CFD Online Logo CFD Online URL
Home > Forums > STAR-CCM+

Fluid Flow over a bus -- Convergence Problem

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

LinkBack Thread Tools Display Modes
Old   May 11, 2016, 13:52
Default Fluid Flow over a bus -- Convergence Problem
New Member
Roberto J.
Join Date: Mar 2016
Posts: 2
Rep Power: 0
Roberto J. is on a distinguished road
Hi everyone.

I am am relatively new to CFD and I am hoping to get some advice with my current project. I have model air flow around a passenger bus and determine separation points. Essentially a rectangular box with wheels. the bus is 110mm wide, 126mm high and 487mm long.

I have modeled it using the following models:
All y + Wall treatment
SST K-Omega
K-Omega Turbulence
Constant Density
Segregated flow

I used a polyhedral mesh with 12 layer 3mm prism layer which gives y+ values of between 0-1. The number of cells is around 470 000 with a base size of 5 mm.

However when I run it after 3 hours and 600 iterations it doesn't seem to converge. The velocity inlet condition was set at 120kph. Is there anyway I can improve my convergence? I have attached my residual results and Cd results
Roberto J. is offline   Reply With Quote

Old   May 11, 2016, 15:52
Senior Member
kevin alun
Join Date: Sep 2011
Location: Germany
Posts: 106
Rep Power: 7
marmot is on a distinguished road
If you are going for a y+ <1 you should use the low Re approach not the all Y+ approach.

Looking at your residuals, its not great but one could live with that convergence, you always need to look at other variables like you did with drag, I would say drag is your main indicator for convergence,
marmot is offline   Reply With Quote

Old   May 12, 2016, 13:05
Senior Member
Join Date: Aug 2014
Posts: 605
Rep Power: 8
MBdonCFD is on a distinguished road
This is almost certainly an unsteady flow (due to separation) which is why you are seeing such poor convergence. Switch your physics models from steady to implicit unsteady and set your inner iteration stopping criteria to 100, at least to start with. You may eventually need to play around with different time steps (keeping your largest CFL number below 5-10 if time and resources allow). Assuming you don't have mesh issues then you will see your residuals drop, then spike and drop off again at each new time step.

Your turbulence model selection is appropriate. K-W SST is good for separated flows. The use of a low-Re model doesn’t make sense with K-W since there is no such thing as a low-Re k-w model. There are low-Re damping parameters already built into the model which you can adjust, but I do not recommend doing so. The use of the all wall y+ approach simply gives you flexibility to leave some wall boundary meshes coarse while refining others that may be more important to you while maintaining some level of accuracy. In general, k-w sst works best with y+ around 1.
MBdonCFD is offline   Reply With Quote


bus, convergence, star ccm+

Thread Tools
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 On
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
convergence problem with compressible flow sarah l FLUENT 0 July 1, 2015 15:47
Waterwheel shaped turbine inside a pipe simulation problem mshahed91 CFX 3 January 10, 2015 12:19
convergence problem in 2D steady supersonic flow sehs15 FLUENT 4 November 6, 2014 08:06
Problem with Convergence (Over flow) armlic CFX 4 July 14, 2014 04:48
Convergence Problem in Axisymmetric Periodic Flow atheresia FLUENT 3 February 10, 2014 04:00

All times are GMT -4. The time now is 11:09.