctuation in your area-average velocities. And residuals are not monotonical.

Quote:
 for extenal flow one equation (spalart allmaras) model is preferred
Spalart–Allmaras model only solves Euler equations, instead of Navier-Stokes equations. This assumes that the viscous effects of the fluid are nullified by intertial effects (typically at very high velocities). For moderate flow rates around buildings, such assumption can prove to be significant and hence unreasonable. Although, this can be used to initialise the solution.

It may help to use first order scheme and k-epsilon model untill you see some stability. Both of these induce a much-needed diffusion to stabilise the turbulent instabilities in the initial part of solution. Once you see some stability, you can switch to second order. Also, you can explore the blended factor and choose the order of accuracy for momentum between 1 and 2(say 1.5). This should help in smooth convergence. Also, try FMG initialisation, to see if it helps.

Additionally, it is a thumb-rule to keep the addition of URFs for pressure and momentum as 1 for SIMPLE based schemes. But this is not always possible every time, as perhaps is the case here.

March 27, 2013, 12:11
#11
Senior Member

Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,490
Rep Power: 25
Quote:
 Originally Posted by oj.bulmer Additionally, it is a thumb-rule to keep the addition of URFs for pressure and momentum as 1 for SIMPLE based schemes. But this is not always possible every time, as perhaps is the case here.
I also heard of this rule, but until today, I havent come across any reasonable explanation why it should be valid. Do you know more about this?
When I reduce the URFs, i reduce both pressure and momentum simultaneously and never got into trouble because they didnt add to 1.

Quote:
 Also, you can explore the blended factor
There is a blending factor for the order of the momentum discretization in Fluent? I thought only CFX has this. Where can I find it and in which version?

Quote:
 started with frist order then switched to second order when it converged
Totally overlooked this line. Yet oj.bulmer is right, the first order solution is still far from being converged. You will need to run this for more iterations.

March 28, 2013, 16:58
#12
Senior Member

OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 13
Quote:
 I also heard of this rule, but until today, I havent come across any reasonable explanation why it should be valid. Do you know more about this?
Care for some theory? And yea, patience, this is exhaustive and enough to give good LATEX practice

Peric (Computational Methods for Fluid Dynamics) outlined an elaborate proof of this. The momentum equation can be represented as:

(1)

P being the point of interest and l being neighbouring points.

For m coefficient loops withing each timestep in SIMPLE solver, source matrices are updated as:

(2)

is latest coefficient loop value of u.

Above equation can be written as:

(3)

Or,

(4)

where

Thus we build Poisson equation for pressure and obtain that satisfies continuity equation but not momentum equation nor does the pressure. We define as (5)

The momentum equation thus becomes:

(6)

We now solve for pressure correction. It can be shown with some mathematics that

(7)

In SIMPLE, we omit and write :

(8)

Problem arises in equation equation 8. We need to use pressure under relaxation otherwise the simplifications produce overpredicted pressure. Thus we use under relaxation factor for pressure and rewrite the equation 4 for as

(9)

From equation 8 and 9:

(10)

From equation 7 and 10

(11)

Now, here comes the velocity under relaxation factor, which is introduced in momentum equation 1:

(12)

Thus (13)

with additional source term in equation 12.

We also know originally. From equation 13 with additional source term in momentum equation due to under relaxation factor, we have :

(14)

From equation 11 and 14,

Or

Hushhhhhhh!

There are many assumptions in this illustrations. Peric decided to do some trial and errors. You can read detailed analysis in his paper : ANALYSIS OF PRESSURE-VELOCITY COUPLING ON NONORTHOGONAL GRIDS.

I have attached images of study he had done for different and . According to him, was stablest for value of 0.2 for a wide range of . Differnet graphs include different configurations he did and for complex flows, the sum of the underrelaxation factors mattered.

He corrected his hypothesis later to propose that for more wider applicability, the sum of and should be 1.1!

OJ
Attached Images
 under_relaxation.jpg (71.7 KB, 45 views)

March 28, 2013, 17:08
#13
Senior Member

OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 13
Quote:
 There is a blending factor for the order of the momentum discretization in Fluent? I thought only CFX has this. Where can I find it and in which version?
Go to TUI.
Navigate to solve > set > numerics
Keep entering till you get to: "1st-order to higher-order blending factor [min=0.0 - max=1.0]: "

Here you can specify the factor. 0 means first order. 1 means second order. 0.5 means 1.5 etc. Use of blending factor will make convective fluxes more diffusive, inducing some stability. But make sure in original setting, you have specified discretization as second order.

OJ

 March 28, 2013, 20:38 #14 Senior Member   Astio Lamar Join Date: May 2012 Location: Pipe Posts: 181 Rep Power: 7 what I recommend before all, check you mesh. make sure that you have enough fine mesh. check for the skewness. If you have low quality, you will not have a converge solution. Moreover, big size variation, you will have fluctuation in the residuals.

 Thread Tools 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 On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post fayaazhussain Main CFD Forum 3 August 21, 2014 10:31 Irene FLUENT 2 February 7, 2012 12:55 Cairol FLUENT 1 July 28, 2006 01:47 Jake FLUENT 3 June 16, 2005 09:34 dave FLUENT 2 December 10, 2004 04:01