CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Temperature blowup for with 6-DOF falling object

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 16, 2005, 00:39
Default Temperature blowup for with 6-DOF falling object
  #1
Andrew Wick
Guest
 
Posts: n/a
I am modeling an object falling through air using the dynamic mesh function and the 6-DOF solver. It works perfectly for an incompressible flow, but when I attempt to turn on the energy equation, the temperature diverges between 0.3 and 1 second of flow time. I am using Piso with Non-Iterative time advancement.

There is one grid point on the body surface with a temperature of 1 and another with a very large temperature. This causes the solution to diverge. I've tried changing the timestep, the under-relaxation factors, the grid, the convective schemes, and this always pops up. The object's BC's are adiabatic walls. When I switch to isothermal, this still pops up, only its later in time and a few grid points away from the body.

Anyone run into this problem before or can offer some insight?
  Reply With Quote

Old   October 16, 2005, 03:47
Default Re: Temperature blowup for with 6-DOF falling obje
  #2
Razvan
Guest
 
Posts: n/a
There are be three possible problems:

- some dynamic mesh settings which do not work anymore when the object accelerates over some specific velocity; you shold try (if you did not already...) to remesh every 2-3 time steps and also use sizing functions and set "spring factor to 0.5

- you did not specify a rigid grid zone around the object; this is VERY important because high gradients near the wall could lead to solution instability if grid is bad (high skewness)- the best way is to make a BL, at least 7-8 layers and specify this region as rigid, with 6DOF passive and same CG as the body

- try disabling "skewness and neighbour coupling" and if this is not enough, disable "neighbour correction" too - this was the answer to my own problem some time ago (store release) where I was stuck with a "floating point error" something like 0.4 seconds after launching.

Also, if none of this solves your problem, go back to iterative solver. It could be your only chance.

Best regards, Razvan
  Reply With Quote

Old   October 16, 2005, 12:48
Default Re: Temperature blowup for with 6-DOF falling obje
  #3
Andrew Wick
Guest
 
Posts: n/a
Razvan,

Thank you for your reply.

I do have a rigid zone around the object and I am remeshing every timestep. The blowup is occuring within the rigid zone around the object, very far away from any remeshing that is occuring. The interesting thing is that if I specify the object's motion with a profile, the temperature never diverges. It's only with the 6-DOF.

I tried turning off neighbor correction, but that only led to divergence earlier. There is no "skewness and neighbour coupling" with the NITA option, so I could not change this. I might have to iterate, but that will take much longer than NITA.

I did notice that I am not specifying the rigid zone as a passive body. Changing the surrounding zones to passive did not fix the problem though. What exactly does this option do?

Thanks,

Andrew
  Reply With Quote

Old   October 16, 2005, 15:56
Default Re: Temperature blowup for with 6-DOF falling obje
  #4
Jason
Guest
 
Posts: n/a
I'm not sure if this will fix the problem, but you may want to set the temperature and pressure limits to prevent the values from going to the extremes. The default limits of 1K to 5000K, and 1Pa to 50000000000Pa are a bit extreme... when's the last time you had a situation where you made it all the way down to 1K?

Solve=>Controls=>Limits

I recommend calculating your max/min temperatures and pressures then adding a "buffer" because the solution will have to go outside of the realistic range some, but not to the extent of the default range. Typically for the pressure range I will calculate the dynamic pressure (if you're falling I would use the maximum dynamic pressure you'd expect at terminal velocity... or some estimation of your terminal velocity) and I use the maximum pressure as Static + (2 or 3)*Dynamic, and my minimum pressure as Static - (3 or 4)*Dynamic. Then I estimate temperatures at these pressures (any compressible flow book will give you the equations or a table representing total pressures and temperatures to Mach number and static values).

May not fix the problem, but I've seen stranger things happen!

Hope this helps, and good luck, Jason
  Reply With Quote

Reply

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
Error compiling OpenFOAM-1.6-ext Canesin OpenFOAM Installation 136 April 25, 2012 11:22
Force can not converge colopolo CFX 13 October 4, 2011 22:03
How to show the transient case? H.P.LIU Phoenics 7 July 13, 2010 04:31
Compilation error OF1.5-dev on Suse10.3 darenyang OpenFOAM Installation 0 April 29, 2009 04:55
BlockMeshmergePatchPairs hjasak OpenFOAM Native Meshers: blockMesh 11 August 15, 2008 07:36


All times are GMT -4. The time now is 05:25.