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

smaller timestep leads not to converge

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 10, 2011, 23:47
Question smaller timestep leads not to converge
  #1
New Member
 
Join Date: Mar 2009
Location: Dublin
Posts: 11
Rep Power: 8
vovogoal is on a distinguished road
Dear all,

I got a transient run with constant timestep 0.001s, smoothly done by CFX (ver 13.0).
Other I input BCs:
Laminar, isothermal.
inlet flowrate around 0.003 kg/s; outlet is about 10000Pa
For first two iteration , the courant number is about 200s, then reduced to the level of 50s.(I was noticed the CFX is fully implicit so greater courant number is not issue once converged. )
I monitor the outflow and inlet pressure, everything seems alright for this run.

Then I tried smaller timestep 0.0001s but the it couldn't get convergence for the first iteration.
The solver manager shows the linear solution failed in equations of U-Mom, V-Mom, and W-Mom; then fatal error, Floating point exception: Overflow.
I haven't checked the mesh yet.
I ticked the CFX-Pre->Solver control->Basic Setting->Timestep Initialisation-> Upper courant Number, and gave value to 10.
The first iteration just flow through and running and running.

I am wondering if this is right. Or there's another way around, I could use 0.0001s without divergence.

THANKS
vovogoal is offline   Reply With Quote

Old   October 11, 2011, 06:53
Default
  #2
Senior Member
 
Matthias Voß
Join Date: Mar 2009
Location: Berlin, Germany
Posts: 446
Rep Power: 11
mvoss is on a distinguished road
hey,

really not sure about that but i think it could be a problem if the time step isn´t sufficient for letting the flow pass the very first volume with given velocity.

neewbie
mvoss is offline   Reply With Quote

Old   October 11, 2011, 17:38
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,945
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You should set the outlet to 0Pa pressure and use the reference pressure to give the correct absolute pressure. Using a large outlet pressure causes large round-off errors which will get worse when you decrease the time step.

Also running double precision numerics might help.
ghorrocks is offline   Reply With Quote

Old   October 11, 2011, 23:00
Default
  #4
New Member
 
Join Date: Mar 2009
Location: Dublin
Posts: 11
Rep Power: 8
vovogoal is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
You should set the outlet to 0Pa pressure and use the reference pressure to give the correct absolute pressure. Using a large outlet pressure causes large round-off errors which will get worse when you decrease the time step.

Also running double precision numerics might help.
I am doing FSI problem, so expect having the 'real' pressure.
I almost have the run finished I will check any diffrerence between two cases(0.001s and 0.0001s)

Thanks!
vovogoal is offline   Reply With Quote

Old   October 12, 2011, 06:48
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,945
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I am no expert on FSI but I am sure it is smart enough to be able to handle a reference pressure. This is really basic stuff. And very important for exactly the reason you have found.
ghorrocks is offline   Reply With Quote

Old   October 17, 2011, 09:10
Default
  #6
Senior Member
 
Julio Mendez
Join Date: Apr 2009
Location: Greensboro, U.S.A
Posts: 108
Rep Power: 8
juliom is on a distinguished road
Send a message via Skype™ to juliom
I I were you, I would use a steady state first.
I would define the reference pressure and I would defined the outlet pressure as a relative pressure, as a Glenn said.
Besides, I would start as a Steady state with and Auto time scale = 1 (conservative), and let the program to make some iteration, as a result you will get an "accurate" time step.
After you del with steady jump to transient....
Good luck!!
juliom is offline   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
Restart 2-way FSI with different timestep? Lance CFX 11 April 17, 2013 00:37
IcoFsiFoam simulation crashes when using a smaller timestep mathieu OpenFOAM Running, Solving & CFD 1 May 17, 2009 03:54
interTrackFoam timestep virginie_e OpenFOAM Running, Solving & CFD 4 April 6, 2009 05:02
Smaller time step leads to divergence? Feidao Li FLUENT 0 January 22, 2009 13:32
Use of Timestep in obtaining solution. hagupta CFX 7 February 28, 2006 14:14


All times are GMT -4. The time now is 11:52.