impot .inp file to abaqus???help emergency

[sabuy]

hi friends
can anybody help me to solve this problem that i can not import this .inp file to abaqus?
the error is parametrized.i am trying to replace the real value, but the abaqus siad that :
WARNING: The following keywords/parameters are not yet supported by the input file reader:
---------------------------------------------------------------------------------
*CONTACTOUTPUT, MASTER, SLAVE"

please help me. the inp file is here:

*HEADING
3D Double cantilever beam test model
- use vcct *debond to model crack growth
orthogonal mesh, short run
**
**preprint,model=yes,history=yes,contact=yes
**Restart, Write
**
*parameter
** User input data defining the interface properties
** Fracture toughness (N/mm):
GIc = 1.2
GIIc = 6.0
GIIIc = 6.0
** B-K parameter:
eta = 1.75
modeMixLaw=3
** mixed mode parameter
am = 1.0
an=1.5
ao=1.0
** Damage and tolerance parameters
damv=0
**5.0e-5
tol=0.1
width=12.7
*NODE
1, 0.0, 0.0
11, 0.0, 1.0
51, 0.0, 0.0
61, 0.0, 1.0
**
**
9001, 4.5, 0.0
9011, 4.5, 1.0
9051, 4.5, 0.0
9061, 4.5, 1.0
**
18001, 9.0, 0.0
18011, 9.0, 1.0
18051, 9.0, 0.0
18061, 9.0, 1.0
**
*NGEN,NSET=NS1
1 , 9001, 100
51 , 9051, 100
9001 ,18001, 100
9051 ,18051, 100
*NGEN,NSET=NS2
11 , 9011, 100
61 , 9061, 100
9011 ,18011, 100
9061 ,18061, 100
**
*NFILL
NS1,NS2,10,1
**
**
*element,type=S4
20001, 1, 101, 102, 2
20051,51, 151, 152,52
**
*ELGEN,ELSET=lower_elements
20001, 180,100,100, 10, 1,1
*ELGEN,ELSET=upper_elements
20051, 180,100,100, 10, 1,1
**
**
*Shell Section, elset=upper_elements, material=MAT_upper,Orientation=Or1
0.2,
**
*Shell Section, elset=lower_elements, material=MAT_lower,Orientation=Or1
0.2,
**
*Orientation,Name=Or1
1.0, 0.0, 0.0, 0.0, 1.0, 0.0
3, 0.0
**
*MATERIAL,NAME=MAT_upper
*ELASTIC,TYPE=ENGINEERING CONSTANTS
8000000.0,8000000.0,8000000.0, 0.0, 0.0, 0.0,4000000.0,4000000.0,
4000000.0,
**
*MATERIAL,NAME=MAT_lower
*ELASTIC,TYPE=ENGINEERING CONSTANTS
8000000.0,8000000.0,8000000.0, 0.0, 0.0, 0.0,4000000.0,4000000.0,
4000000.0,
*elset,elset=slave,generate
20101,37901,100
20102,37902,100
20103,37903,100
20104,37904,100
20105,37905,100
20106,37906,100
20107,37907,100
20108,37908,100
20109,37909,100
20110,37910,100
*surface,type=element,name=slave
slave,SPOS
*surface,type=element,name=master
upper_elements,SNEG
*ELSET,ELSET=ETIED,GENERATE
29101,37901,100
29102,37902,100
29103,37903,100
29104,37904,100
29105,37905,100
29106,37906,100
29107,37907,100
29108,37908,100
29109,37909,100
29110,37910,100
*NSET,NSET=NTIED,ELSET=ETIED
*initial conditions, type=contact
slave, master,ntied
*Contact Pair, interaction=SURFS, small sliding, type=NODE TO SURFACE, no thickness
slave, master
*Surface Interaction, name=SURFS
1.,
*Friction, slip tolerance=0.005
0.,
*clearance,slave=slave,master=master,value=1.0E-8
*NSET,NSET=FIX,GENERATE
**18001, 18011
18051, 18061
*BOUNDARY
FIX,1,6
**
**
*MPC
BEAM, 1, 6
BEAM, 2, 6
BEAM, 3, 6
BEAM, 4, 6
BEAM, 5, 6
BEAM, 7, 6
BEAM, 8, 6
BEAM, 9, 6
BEAM,10, 6
BEAM,11, 6
**
BEAM, 51, 56
BEAM, 52, 56
BEAM, 53, 56
BEAM, 54, 56
BEAM, 55, 56
BEAM, 57, 56
BEAM, 58, 56
BEAM, 59, 56
BEAM, 60, 56
BEAM, 61, 56
**
**
*NSET, NSET=LP
6, 56
**
*************************************************************************************
**
**
** STEP: Step-1
**
** STEP: Step-1
**
*STEP, INC=1000
**,nlgeom
**
*STATIC,direct
0.107, 0.214
*debond, slave=slave, master=master
*FRACTURE CRITERION,TYPE=VCCT,MIXED MODE BEHAVIOR=REEDER,TOLERANCE=<tol>
<GIc>, <GIIc>, <GIIIc>, <eta>
*CONTROLS,PARAMETERS=TIME INCREMENTATION
, , , , , , , 10,
*BOUNDARY
**
6,3,3, -0.107
56,3,3, 0.107
**
**
**print,contact=yes
** OUTPUT REQUESTS
**
**Output, field, variable=PRESELECT
**Output, history, variable=PRESELECT
**NODE PRINT,NSET=LP
** U3, RF3
**
**
**output, field,freq=2
**node output
**u
**contact output,slave=slave,master=master
**sdv
*Output, history,freq=1
*NODE output,NSET=LP
U3, RF3
**energy output,var=all
*End Step
*STEP, INC=1000
**,nlgeom
**
*STATIC
**,stabilize=1.0E-8
0.001, 0.086,1.0E-8,0.002
**debond, slave=slave, master=master
**FRACTURE CRITERION,TYPE=VCCT,MIXED MODE BEHAVIOR=REEDER,TOLERANCE=<tol>
**<GIc>, <GIIc>, <GIIIc>, <eta>
*CONTROLS,PARAMETERS=TIME INCREMENTATION
, , , , , , , 10,
*BOUNDARY
**
6,3,3, -0.15
56,3,3, 0.15
**
**
**print,contact=yes
** OUTPUT REQUESTS
**
**Output, field, variable=PRESELECT
**Output, history, variable=PRESELECT
***NODE PRINT,NSET=LP
**U3, RF3
**
**
*output, field,freq=10
*element output
s
*node output
u
*contact output,slave=slave,master=master
dbt,dbsf,dbs,openbc,crsts,enrrt,efenrrtr,bdstat
*Output, history,freq=1
*NODE output,NSET=LP
U3, RF3
**energy output,var=all
*End Step

 

[vandergram]

Hi,

There is some keywords that are not supported in abaqus cae. If this parameter *CONTACTOUTPUT, MASTER, SLAVE" is a required parameter of your analysis. You just need to launch the analysis using the abaqus command instead of importing the inp file.
To do this: choose abaqus command, then type this:
abaqus job=your_file.inp
Make sure that the inp file is in the work directory of abaqus.

 

[sabuy]

hi dear Vandergram
i have try this way"abaqus command" but the file is not work correctly and we have some errors:
WARNING: The input file contains one or more data items which have been parameterized. Parameterized input files can not yet be imported into Abaqus/CAE. This occurred while scanning input file for parameterized data. The input file will not be imported.
what should i do?

 

[Dave442]

The warning messages tell you exactly what is causing your problem.

"WARNING: The input file contains one or more data items which have been parameterized. Parameterized input files can not yet be imported into Abaqus/CAE. This occurred while scanning input file for parameterized data. The input file will not be imported."

You have defined a number of parameters at the start of your input file:

** Fracture toughness (N/mm):
GIc = 1.2
GIIc = 6.0
GIIIc = 6.0
** B-K parameter:
eta = 1.75
modeMixLaw=3
** mixed mode parameter
am = 1.0
an=1.5
ao=1.0
** Damage and tolerance parameters
damv=0
**5.0e-5
tol=0.1
width=12.7

Some of these parameters are used later in the input file. Parameterized input files cannot be imported into CAE. You could remove the parameters defined at the start of the input file and instead use the numeric values directly. Alternatively, as vandergram suggested, you can bypass CAE and submit your job from the command line by opening a command window, navigating to the working directory and typing: abaqus job=yourfile.inp.

Good Luck,
Dave

 

[sabuy]

thank u so much dear Dave442
but when i replace the parametrize values, the problem does not solve.
i import the file from command to abaqus,but in job we have some problems.
i am trying to solve the problems.please see the file attached.
thanks

 

[Dave442]

If you want help you need to describe the problem/error you have encountered.

 

[sabuy]

here is the errors;
*CONTACTOUTPUT, MASTER, SLAVE
The model "3d" has been imported from an input file.
Please scroll up to check for error and warning messages.

i do not know what the problem is. because i replaced the values.

 

[Dave442]

In the second step of your analysis you request contact output:

*contact output,slave=slave,master=master

When you import your .inp file it tells you that this keyword is not supported by CAE:

WARNING: The following keywords/parameters are not yet supported by the input file reader:
---------------------------------------------------------------------------------
*CONTACTOUTPUT, MASTER, SLAVE"

If you remove this from the input file it opens in CAE without any warnings, but you will need to redefine your contact output for step 2.

Alternatively, launch your analysis from the command line as we have suggested a number of times.

 

[sabuy]

thank u so much.
my problems solved.
Good Luck