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

overflow c fpx handler error

Register Blogs Community New Posts Updated Threads Search

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 15, 2016, 06:14
Default overflow c fpx handler error
  #1
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 313
Rep Power: 13
Martin_Sz is on a distinguished road
Hello everyone
I have problem with my simulation. I have multiphase flow air and nh3 at stp.
If I have 50 mm diameter of outlet (opening boundary) my simulation goes on. If I have 20 mm diameterr of outlet I have error overflow. What can I change to run this simulation with smaller outlet (diameter)??
I need to have opening because I need to have fluid flow to domain by opening boundary (I have pressure difference between opening and domain - 1 bar).
Attached Images
File Type: png domain with opening and inlet.png (9.2 KB, 12 views)
__________________
Quick Tips and Tricks, Tutorials FLuent/ CFX (CFD)
https://howtooansys.blogspot.com/
Martin_Sz is offline   Reply With Quote

Old   June 15, 2016, 06:19
Default
  #2
Senior Member
 
Join Date: Jul 2011
Location: Berlin, Germany
Posts: 173
Rep Power: 15
monkey1 is on a distinguished road
What is the exact error you are getting?
What are you exactly simulating? Transient? Steady state?

If your errore is
Quote:
"Floating point exception: Overflow"
maybe this might help you already:
http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F
monkey1 is offline   Reply With Quote

Old   June 15, 2016, 06:28
Default
  #3
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 313
Rep Power: 13
Martin_Sz is on a distinguished road
transient simulation
840 s with step 1 s
__________________
Quick Tips and Tricks, Tutorials FLuent/ CFX (CFD)
https://howtooansys.blogspot.com/
Martin_Sz is offline   Reply With Quote

Old   June 15, 2016, 06:52
Default
  #4
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 313
Rep Power: 13
Martin_Sz is on a distinguished road
If i define outlet on outlet simulation goes on.
__________________
Quick Tips and Tricks, Tutorials FLuent/ CFX (CFD)
https://howtooansys.blogspot.com/
Martin_Sz is offline   Reply With Quote

Old   June 15, 2016, 08:35
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,871
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
You have answered 1 of Monkey1's questions. The others are "What is the exact error you are getting? What are you exactly simulating?". We can't help you until you answer these questions.
ghorrocks is offline   Reply With Quote

Old   June 15, 2016, 08:54
Default
  #6
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 313
Rep Power: 13
Martin_Sz is on a distinguished road
Multiflow
On inlet I define nh3 gas. On domain I have air. On outlet I defined opening boundary with 1 bar relative pressure. If i decrease diameter of outlet from 50 mm to 20 mm I get error overflow c fpx handler nothing else.
I define isothermal/sst/ solvers.
__________________
Quick Tips and Tricks, Tutorials FLuent/ CFX (CFD)
https://howtooansys.blogspot.com/
Martin_Sz is offline   Reply With Quote

Old   June 15, 2016, 08:55
Default
  #7
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 313
Rep Power: 13
Martin_Sz is on a distinguished road
FLOW: Flow Analysis 1
&replace DOMAIN: Default Domain
Coord Frame = Coord 0
Domain Type = Fluid
Location = B23
BOUNDARY: Default Domain Default
Boundary Type = WALL
Create Other Side = Off
Interface Boundary = Off
Location = F24.23,F26.23,F27.23,F28.23,F30.23
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: Opening
Boundary Type = OPENING
Interface Boundary = Off
Location = Outlet
BOUNDARY CONDITIONS:
FLOW DIRECTION:
Option = Normal to Boundary Condition
END
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Opening Pressure and Direction
Relative Pressure = 1 [bar]
END
TURBULENCE:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
FLUID: Fluid 1
BOUNDARY CONDITIONS:
VOLUME FRACTION:
Option = Value
Volume Fraction = 1
END
END
END
FLUID: amoniak
BOUNDARY CONDITIONS:
VOLUME FRACTION:
Option = Value
Volume Fraction = 0
END
END
END
END
BOUNDARY: inlet
Boundary Type = INLET
Interface Boundary = Off
Location = Inlet
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Normal Speed = 4.78 [m s^-1]
Option = Normal Speed
END
TURBULENCE:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
FLUID: Fluid 1
BOUNDARY CONDITIONS:
VOLUME FRACTION:
Option = Value
Volume Fraction = 0
END
END
END
FLUID: amoniak
BOUNDARY CONDITIONS:
VOLUME FRACTION:
Option = Value
Volume Fraction = 1
END
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Option = Non Buoyant
END
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 1 [bar]
END
END
FLUID DEFINITION: Fluid 1
Material = Air at 25 C
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID DEFINITION: amoniak
Material = NH3 at STP
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Fluid Temperature = 360 [C]
Homogeneous Model = On
Option = Isothermal
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = SST
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
END
END
FLUID PAIR: Fluid 1 | amoniak
INTERPHASE TRANSFER MODEL:
Interface Length Scale = 1. [mm]
Option = Mixture Model
END
MASS TRANSFER:
Option = None
END
END
INITIALISATION:
Option = Automatic
FLUID: Fluid 1
INITIAL CONDITIONS:
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = 1
END
END
END
FLUID: amoniak
INITIAL CONDITIONS:
VOLUME FRACTION:
Option = Automatic with Value
Volume Fraction = 0
END
END
END
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic with Value
U = 0 [m s^-1]
V = 0 [m s^-1]
W = 0 [m s^-1]
END
STATIC PRESSURE:
Option = Automatic with Value
Relative Pressure = 0 [bar]
END
TURBULENCE INITIAL CONDITIONS:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
END
MULTIPHASE MODELS:
Homogeneous Model = On
FREE SURFACE MODEL:
Option = None
END
END
END
END
__________________
Quick Tips and Tricks, Tutorials FLuent/ CFX (CFD)
https://howtooansys.blogspot.com/
Martin_Sz is offline   Reply With Quote

Old   June 15, 2016, 09:12
Default
  #8
Senior Member
 
Join Date: Jul 2011
Location: Berlin, Germany
Posts: 173
Rep Power: 15
monkey1 is on a distinguished road
First: Why are you using a multiphase model?
At 360°C NH3 and Air are gaseous and could just be treated as "variable composition mixture" single phase.

Second (although maybe not that relevant): you define Air at 25°C as your substance but you want to use it for a domain temperature of 360°C? You should switch to air ideal gas.

Third: You are mixing 2 gases at quite high temperatures, shouldn't you take into account the bouyancy?

Fourth:
Glenn may correct me if I'm wrong but you define at your opening
Quote:
Option = Opening Pressure and Direction
Relative Pressure = 1 [bar]
Isn't that meaning that you have an overpressure OUTSIDE of your domain of 1 bar?
Meaning if your pressure inside is below 1 bar + reference pressure you will get no outflow?!?
monkey1 is offline   Reply With Quote

Old   June 15, 2016, 09:12
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,871
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
You have a fundamental error. You are modelling a mixture of 2 gases with a multiphase model. But you only have one phase as everything is gas! So you are using the wrong physical model. You should be using a multicomponent model which is the appropriate model for a mixture of gases.

Also you should make your reference pressure 2 bar and the outlet pressure 0 bar. This will minimise round off errors.
ghorrocks is offline   Reply With Quote

Old   June 15, 2016, 09:23
Default
  #10
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 313
Rep Power: 13
Martin_Sz is on a distinguished road
OK So I use multiphase flow to determine nh3 fraction in domain
on initialization on domain is only air
on inlet only nh3
On outlet i give higher pressure than on domain because I need to have nonlinear flux of air from opening into domain.

So my question is any tutorial similar to my case if not which solvers do i need to choose to determine nh3 fraction on domain over time??
Best regards
__________________
Quick Tips and Tricks, Tutorials FLuent/ CFX (CFD)
https://howtooansys.blogspot.com/
Martin_Sz is offline   Reply With Quote

Old   June 15, 2016, 09:47
Default
  #11
Senior Member
 
Join Date: Jul 2011
Location: Berlin, Germany
Posts: 173
Rep Power: 15
monkey1 is on a distinguished road
You do not need multiphase to get the repartition of the substance in the domain.
You have only ONE phase = the gaseous phase
This one is compsed of several gases of varying fraction = variable composition mixture
And for each gas you can define separate Initial conditions, boundary conditions and will get for each substance the fractions in the domain!

For a first idea what I am talking about have a look at the "Reacting Flow in a mixing tube" Tutorial, and just ignore the reaction part, to understand how to to define such a variable composition mixture.
monkey1 is offline   Reply With Quote

Old   June 16, 2016, 07:50
Default
  #12
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 313
Rep Power: 13
Martin_Sz is on a distinguished road
Hey
I change to single phase flow with mixture of air and nh3 ideal gases.
So I have the same problem like before. Overflow If I give higher pressure on opening boundary that on the domain . Difference must be 1 bar between outlet and domain.

I need (on overall description of the problem) pump up tank from 0.01 bar to 1 bar with amonium nh3 with little holes (leaks) of air for example 20 mm diameter hole. Tank has 1300 mm doiameter and 1000 mm long.,
__________________
Quick Tips and Tricks, Tutorials FLuent/ CFX (CFD)
https://howtooansys.blogspot.com/
Martin_Sz is offline   Reply With Quote

Reply

Tags
ansys, ansys cfx, c fpx handler, overflow, workbench


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
[blockMesh] blockMesh with double grading. spwater OpenFOAM Meshing & Mesh Conversion 92 January 12, 2019 10:00
Compile calcMassFlowC aurore OpenFOAM Programming & Development 13 March 23, 2018 08:43
DPM udf error haghshenasfard FLUENT 0 April 13, 2016 07:35
Compile problem ivanyao OpenFOAM Running, Solving & CFD 1 October 12, 2012 10:31
ParaView for OF-1.6-ext Chrisi1984 OpenFOAM Installation 0 December 31, 2010 07:42


All times are GMT -4. The time now is 03:47.