
[Sponsors] 
February 10, 2004, 10:26 
Error message: Insufficient Catalogue Size

#1 
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 

February 10, 2004, 17:19 
re: Error message: Insufficient Catalogue Size

#2 
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 

February 11, 2004, 00:56 
re: Error message: Insufficient Catalogue Size

#3 
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 

February 11, 2004, 17:01 
re: Error message: Insufficient Catalogue Size

#4 
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 CFXhelpdesk.
Pascale 

February 11, 2004, 17:20 
re: Error message: Insufficient Catalogue Size

#5 
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 

February 12, 2004, 04:39 
re: Error message: Insufficient Catalogue Size

#6 
Guest
Posts: n/a

Hello Glenn and Pascale, Thank you for your concern. I m giving the details in brief. I am simulation GasLiquid 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) Code:
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.E4 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 regards Paresh Jain Last edited by wyldckat; January 6, 2016 at 18:40. Reason: Added [CODE][/CODE] markers 

February 12, 2004, 17:14 
re: Error message: Insufficient Catalogue Size

#7 
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 

February 14, 2004, 01:31 
re: Error message: Insufficient Catalogue Size

#8 
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 

October 8, 2007, 10:58 
*** INSUFFICIENT CATALOGUE SIZE ***

#9 
Guest
Posts: n/a

Hello, have you got an idea about this error?
Slave: 3 Slave: 3 Slave: 3 ++ Slave: 3  *** INSUFFICIENT CATALOGUE SIZE ***  Slave: 3   Slave: 3  ACTION REQUIRED : Increase the file catalogue size.  Slave: 3   Slave: 3  If the situation persists please contact the CFX Customer Helpline  Slave: 3  giving the following details:  Slave: 3  Current catalogue size : 55269  Slave: 3 ++ Slave: 3  Slave: 3 Error in subroutine GET_VARELAV : Slave: 3 FCAT : Failed to get space for data area Slave: 3 GETVAR originally called by subroutine ASS_TRANS ++  ERROR #333000014 has occurred in subroutine RCVBUF.   Message:   Problems receiving a PVMbuffer from part. 3 to part. 1   > PVMerror flag from notifying missing partition: 31  ++ 

October 10, 2007, 08:43 
Re: *** INSUFFICIENT CATALOGUE SIZE ***

#10 
Guest
Posts: n/a

Increase the catalogue size by,
Catalogue Size Multiplier = 2 You can have 3,4. Insert it into solver control section using command editor. This must help. Thanks and regards. Pankaj. 

October 10, 2007, 09:54 
Re: *** INSUFFICIENT CATALOGUE SIZE ***

#11 
Guest
Posts: n/a

I have tried with catalogue size multiplier = 1.5 and it is working. So thank you very much. I keep your mail in mind. Regards. Bruyère.


August 1, 2012, 15:04 

#12 
Member

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.


August 1, 2012, 18:49 

#13 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,201
Rep Power: 103 
The def file is a binary file.
You can extract and write new CCL into the def file in CFXPre or using the cfx5cmds command. 

August 30, 2012, 23:21 

#14 
Senior Member
Join Date: Nov 2009
Posts: 125
Rep Power: 9 
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 Steadystate. 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 

August 31, 2012, 07:00 

#15 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,201
Rep Power: 103 
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.


September 2, 2012, 10:56 

#16 
Senior Member
Join Date: Nov 2009
Posts: 125
Rep Power: 9 
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 

September 4, 2012, 08:53 

#17 
Senior Member
Join Date: Nov 2009
Posts: 125
Rep Power: 9 
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 

September 5, 2012, 03:31 

#18  
Senior Member
Join Date: Nov 2009
Posts: 125
Rep Power: 9 
Quote:
Hi Glenn, do i use the command line as: cfx5solve sizecat 254k ?
__________________
Thank you for your kind attention. Kind regards, mactech001 Currently using: ANSYS v13 

September 6, 2012, 00:42 
increase cat size

#19 
Senior Member
Join Date: Nov 2009
Posts: 125
Rep Power: 9 
I've attached a screenshot of where in the Solver setting the catalogue size can be increased.
__________________
Thank you for your kind attention. Kind regards, mactech001 Currently using: ANSYS v13 

March 11, 2014, 12:40 

#20 
New Member
Join Date: Nov 2009
Posts: 10
Rep Power: 9 
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.


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
crash sHM  H25E  OpenFOAM Native Meshers: snappyHexMesh and Others  11  November 10, 2014 12:27 
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 