Defining a unique material for each element in ABAQUS through a .inp file 1

[Kuba_707]

Hello,
I'm currently trying to assign a unique material for each element of my FEM-calculation in ABAQUS. What I have is a .inp file, where every important definition is made, and its working fine if I'm assigning one Material for all elements. But as soon as I want to assign a individual material for each element I get an error message saying :

***ERROR: Problem when parsing keyword: MATERIAL Invalid parameter:
*ELASTIC. The parameter may be misspelled, obsolete, or invalid.
***NOTE: DUE TO AN INPUT ERROR THE ANALYSIS PRE-PROCESSOR HAS BEEN UNABLE TO
INTERPRET SOME DATA. SUBSEQUENT ERRORS MAY BE CAUSED BY THIS OMISSION

***ERROR: Problem when parsing keyword: MATERIAL Invalid parameter:
*ELASTIC. The parameter may be misspelled, obsolete, or invalid.

***ERROR: Problem when parsing keyword: MATERIAL Invalid parameter:
*ELASTIC. The parameter may be misspelled, obsolete, or invalid.
%%%%%%%% This continues for a few times %%%%%%%%
***ERROR: No more (non-fatal) errors will be reported ...

***ERROR: in keyword *DENSITY, file "ZS1.1E_214x722_loadDriv.pes", line
308336: The keyword is misplaced. It can be suboption for the
following keyword(s)/level(s): material

What I did in the Masters.inp is to add the following lines:

*ELEMENT, TYPE=S4R, ELSET=all_elements,INPUT=<elementfile>
*TRANSFORM, TYPE=C, NSET=all_nodes
0., 0., 0., 0., 0., 1.
*ORIENTATION, SYSTEM=C, NAME=OID11
0., 0., 0., 0., 0., 1.
1, 90.
*MATERIAL,NAME=MAT1,
*ELASTIC, TYPE=LAMINA
<E1_1>, <E2_1>, <nue>, <G12_1>, <G13_1>, <G23_1>
*Density
<rho>
*MATERIAL,NAME=MAT2,
*ELASTIC, TYPE=LAMINA
<E1_2>, <E2_2>, <nue>, <G12_2>, <G13_2>, <G23_2>
*Density
<rho>
...
*ELSET, ELSET=SHELL1
1
*SHELL SECTION, ELSET=SHELL1, MATERIAL=MAT1
*ELSET, ELSET=SHELL2
2
*SHELL SECTION, ELSET=SHELL2, MATERIAL=MAT2
...

The values for the single properties like E1_2 are in a seperate .inp file which is loaded at the begining of the Masters.inp, as well as the node.txt and the element.txt which are defining the nodes and elements.

Is someone able to help me? If some informations are missing please tell me, I tried to keep this as short as possible.

 

[FEA way]

Each material must be assigned to a separate section. Keywords have to be placed in the proper part of input file (you can find the information about their location in Keywords Reference Guide). Section must be placed where mesh is defined - within either part or instance definition (depends on the type of instance). Materials are created at the model level so their definitions can’t be placed within part, instance or assembly definition. For example:

*Part
.
.
.
*Shell Section, ...
*End Part
.
.
.
*End Assmebly
*Material, ...
*Elastic
...

See also „Assembly definition” chapter of the documentation.

 

[Mustaine3]

I think he comma at the end of each *Material line is the problem. Take it away and submit the job again.

Have you checked if working with *Distribution and *Distribution Table isn't much more effective? This is made to handle such situations (one material property for each element) much more efficient.

 

[Kuba_707]

@Mustaine3

I tried leaving the comma away, still not working.

I also took a look at the *Distribution function but I'm getting this error now:

***ERROR: ELEMENT 1 HAS NO ELASTIC PROPERTY REFERENCE

***ERROR: ELEMENT 1 HAS NO ELASTIC PROPERTY REFERENCE

***ERROR: ELEMENT 1 HAS NO ELASTIC PROPERTY REFERENCE

***ERROR: ELEMENT 1 HAS NO ELASTIC PROPERTY REFERENCE

***ERROR: ELEMENT 1 HAS NO ELASTIC PROPERTY REFERENCE

***ERROR: ELEMENT 2 HAS NO ELASTIC PROPERTY REFERENCE

...

***ERROR: ELEMENT 153786 HAS NO ELASTIC PROPERTY REFERENCE

***ERROR: 153786 elements have zero transvere shear stiffness. The elements have been identified in element set ErrElemZeroTransShearStiff.

***ERROR: 153786 elements have invorrect property definitions. The elements have been identified in element set WarnElemIncorrectProperty.

***ERROR: 153786 elements are missing elastic property reference. The elements have been identified in element set ErrElemMissingElasticPropRef.


My code looks like this now. I don't know if I did it right with defining the material properties like Young's and Shear Moduli. Since I'm dealing with an CFRP-Composite I need to define The Young's Moduli E1 (in fibre direction) and E2 (perpendicular to fibre direction), the poisson's ratio and the shear moduli G12, G13, G23.

*HEADING
Cylinder
*PARAMETER
elementfile = 'Z01a_elements.txt'
nodefile = 'Z01a_nodes.txt'
** Loading
ax_load=-100000
*INCLUDE,INPUT = Z01_layup.inp
*INCLUDE,INPUT = Z01_Material_AS7.inp
*INCLUDE,INPUT = Z01_shell_section.inp
*INCLUDE,INPUT = Z01_244x722Set.inp
*INCLUDE,INPUT = Z01_FxFy.inp
**********************
*NODE,INPUT=<nodefile>
*NODE
999998,0.,0.,0.0
999999,0.,0.,263.0
*NSET,NSET=ref_u
999998,
*NSET,NSET=ref_o
999999,
*RIGID BODY,REF NODE=999998,TIE NSET=bottom_nodes
*RIGID BODY,REF NODE=999999,TIE NSET=top_nodes

*ELEMENT, TYPE=S4R, ELSET=all_elements,INPUT=<elementfile>
*TRANSFORM, TYPE=C, NSET=all_nodes
0., 0., 0., 0., 0., 1.
*ORIENTATION, SYSTEM=C, NAME=OID11
0., 0., 0., 0., 0., 1.
1, 90.
*ELSET, ELSET=ALLELE, GENERATE
1,153786
*DISTRIBUTION TABLE, NAME=tab1
MODULUS, MODULUS, RATIO, MODULUS, MODULUS, MODULUS
*DISTRIBUTION, NAME=stiffness, LOCATION=element, TABLE=tab1
1, 123020, 9842, 0.3, 3199, 3199, 2460
...
153786, 129571, 10366, 0.3, 3369, 3369, 2591
*MATERIAL, NAME=CFK
*ELASTIC, TYPE=LAMINA
stiffness
*DENSITY
1.6E-9,
*SOLID SECTION, ELSET=all_elements, MATERIAL=CFK
*BOUNDARY, OP=NEW
ref_u, 1,6,0.

**********************
*STEP, NLGEOM, INC=1000
*STATIC, STABILIZE=1e-6
0.05, 1.0, , 0.05
*CLOAD
ref_o, 3, <ax_load>
ref_o, 1, <Fx>
ref_o, 2, <Fy>
*OUTPUT, FIELD
*NODE OUTPUT, NSET=all_nodes
U
*NODE OUTPUT, NSET=ref_u
RF,
*OUTPUT,HISTORY,FREQUENCY=1
*NODE OUTPUT,NSET=ref_u
RF,
*NODE OUTPUT,NSET=ref_o
U
*NODE PRINT,NSET=ref_o
U
*NODE PRINT,NSET=ref_u
RF
**RESTART, WRITE
*END STEP

 

[Mustaine3]

Can you attach the files, or at least an representative example? Then I can run a datacheck here and see whats wrong.

 

[Kuba_707]

@Mustaine3

Sure I attached a .rar containing all the needed files.
Normally I just execute the calculations through a .bat file with the order

call abaqus job="Cylinder1" analysis input="C:/Users/.../Master.inp"

 

[FEA way]

You have to add one more line as a first line of the *DISTRIBUTION keyword. This line must specify the default material properties to be used in case if some elements are not listed in the distribution definition. However apparently you can’t define orthotropic linear elastic behavior for shells using distribution. Distribution with *ELASTIC, TYPE=LAMINA is only available for solid continuum elements.

 

[Mustaine3]

Yeah, I was just about to write the same thing. The line in *Distribution with the default values is missing and *Solid Section need to be removed. But then I also got this message:
***ERROR: THE MATERIAL CFK WAS DEFINED WITH DISTRIBUTIONS AND CANNOT BE USED
FOR SHELL ELEMENTS.

It seems that composite shells only support distributions for those things:
thicknesses, offsets, material orientations, composite layer thicknesses, composite layer angles

 

[Kuba_707]

@Mustaine3, @FEA way

Guess I need to try the first suggestion of FEA way
But thank you Mustaine3 for your help.