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

ERROR #001100279 has occurred in subroutine ErrActio

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 18, 2011, 08:59
Default ERROR #001100279 has occurred in subroutine ErrActio
  #1
New Member
 
Bobby
Join Date: Dec 2010
Posts: 21
Rep Power: 6
tomcatbobby is on a distinguished road
Hi

I could use some help with an error I am getting in CFX.

| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Floating point exception: Overflow

Details of error:-
----------------
Error detected by routine POPDIR
CRESLT = ILEG

I have no idea why I am having this error but it is driving me insane! I have seen many forum posts for this type of error but none of the solutions solve my problem.

I am trying to model a simple problem of natural convection in a room. The room is a box with walls set as adiabatic. Inside the room is a heater raised off the floor with a static temperature. The fluid is air at 25 degrees C with buoyancy enabled and no turbulence (laminar).

Any ideas.

Thanks
tomcatbobby is offline   Reply With Quote

Old   January 18, 2011, 19:11
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,814
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
It means your simulation is diverging. You need to improve numerical stability - better mesh quality, smaller timesteps, better initial conditions, start off with first order discretisation, check the physics is correct.

In your case is your simulation steady state? If so what is the heat source (you said it is a heater), and what is the heat sink?
ghorrocks is offline   Reply With Quote

Old   January 18, 2011, 21:21
Default
  #3
New Member
 
Bobby
Join Date: Dec 2010
Posts: 21
Rep Power: 6
tomcatbobby is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
It means your simulation is diverging. You need to improve numerical stability - better mesh quality, smaller timesteps, better initial conditions, start off with first order discretisation, check the physics is correct.

In your case is your simulation steady state? If so what is the heat source (you said it is a heater), and what is the heat sink?
Ok, I can appreciate those considerations. In terms of yours questions I have been trying to keep the problem as simple as possible. Mesh default size is set to 100, no timesteps, no initial conditions, not sure about where to set first order discretisation within CFX?

Heat source is effectively a box at a constant temperature of 145 degrees C. So as far as know, it is unsteady and a transient solution is required...but....my limited knowledge of CFD was telling me run a steady state analysis first so that the transient solution had some results to start with? There is no heat sink at the moment (but I want to add this later), all I want to do at the moment is moniter the room as it gets hotter and hotter.

Am welcome to any suggestions and fully accept what im doing could be completely wrong, I have only started learning CFD this year.

Thanks
tomcatbobby is offline   Reply With Quote

Old   January 18, 2011, 21:26
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,814
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You are never going to get convergence using a steady state model on a model which is not steady state. If you put a heater in a room with adiabatic walls, it is going to slowly heat up as time progress. This means there is no steady state so of course it diverges.

You could say that the steadys state result is the entire room at the heater temperature and no flow, but the steady state solver will have a hard tiem getting there as the initial condition is so far from the final result.

So I would forget the steady state bit and just start off with a transient run.
ghorrocks is offline   Reply With Quote

Old   January 18, 2011, 21:31
Default
  #5
New Member
 
Bobby
Join Date: Dec 2010
Posts: 21
Rep Power: 6
tomcatbobby is on a distinguished road
Thanks for the reply. This is very helpful. I have tried to run transient analysis in the past and have become confused by which timesteps to use?

I was referred to here for choosing them

http://my.fit.edu/itresources/manual...ug/node572.htm

in particular, equations 13.2-21 and 13.2-22.

How do I know my length and velocity scales?

Thanks
tomcatbobby is offline   Reply With Quote

Old   January 18, 2011, 21:45
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,814
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The best way to set time step size when you are doign new work is to use adaptive timestepping, targetting 3-5 coeff loops per iteration (assuming a single phase simulation). Then let the solver find the timestep size itself.
ghorrocks is offline   Reply With Quote

Old   January 19, 2011, 09:24
Default
  #7
New Member
 
Bobby
Join Date: Dec 2010
Posts: 21
Rep Power: 6
tomcatbobby is on a distinguished road
ok I changed to transient solution and used adaptive settings but am still getting the overflow error? I think its because of the initial conditions are not enough but I dont know why? I have set an (t0) initialisation criteria to 0velocity in all directions, pressure the same as the reference pressure and a temperature of 10 degrees c?

What am I missing?

Thanks
tomcatbobby is offline   Reply With Quote

Old   January 19, 2011, 20:27
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,814
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Are you sure your initial conditions are sensible? If so then try starting with a smaller timestep.
ghorrocks is offline   Reply With Quote

Old   January 19, 2011, 20:30
Default
  #9
New Member
 
Bobby
Join Date: Dec 2010
Posts: 21
Rep Power: 6
tomcatbobby is on a distinguished road
Tried smaller timestep and a smaller mesh today and yet its still a no go. Either an overflow error or and invalid number error.

Inititial conditions are as follows (by initial, I clicked the global initialisation button)

Velocity= 0 in all directions.

Pressure=same as reference pressure=atm

Temperature=15 degrees centigrade.

Thanks
tomcatbobby is offline   Reply With Quote

Old   January 19, 2011, 21:39
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,814
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
What is your timestep? I bet your timestep is still too large.

Also you are running a laminar model on a flow which is almost certainly turbulent. That will also cause convergence problems.

Please post your CCL.
ghorrocks is offline   Reply With Quote

Old   January 20, 2011, 15:56
Default
  #11
New Member
 
Bobby
Join Date: Dec 2010
Posts: 21
Rep Power: 6
tomcatbobby is on a distinguished road
Yes I have been selecting laminar for two reasons. Thought it would keep the problem simple and also as flow initially has 0 velocity in all directions. I figured the flow would be turbulent anyway.

I've exported my CCL but how do i get it onto the post?

Thanks
tomcatbobby is offline   Reply With Quote

Old   January 20, 2011, 16:10
Default
  #12
New Member
 
Bobby
Join Date: Dec 2010
Posts: 21
Rep Power: 6
tomcatbobby is on a distinguished road
Here it is.

Just delete the .txt at the end. wouldnt let me load a .ccl.
Attached Files
File Type: txt room&heater.ccl.txt (18.4 KB, 18 views)
tomcatbobby is offline   Reply With Quote

Old   January 20, 2011, 17:21
Default
  #13
New Member
 
Bobby
Join Date: Dec 2010
Posts: 21
Rep Power: 6
tomcatbobby is on a distinguished road
Ok i changed the reference pressure for the domain and the initialisation to 1 atm. This meant that the run continued without any errors. Havent checked results yet though. Im sure i have made mistakes in my setup anyway so would you mind checking the CCL anyway.

Thanks
tomcatbobby is offline   Reply With Quote

Old   January 20, 2011, 21:19
Default
  #14
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,814
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Check your adaptive time stepping settings. You are currently doing the first update after one minute, should be after the first timestep. Also your initial timestep and minimum timestep are invalid.
ghorrocks is offline   Reply With Quote

Old   January 20, 2011, 21:22
Default
  #15
New Member
 
Bobby
Join Date: Dec 2010
Posts: 21
Rep Power: 6
tomcatbobby is on a distinguished road
Can you elobrate, how are they invalid? How do i set the first update to be after the first timestep?

Other than that is it ok?

Thanks for your help on this.
tomcatbobby 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
ERROR #001100279 has occurred in subroutine ErrAction alinik Main CFD Forum 0 July 3, 2010 08:11
ERROR #001100279 has occurred in subroutine ErrAction. P9408 CFX 1 August 19, 2009 07:56
ERROR #001100279 has occurred in subroutine ErrAct Mohamed Musthafa CFX 0 September 29, 2005 08:41
ERROR #001100279 has occurred in subroutine ErrAct Carl CFX 2 July 16, 2005 14:39
ERROR #004100018 has occurred in subroutine FINMES San Chang CFX 1 May 26, 2004 18:30


All times are GMT -4. The time now is 21:49.