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

Solver: Fatal Bounds error detected

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 23, 2006, 10:31
Default Solver: Fatal Bounds error detected
  #1
hagupta
Guest
 
Posts: n/a
I get this error after about 600 iterations and the solver stops.

Fatal bounds error detected. HF.Specific heat capacity at constant volume Location: <my domain name>

I have defined Cp(T) for HF manually using an expression and an user function. The Cp values are right.

My problem consists of a "Reacting Mixture" consisting of 4 gases and 1 solid. Out of these, the solid and a gas(HF) are formed after the reaction.

What could be wrong? What do I need to check? Thank you in anticipation.
  Reply With Quote

Old   March 23, 2006, 12:21
Default Re: Solver: Fatal Bounds error detected
  #2
opaque
Guest
 
Posts: n/a
Dear hagupta,

The solver is stopping because your expression resolves to a negative value.. Are you sure that your expression resolve to positive values for any positive temperature? Perhaps the solver under/over shoots the range of your expression for temperature.

Have you tried plotting your expression in CFX-Pre ?

Good luck, Opaque
  Reply With Quote

Old   March 23, 2006, 13:43
Default Re: Solver: Fatal Bounds error detected
  #3
hagupta
Guest
 
Posts: n/a
For Cp of HF, I had defined a user function (ie: entered the Cp values at different temperatures starting from 0K). then an expression was defined. And yes, I have plotted the expression for Cp.

As per the error I am getting, does it mean that Cv=Cp-R for HF evaluates to a negative value??

I have also ticked the option for EXTEND MIN/MAX in the user function and given a wide range of temperature in the TABLE GENERATION option in the material properties tab for HF. Anyways, I will again have a look at the Cp values and will increase the range of temperatures for the TABLE GENERATION option when I will get back to CFX tomorrow.

Thanks for your support. I will get back soon.
  Reply With Quote

Old   March 24, 2006, 08:16
Default Re: Solver: Fatal Bounds error detected
  #4
hagupta
Guest
 
Posts: n/a
I had entered HF Cp as 0 at 0K. I deleted this value. Now this error has vanished.

But now I am getting errors like "newtons method failed to converge in 200 iterations........ Variable: Total Pressure................" However, the run is not stopping.

Any idea of the consequences of such a message?
  Reply With Quote

Old   March 24, 2006, 08:56
Default Re: Solver: Fatal Bounds error detected
  #5
hagupta
Guest
 
Posts: n/a
The exact error I am getting is posted on this link.

http://tp-txdp4281.content-type.com/...o+converge.JPG
  Reply With Quote

Old   March 24, 2006, 11:17
Default Re: Solver: Fatal Bounds error detected
  #6
opaque
Guest
 
Posts: n/a
Dear hagupta,

The conversion from total pressure to static pressure requires a very delicated consistency between enthalpy and entropy. The formula to compute enthalpy and entropy are a function of temperature, pressure and specific heat capacity. Recall that for variable specific heat the total to static pressure conversion is not trivial since it requires integration.

Expression for specific heat capacity must satisfy certain conditions, as well as which are the reference state for enthalpy, entropy and their reference temperatures.

Have you run your case using constant specific heat capacity? If it does well, have you tried any other of the supplied option for specific heat capacity? If that still goes well, you should look more into your Cp definition..

Good luck, Opaque

  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
smoothSolver diverges - solution in using PBiCG solver? makaveli_lcf OpenFOAM Running, Solving & CFD 3 September 11, 2013 12:44
Quarter Burner mesh with periosic condition SamCanuck FLUENT 2 August 31, 2011 11:34
desperate Fatal overflow in linear solver - transient kingjewel1 CFX 9 January 5, 2010 14:53
Setting a B.C using UserFortran in 4.3 tokai CFX 10 July 17, 2001 16:25
Error during Solver cfd guy CFX 4 May 8, 2001 06:04


All times are GMT -4. The time now is 12:49.