CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > Siemens > STAR-CCM+

Residual Divergence Issue In Convective Fan Cooling Simulation

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

Like Tree2Likes
  • 1 Post By fluid23
  • 1 Post By LuckyTran

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 27, 2020, 21:03
Default Residual Divergence Issue In Convective Fan Cooling Simulation
  #1
New Member
 
CT
Join Date: Feb 2020
Posts: 1
Rep Power: 0
JulianH is on a distinguished road
Hello everybody, I hope you're having a great day.

Overview:
I am running a simulation in STARCCM+ to determine if fan cooling will be powerful enough to cool an electric car battery. The battery and two fans are contained in a case with room for air to flow around the battery. Holes are on either side of the case act as inlets and outlets (real world inlets and outlets as opposed to those set up in the regions portion of the simulation) for air to flow in the z-direction. The whole case, battery and fans are contained in a larger fluid volume.

Mesh:
I am using surface mesher, polyhedral mesher, and prism layer mesher. A custom control has increased mesh resolution to a fixed 1.5 mm within the battery case and the cells grow outside the case towards the boundaries of the encasing fluid region. 8.5 million cells in total. Cell skewness is less than .5. Cell quality could stand to be improved. There are a handful (200 or so) of particularly bad cells near the fan blades.

Physics:
I am running 3D, steady, coupled energy, coupled flow, constant density, and K-e turbulence.

Regions:
There is a main fluid region that was made by subtracting the case, batteries, and fans from a block. I've set heat flux generated on the surface of the batteries equal 1200 W/m^2K. Two rotating regions are contained within the large fluid region that are located around the fan blades. They are set to 5500 rpm. I have stagnation inlets and pressure outlets on all three regions and there are interfaces between the fluid region and the rotating regions.

My Problem:
I run the solution and it looks good until the 33rd iteration and then the turbulent kinetic energy, z-momentum, and turbulent dissipation rate residuals spike up drastically and stay up for 3000 more iterations at which point, the solution is cancelled. The temperature on the batteries never settles at a fixed value. I'm not sure what is causing the solution to diverge and any insight would be GREATLY appreciated. It may just be that I need to really work on the mesh some more but I have a feeling its the physics models since I've never worked with turbulence before. If it is the mesh, is there any way I can correlate which cells are causing the residuals to spike at 33 iterations in? Thank you so much for your replies. Let me know if you need any more information!
JulianH is offline   Reply With Quote

Old   February 28, 2020, 11:16
Default
  #2
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17
fluid23 is on a distinguished road
A few thoughts:

1. If you know that your mesh needs improvement, make it so.

2. How are you initializing the solution? With coupled solver you can use the expert initialization option. It usually does a decent job.

3. Early instability can be improved using a courant number ramp. Assuming that you haven't changed it from the default setting of 5. Try ramping from 0.1 to 5 over 500 iterations. There is an option for this under solvers > coupled implicit.

4. You can find high residual cells, but it is a little involved. There are better discussions of this on Steve Portal, but basically you will need to turn on 'temporary storage retained' under solvers > coupled implicit and solvers > k-e Turbulence. Then step your solution 1 iteration and create a derived part > threshold inside of a geometry scene. Change the mode to 'outside' and query the range. Reduce the upper/lower limits of the range by 5% and hit apply. You will then see the cells with the highest residuals.

5. Also, don't get hung up on trying to find a steady solution. If none of this brings your residuals below 10^-3 then you might need to consider an unsteady simulation.
JulianH likes this.
fluid23 is offline   Reply With Quote

Old   February 28, 2020, 12:52
Default
  #3
Senior Member
 
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,636
Rep Power: 65
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Check the maximum skewness angle and make sure it's less than 89 degrees, less than 80 would be even better.


It's probably a poor guess for the initial condition. You can provide better initial conditions or baby the solution. One way to verify the initial conditions are the problem is to change all your boundary conditions to be consistent with the BC's, i.e. make everything pressure inlet/outlets at the same pressure so that there is no flow.



Quote:
Originally Posted by JulianH View Post
If it is the mesh, is there any way I can correlate which cells are causing the residuals to spike at 33 iterations in? Thank you so much for your replies. Let me know if you need any more information!

Go to solvers, click on the equation, and click the check box to enable temporary storage. If you 1 iteration after enabling this option, you willhave access to the fields used by the solver, including the corrections. Plot those.
JulianH likes this.
LuckyTran is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Maximum number of iterations exceeded chtmultiregionsimpleFoam Moncef OpenFOAM Running, Solving & CFD 28 July 13, 2020 15:26
pressure in incompressible solvers e.g. simpleFoam chrizzl OpenFOAM Running, Solving & CFD 13 March 28, 2017 06:49
Cannot run the code properly: very large time step continuity error crst15 OpenFOAM Running, Solving & CFD 9 December 14, 2014 19:17
Micro Scale Pore, icoFoam gooya_kabir OpenFOAM Running, Solving & CFD 2 November 2, 2013 14:58
Orifice Plate with a fully developed flow - Problems with convergence jonmec OpenFOAM Running, Solving & CFD 3 July 28, 2011 06:24


All times are GMT -4. The time now is 11:14.