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

Please Help.....Insufficient Catalogue Size

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

Like Tree4Likes
  • 2 Post By mactech001
  • 2 Post By Marvin

Reply
 
LinkBack Thread Tools Display Modes
Old   February 10, 2004, 10:26
Default Please Help.....Insufficient Catalogue Size
  #1
Paresh Jain
Guest
 
Posts: n/a
Hi friends, i m new user of cfx 5.6 while running a simulation with multiple subdomains, i m getting the following error. please guide me how to solve this.

*** INSUFFICIENT CATALOGUE SIZE *** | | Action required : Increase the file catalogue size. | If the situation persists please contact the CFX Customer Helpline | | giving the following details:- | | Current catalogue size: 78925

i tried running this simulations many times. all the time it gave the same error but the detailes of error were different all the times like

Details of error:- 1. Error detected by routine MAKLNK COLDNM = /FLOW/PHYSICS/ZN1 CNEWNM = /FLOW/GETVAR/PHYS_ZONE_DIR CRESLT = FCAT

2.Error detected by routine MAKLNK CDANAM = CELIWRK CDTYPE = INTR ISIZE = 4 CRESLT = FCAT

please help me. i will be highly thankful to u all.

Sincerely waiting for some help this time.

Paresh Jain
  Reply With Quote

Old   February 10, 2004, 17:19
Default Re: Please Help.....Insufficient Catalogue Size
  #2
Glenn Horrocks
Guest
 
Posts: n/a
Hi Paresh,

Try increasing the memory available to the solver. In solver manager, click on "Show Advanced Controls", then the Solver tab, and increase the number in the solver allocation factor. By default it is 1, try increasing it by 20% (or whatever increase is required to make it work!). You can increase it by 20% by entering "1.2x".

Glenn
  Reply With Quote

Old   February 11, 2004, 00:56
Default Re: Please Help.....Insufficient Catalogue Size
  #3
Paresh Jain
Guest
 
Posts: n/a
Hello Glenn, i tried increasing the memory allocation factor for solver to as much as 10 but its not working. The simulation starts for 1st iteration and then gives the same error. What may be the cause of this error ? and how can it be solved ?

Thanks in Advance for ur help.

Sincere Regards Paresh Jain
  Reply With Quote

Old   February 11, 2004, 17:01
Default Re: Please Help.....Insufficient Catalogue Size
  #4
Pascale Fonteijn
Guest
 
Posts: n/a
Something physically is incorrect in your simulation. It could be anything. Thus, please provide more info to this global helpdesk or consult you local CFX-helpdesk.

Pascale
  Reply With Quote

Old   February 11, 2004, 17:20
Default Re: Please Help.....Insufficient Catalogue Size
  #5
Glenn Horrocks
Guest
 
Posts: n/a
Hi Paresh,

I think Pascale is right. There is something wrong in the setup of your simulation. We might be able to work out the problem if you can show us your output file (Try not to make it too big for the web - only put the relevant bits if it is large).

Glenn
  Reply With Quote

Old   February 12, 2004, 04:39
Default Re: Please Help.....Insufficient Catalogue Size
  #6
Paresh Jain
Guest
 
Posts: n/a
Hello Glenn and Pascale, Thank you for your concern. I m giving the details in brief. I am simulation Gas-Liquid Reaction in a Packed Bed Reactor.

Domain cylinder L=0.3 m, D=0.2 m, Liquidphase+Gasphse Gasphase (dispersed phase D=0.005 m) liquidphase (continuous phase)

Liquidphase= X (transport equation) + S (constraint) Gasphase= CO2, O2, Water Vap at 25 C (transport equations) + N2 (constraint)

Reaction is 2S + 0.8 O2 ==> X + 1.1 H2O + CO2

Based on the physics and reaction in particular, i am using 10 subdomains to define sink and source terms in the continuity equation of the phases and inturn for species involved in reaction. I think the problem is with these many number of subdomains only. (though i have set the environmental variable GTM_BETA_ALLOW_SUBDOMAIN_OVERLAP=1, in Pre it gives BLUE colored error that u have used same region more than once but still it allows to write .def file. But solver does exit after 1st iteration. So please look into the problem. I am providing you some part of .out file. (domain detail, boundary conditions, 3 subdomains, solver parameters)

MATERIAL : S Liquid Density = 700 [kg m^-3] Molar Mass = 30 [kg kmol^-1] MATERIAL : X Liquid Density = 1000 [kg m^-3]Molar Mass = 21.8 [kg kmol^-1]

EXECUTION CONTROL :

PARTITIONER STEP CONTROL :

Runtime Priority = Standard

MEMORY CONTROL :

Memory Allocation Factor = 1

END

END

SOLVER STEP CONTROL :

Runtime Priority = Standard

EXECUTABLE SELECTION :

Double Precision = Off

Use 64 Bit = Off

END

MEMORY CONTROL :

Memory Allocation Factor = 5

END

PARALLEL ENVIRONMENT :

Option = Serial

Parallel Mode = PVM

FLOW :

SIMULATION TYPE : Transient

TIME DURATION :

Option = Total Time

Timesteps = 0.2 [s]

Total Time = 10 [s]

END

END

DOMAIN : PBR

Coord Frame = Coord 0

Domain Type = Fluid

Fluids List = Gasphase,Liquidphase

Location = PBR

DOMAIN MODELS :

BUOYANCY MODEL :

Buoyancy Reference Density = 1.17 [kg m^-3]

Gravity X Component = 0 [m s^-2]

Gravity Y Component = 0 [m s^-2]

Gravity Z Component = -9.81 [m s^-2]

Option = Buoyant

END

DOMAIN MOTION :

Option = Stationary

END

REFERENCE PRESSURE :

Reference Pressure = 101325 [Pa]

FLUID MODELS :

HEAT TRANSFER MODEL :

Option = Thermal Energy

TURBULENCE MODEL :

Homogeneous Model = Off

Option = Fluid Dependent

END

END

MASS TRANSFER :

Option = None

END

MOMENTUM TRANSFER :

DRAG FORCE :

Option = Schiller Naumann

END

TURBULENT DISPERSION FORCE :

Option = None

END

END TURBULENCE TRANSFER :

ENHANCED TURBULENCE PRODUCTION MODEL :

Option = None

END

END

END

FLUID : Gasphase

TURBULENCE MODEL :

Option = Dispersed Phase Zero Equation FLUID : Liquidphase

TURBULENCE MODEL :

Option = k epsilon

END

TURBULENT WALL FUNCTIONS :

Option = Scalable

MULTIPHASE MODELS :

Homogeneous Model = Off

FREE SURFACE MODEL :

Option = None

END

END

SUBDOMAIN : SubCO2

FLUID : Gasphase

SOURCES :

EQUATION SOURCE : continuity

Option = Fluid Mass Source

Source = 1*rxnrate*Gasphase.CO2.mw

VARIABLE : CO2.mf

Option = Value

Value = 1.0 [m m^-1]

END

VARIABLE : T

Option = Value

Value = Liquidphase.T

END

BOUNDARY : in

Boundary Type = INLET

Location = in

BOUNDARY CONDITIONS :

FLOW REGIME :

Option = Subsonic

END

HEAT TRANSFER :

Option = Fluid Dependent

END

MASS AND MOMENTUM :

Option = Fluid Velocity

END

END

FLUID : Gasphase

BOUNDARY CONDITIONS :

COMPONENT : CO2

Mass Fraction = 0.0

Option = Mass Fraction

END

COMPONENT : O2

Mass Fraction = 0.23

Option = Mass Fraction

END

COMPONENT : Water Vapour at 25 C

Mass Fraction = 0.0

Option = Mass Fraction

END

HEAT TRANSFER :

Option = Static Temperature

Static Temperature = 310 [K]

END

VELOCITY :

Normal Speed = 0.3 [m s^-1]

Option = Normal Speed

END

VOLUME FRACTION :

Option = Value

Volume Fraction = 1

END

END

END

FLUID : Liquidphase

BOUNDARY CONDITIONS :

COMPONENT : X

Mass Fraction = 0.005

Option = Mass Fraction

END

HEAT TRANSFER :

Option = Static Temperature

Static Temperature = 310 [K]

END

TURBULENCE :

Option = Low Intensity and Eddy Viscosity Ratio

END

VELOCITY :

Normal Speed = 0 [m s^-1]

Option = Normal Speed

END

VOLUME FRACTION :

Option = Value

Volume Fraction = 0

END

END

END

END

BOUNDARY : PBR Default

Boundary Type = WALL

Location = Solid 1.3,Solid 1.4

BOUNDARY CONDITIONS :

HEAT TRANSFER :

Option = Fluid Dependent

END

WALL ROUGHNESS :

Option = Smooth Wall

END

END

FLUID : Gasphase

BOUNDARY CONDITIONS :

HEAT TRANSFER :

Fixed Temperature = 298 [K]

Option = Fixed Temperature

END

WALL INFLUENCE ON FLOW :

Option = Free Slip

END

END

END

FLUID : Liquidphase

BOUNDARY CONDITIONS :

HEAT TRANSFER :

Fixed Temperature = 298 [K]

Option = Fixed Temperature

END

WALL INFLUENCE ON FLOW :

Option = No Slip

END

END

END

WALL CONTACT MODEL :

Option = Use Volume Fraction

END

END

BOUNDARY : out

Boundary Type = OUTLET

Location = out

BOUNDARY CONDITIONS :

FLOW REGIME :

Option = Subsonic

END

MASS AND MOMENTUM :

Option = Degassing Condition

END

END

END

SUBDOMAIN : SubX

FLUID : Liquidphase

EQUATION SOURCE : continuity

Option = Fluid Mass Source

Source = rxnrate*Liquidphase.X.mw

VARIABLE : T

Option = Value

Value = Liquidphase.T

END

VARIABLE : X.mf

Option = Value

Value = 1.0 [m m^-1]

END

EQUATION SOURCE : energy

Option = Source

Source =rxnrate*Liquidphase.X.mw*heatofrxn

END

SUBDOMAIN : SubWaterVap

FLUID : Gasphase

EQUATION SOURCE : continuity

Option = Fluid Mass Source

Source = 1.1*rxnrate*Gasphase.Water Vapour at 25 C.mw

VARIABLE : T

Option = Value

Value = Liquidphase.T

END

VARIABLE : Water Vapour at 25 C.mf

Option = Value

Value = 1.0 [m m^-1]

END

SUBDOMAIN : SubS

FLUID : Liquidphase

EQUATION SOURCE : continuity

Option = Fluid Mass Source

Source = -2*rxnrate*Liquidphase.S.mw/Liquidphase.S.mf

VARIABLE : T

Option = Value

Value = Liquidphase.T

END

VARIABLE : X.mf

Option = Value

Value = 0.0 [m m^-1]

END

INITIALISATION :

Option = Automatic

FLUID : Gasphase

INITIAL CONDITIONS :

Velocity Type = Cylindrical

COMPONENT : CO2

Mass Fraction = 0.0

Option = Automatic with Value

END

COMPONENT : O2

Mass Fraction = 0.23

Option = Automatic with Value

END

COMPONENT : Water Vapour at 25 C

Mass Fraction = 0.0

Option = Automatic with Value

END

CYLINDRICAL VELOCITY COMPONENTS :

Axis Type = Coordinate Axis

Option = Automatic with Value

Rotation Axis = Coord 0.3

Velocity Axial Component = 0.3 [m s^-1]

Velocity Theta Component = 0 [m s^-1]

Velocity r Component = 0.0001 [m s^-1]

END

TEMPERATURE :

Option = Automatic with Value

Temperature = 308 [K]

END

VOLUME FRACTION :

Option = Automatic with Value

Volume Fraction = 0.3

END

END

END

FLUID : Liquidphase

INITIAL CONDITIONS :

Velocity Type = Cylindrical

COMPONENT : X

Mass Fraction = 0.005

Option = Automatic with Value

END

CYLINDRICAL VELOCITY COMPONENTS :

Axis Type = Coordinate Axis

Option = Automatic with Value

Rotation Axis = Coord 0.3

Velocity Axial Component = 0 [m s^-1]

Velocity Theta Component = 0 [m s^-1]

Velocity r Component = 0 [m s^-1]

END

EPSILON :

Option = Automatic

END

K :

Option = Automatic

END

TEMPERATURE :

Option = Automatic with Value

Temperature = 308 [K]

END

VOLUME FRACTION :

Option = Automatic with Value

Volume Fraction = 0.7

END

END

END

INITIAL CONDITIONS :

STATIC PRESSURE :

Option = Automatic with Value

Relative Pressure = 0 [Pa]

END

END

END

SOLVER CONTROL :

ADVECTION SCHEME :

Option = Upwind

END

CONVERGENCE CONTROL :

Maximum Number of Coefficient Loops = 18

END

CONVERGENCE CRITERIA :

Residual Target = 1.E-4

Residual Type = RMS

END

TRANSIENT SCHEME :

Option = First Order Backward Euler

END

END END COMMAND FILE :

Version = 5.6

Results Version = 5.6 END

**********SOLVER******************* Memory Allocated for Run (Actual usage may be less ) DataType Kwords Words/Node Words/Elem Kbytes Byte/Node Real 37861.2 1500.82 275.28 147895.5 6003.29 Integer 8205.4 325.26 59.66 32052.4 1301.05 Character 3663.3 145.21 26.63 3577.4 145.21 Logical 72.0 2.85 0.52 281.3 11.42 Double 1124.1 4.56 8.17 8782.0 356.48

Total Number of Nodes, Elements, and Faces Total Number of Nodes = 25227 Total Number of Elements =137538 Total Number of Tetrahedrons =137538 Total Number of Faces = 6380

*** INSUFFICIENT CATALOGUE SIZE *** Action required : Increase the file catalogue size If the situation persists please contact the CFX Customer Helpline Current catalogue size: 53707
  Reply With Quote

Old   February 12, 2004, 04:39
Default Re: Please Help.....Insufficient Catalogue Size
  #7
Paresh Jain
Guest
 
Posts: n/a
Hello Glenn and Pascale, Thank you for your concern. I m giving the details in brief. I am simulation Gas-Liquid Reaction in a Packed Bed Reactor.

Domain cylinder L=0.3 m, D=0.2 m, Liquidphase+Gasphse Gasphase (dispersed phase D=0.005 m) liquidphase (continuous phase)

Liquidphase= X (transport equation) + S (constraint) Gasphase= CO2, O2, Water Vap at 25 C (transport equations) + N2 (constraint)

Reaction is 2S + 0.8 O2 ==> X + 1.1 H2O + CO2

Based on the physics and reaction in particular, i am using 10 subdomains to define sink and source terms in the continuity equation of the phases and inturn for species involved in reaction. I think the problem is with these many number of subdomains only. (though i have set the environmental variable GTM_BETA_ALLOW_SUBDOMAIN_OVERLAP=1, in Pre it gives BLUE colored error that u have used same region more than once but still it allows to write .def file. But solver does exit after 1st iteration. So please look into the problem. I am providing you some part of .out file. (domain detail, boundary conditions, 3 subdomains, solver parameters)

MATERIAL : S Liquid Density = 700 [kg m^-3] Molar Mass = 30 [kg kmol^-1] MATERIAL : X Liquid Density = 1000 [kg m^-3]Molar Mass = 21.8 [kg kmol^-1]

EXECUTION CONTROL :

PARTITIONER STEP CONTROL :

Runtime Priority = Standard

MEMORY CONTROL :

Memory Allocation Factor = 1

END

END

SOLVER STEP CONTROL :

Runtime Priority = Standard

EXECUTABLE SELECTION :

Double Precision = Off

Use 64 Bit = Off

END

MEMORY CONTROL :

Memory Allocation Factor = 5

END

PARALLEL ENVIRONMENT :

Option = Serial

Parallel Mode = PVM

FLOW :

SIMULATION TYPE : Transient

TIME DURATION :

Option = Total Time

Timesteps = 0.2 [s]

Total Time = 10 [s]

END

END

DOMAIN : PBR

Coord Frame = Coord 0

Domain Type = Fluid

Fluids List = Gasphase,Liquidphase

Location = PBR

DOMAIN MODELS :

BUOYANCY MODEL :

Buoyancy Reference Density = 1.17 [kg m^-3]

Gravity X Component = 0 [m s^-2]

Gravity Y Component = 0 [m s^-2]

Gravity Z Component = -9.81 [m s^-2]

Option = Buoyant

END

DOMAIN MOTION :

Option = Stationary

END

REFERENCE PRESSURE :

Reference Pressure = 101325 [Pa]

FLUID MODELS :

HEAT TRANSFER MODEL :

Option = Thermal Energy

TURBULENCE MODEL :

Homogeneous Model = Off

Option = Fluid Dependent

END

END

MASS TRANSFER :

Option = None

END

MOMENTUM TRANSFER :

DRAG FORCE :

Option = Schiller Naumann

END

TURBULENT DISPERSION FORCE :

Option = None

END

END TURBULENCE TRANSFER :

ENHANCED TURBULENCE PRODUCTION MODEL :

Option = None

END

END

END

FLUID : Gasphase

TURBULENCE MODEL :

Option = Dispersed Phase Zero Equation FLUID : Liquidphase

TURBULENCE MODEL :

Option = k epsilon

END

TURBULENT WALL FUNCTIONS :

Option = Scalable

MULTIPHASE MODELS :

Homogeneous Model = Off

FREE SURFACE MODEL :

Option = None

END

END

SUBDOMAIN : SubCO2

FLUID : Gasphase

SOURCES :

EQUATION SOURCE : continuity

Option = Fluid Mass Source

Source = 1*rxnrate*Gasphase.CO2.mw

VARIABLE : CO2.mf

Option = Value

Value = 1.0 [m m^-1]

END

VARIABLE : T

Option = Value

Value = Liquidphase.T

END

BOUNDARY : in

Boundary Type = INLET

Location = in

BOUNDARY CONDITIONS :

FLOW REGIME :

Option = Subsonic

END

HEAT TRANSFER :

Option = Fluid Dependent

END

MASS AND MOMENTUM :

Option = Fluid Velocity

END

END

FLUID : Gasphase

BOUNDARY CONDITIONS :

COMPONENT : CO2

Mass Fraction = 0.0

Option = Mass Fraction

END

COMPONENT : O2

Mass Fraction = 0.23

Option = Mass Fraction

END

COMPONENT : Water Vapour at 25 C

Mass Fraction = 0.0

Option = Mass Fraction

END

HEAT TRANSFER :

Option = Static Temperature

Static Temperature = 310 [K]

END

VELOCITY :

Normal Speed = 0.3 [m s^-1]

Option = Normal Speed

END

VOLUME FRACTION :

Option = Value

Volume Fraction = 1

END

END

END

FLUID : Liquidphase

BOUNDARY CONDITIONS :

COMPONENT : X

Mass Fraction = 0.005

Option = Mass Fraction

END

HEAT TRANSFER :

Option = Static Temperature

Static Temperature = 310 [K]

END

TURBULENCE :

Option = Low Intensity and Eddy Viscosity Ratio

END

VELOCITY :

Normal Speed = 0 [m s^-1]

Option = Normal Speed

END

VOLUME FRACTION :

Option = Value

Volume Fraction = 0

END

END

END

END

BOUNDARY : PBR Default

Boundary Type = WALL

Location = Solid 1.3,Solid 1.4

BOUNDARY CONDITIONS :

HEAT TRANSFER :

Option = Fluid Dependent

END

WALL ROUGHNESS :

Option = Smooth Wall

END

END

FLUID : Gasphase

BOUNDARY CONDITIONS :

HEAT TRANSFER :

Fixed Temperature = 298 [K]

Option = Fixed Temperature

END

WALL INFLUENCE ON FLOW :

Option = Free Slip

END

END

END

FLUID : Liquidphase

BOUNDARY CONDITIONS :

HEAT TRANSFER :

Fixed Temperature = 298 [K]

Option = Fixed Temperature

END

WALL INFLUENCE ON FLOW :

Option = No Slip

END

END

END

WALL CONTACT MODEL :

Option = Use Volume Fraction

END

END

BOUNDARY : out

Boundary Type = OUTLET

Location = out

BOUNDARY CONDITIONS :

FLOW REGIME :

Option = Subsonic

END

MASS AND MOMENTUM :

Option = Degassing Condition

END

END

END

SUBDOMAIN : SubX

FLUID : Liquidphase

EQUATION SOURCE : continuity

Option = Fluid Mass Source

Source = rxnrate*Liquidphase.X.mw

VARIABLE : T

Option = Value

Value = Liquidphase.T

END

VARIABLE : X.mf

Option = Value

Value = 1.0 [m m^-1]

END

EQUATION SOURCE : energy

Option = Source

Source =rxnrate*Liquidphase.X.mw*heatofrxn

END

SUBDOMAIN : SubWaterVap

FLUID : Gasphase

EQUATION SOURCE : continuity

Option = Fluid Mass Source

Source = 1.1*rxnrate*Gasphase.Water Vapour at 25 C.mw

VARIABLE : T

Option = Value

Value = Liquidphase.T

END

VARIABLE : Water Vapour at 25 C.mf

Option = Value

Value = 1.0 [m m^-1]

END

SUBDOMAIN : SubS

FLUID : Liquidphase

EQUATION SOURCE : continuity

Option = Fluid Mass Source

Source = -2*rxnrate*Liquidphase.S.mw/Liquidphase.S.mf

VARIABLE : T

Option = Value

Value = Liquidphase.T

END

VARIABLE : X.mf

Option = Value

Value = 0.0 [m m^-1]

END

INITIALISATION :

Option = Automatic

FLUID : Gasphase

INITIAL CONDITIONS :

Velocity Type = Cylindrical

COMPONENT : CO2

Mass Fraction = 0.0

Option = Automatic with Value

END

COMPONENT : O2

Mass Fraction = 0.23

Option = Automatic with Value

END

COMPONENT : Water Vapour at 25 C

Mass Fraction = 0.0

Option = Automatic with Value

END

CYLINDRICAL VELOCITY COMPONENTS :

Axis Type = Coordinate Axis

Option = Automatic with Value

Rotation Axis = Coord 0.3

Velocity Axial Component = 0.3 [m s^-1]

Velocity Theta Component = 0 [m s^-1]

Velocity r Component = 0.0001 [m s^-1]

END

TEMPERATURE :

Option = Automatic with Value

Temperature = 308 [K]

END

VOLUME FRACTION :

Option = Automatic with Value

Volume Fraction = 0.3

END

END

END

FLUID : Liquidphase

INITIAL CONDITIONS :

Velocity Type = Cylindrical

COMPONENT : X

Mass Fraction = 0.005

Option = Automatic with Value

END

CYLINDRICAL VELOCITY COMPONENTS :

Axis Type = Coordinate Axis

Option = Automatic with Value

Rotation Axis = Coord 0.3

Velocity Axial Component = 0 [m s^-1]

Velocity Theta Component = 0 [m s^-1]

Velocity r Component = 0 [m s^-1]

END

EPSILON :

Option = Automatic

END

K :

Option = Automatic

END

TEMPERATURE :

Option = Automatic with Value

Temperature = 308 [K]

END

VOLUME FRACTION :

Option = Automatic with Value

Volume Fraction = 0.7

END

END

END

INITIAL CONDITIONS :

STATIC PRESSURE :

Option = Automatic with Value

Relative Pressure = 0 [Pa]

END

END

END

SOLVER CONTROL :

ADVECTION SCHEME :

Option = Upwind

END

CONVERGENCE CONTROL :

Maximum Number of Coefficient Loops = 18

END

CONVERGENCE CRITERIA :

Residual Target = 1.E-4

Residual Type = RMS

END

TRANSIENT SCHEME :

Option = First Order Backward Euler

END

END END COMMAND FILE :

Version = 5.6

Results Version = 5.6 END

**********SOLVER******************* Memory Allocated for Run (Actual usage may be less ) DataType Kwords Words/Node Words/Elem Kbytes Byte/Node Real 37861.2 1500.82 275.28 147895.5 6003.29 Integer 8205.4 325.26 59.66 32052.4 1301.05 Character 3663.3 145.21 26.63 3577.4 145.21 Logical 72.0 2.85 0.52 281.3 11.42 Double 1124.1 4.56 8.17 8782.0 356.48

Total Number of Nodes, Elements, and Faces Total Number of Nodes = 25227 Total Number of Elements =137538 Total Number of Tetrahedrons =137538 Total Number of Faces = 6380

*** INSUFFICIENT CATALOGUE SIZE *** Action required : Increase the file catalogue size If the situation persists please contact the CFX Customer Helpline Current catalogue size: 53707

i hope this helps.

regards Paresh Jain
  Reply With Quote

Old   February 12, 2004, 17:14
Default Re: Please Help.....Insufficient Catalogue Size
  #8
Juan Carlos
Guest
 
Posts: n/a
Hi,

This is not an insufficient memory problem, but catalogue size problem..

From the Solver Manager, edit your definition file (Tools/Edit Definition File) and add the Catalogue Size Multiplier parameter within the FLOW/SOLVER CONTROL section.

Use a real value, like 1.2 or higher until the solver manages.. Otherwise, contact your local CFX representative..

Hope this helps, let us know if it works, Juan Carlos
  Reply With Quote

Old   February 14, 2004, 01:31
Default Re: Please Help.....Insufficient Catalogue Size
  #9
Paresh Jain
Guest
 
Posts: n/a
Hi Juan, Glenn, Pascale and friends, as rightly pointed out by Juan, the problem was not insufficient memory but was insufficient catalogue size. so i tried the suggestion given by Juan..and it worked....i just added following parameter in Solver Control section of .def file

Catalogue Size Multiplier = 2.0

Thanks again for all ur help. regards Paresh Jain
  Reply With Quote

Old   August 1, 2012, 15:04
Default
  #10
Member
 
Join Date: Jan 2012
Location: Indiana, USA
Posts: 84
Rep Power: 5
Torque_Converter is on a distinguished road
Send a message via AIM to Torque_Converter
What kind of editor can access the .def file properly? So far it opens as giberish and in CFX there doesn't seem to be a function for the modification of the .def.
Torque_Converter is offline   Reply With Quote

Old   August 1, 2012, 18:49
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,929
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The def file is a binary file.

You can extract and write new CCL into the def file in CFX-Pre or using the cfx5cmds command.
ghorrocks is offline   Reply With Quote

Old   August 30, 2012, 23:21
Default
  #12
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
Hi Juan,

when i tried this, i was prompted that:

No New parameters can be added to the /FLOW:Flow Analysis 1/SOLVER CONTROL section of the CFX Command File.

Is there something else i need to setup please?

my simulation run works with no complaints of catalogue size with Steady-state. But when i run Transient, this catalogue size error message appears.

i'm using CFX v13.
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13

Last edited by mactech001; August 30, 2012 at 23:26. Reason: to add more info
mactech001 is offline   Reply With Quote

Old   August 31, 2012, 07:00
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,929
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If it asks for more catalog size then use the approach above to increase it. If you have to make the catalog size really big then you have some other problem, probably a complex GGI interface or convergence problem.
ghorrocks is offline   Reply With Quote

Old   September 2, 2012, 10:56
Default
  #14
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
Hi Glenn, thanks for your response.
i wanted to try the approach above to increase it, but my problem is, CFX prompted me that i can't add parameters anymore with the following message:

No New parameters can be added to the /FLOW:Flow Analysis 1/SOLVER CONTROL section of the CFX Command File.

Is it a setup problem or installation problem would you think?

regards,
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   September 4, 2012, 08:53
Default
  #15
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
would the following error msg mean anything please?
Fatal error generated in gKVxEl_ZN
Message :- FCAT:- Unable to create work space LINK_LIST
gKVxEl_ZN called by :- gKVxEl_ZN
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   September 5, 2012, 03:31
Default
  #16
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
The def file is a binary file.

You can extract and write new CCL into the def file in CFX-Pre or using the cfx5cmds command.

Hi Glenn,

do i use the command line as:

cfx5solve -size-cat 254k ?
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   September 6, 2012, 00:42
Default increase cat size
  #17
Senior Member
 
Join Date: Nov 2009
Posts: 125
Rep Power: 7
mactech001 is on a distinguished road
I've attached a screenshot of where in the Solver setting the catalogue size can be increased.
Attached Images
File Type: jpg cfx catsize.jpg (98.0 KB, 177 views)
j-avdeev and edward.pocock like this.
__________________
Thank you for your kind attention.

Kind regards,
mactech001
Currently using: ANSYS v13
mactech001 is offline   Reply With Quote

Old   March 11, 2014, 12:40
Default
  #18
New Member
 
Join Date: Nov 2009
Posts: 10
Rep Power: 7
Marvin is on a distinguished road
Just to mention that this error can also occur at the interpolation phase of the simulation. Even, for example, when starting the simulation from a current solution onto identical mesh. In this case, increase the catalogue size on the "Interpolator" tab of the solver manager.
Chander and edward.pocock like this.
Marvin 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
critical error during installation of openfoam Fabio88 OpenFOAM Installation 21 June 2, 2010 03:01
OF 1.6 | Ubuntu 9.10 (64bit) | GLIBCXX_3.4.11 not found piprus OpenFOAM Installation 22 February 25, 2010 14:43
Phase locked average in run time panara OpenFOAM 2 February 20, 2008 15:37
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
Error Message: INSUFFICIENT CATALOGUE SIZE ahlo CFX 2 December 14, 2007 16:59


All times are GMT -4. The time now is 00:29.