abaqusStruct2inp

Below is a demonstration of the features of the abaqusStruct2inp function

Syntax
Description
About Abaqus INP input files
Coding INP files in MATLAB
Using field names with spaces in them
Creating the INP file
View the inp file

clear; close all; clc;

Syntax

[T]=abaqusStruct2inp(abaqus_spec,fileName,optionStruct);

Description

This function provides the basis for coding Abaqus .inp input files

About Abaqus INP input files

Abaqus input files (.inp) are plain text files.

% Using a _ in a structure field name results in a space in the INP file,
% e.g. Solid_section becomes Solid Section.
% Similarly, using __ (two underscores) in a structure field name results
% in a phyphen (-) in the INP file, e.g. Solid__section becomes
% Solid-Section.

Coding INP files in MATLAB

Specify file heading Users may provide a heading which can be used to give a description of the input file.

% *Heading
% ** Job name: ABAQUS inp file creation demo
% ** Generated by: GIBBON

abaqus_spec.Heading.COMMENT{1}='Job name: ABAQUS inp file creation demo';
abaqus_spec.Heading.COMMENT{2}='Generated by: GIBBON';

The preprint section

% *Preprint, echo=NO, model=NO, history=NO, contact=NO
abaqus_spec.Preprint.ATTR.echo='NO';
abaqus_spec.Preprint.ATTR.model='NO';
abaqus_spec.Preprint.ATTR.history='NO';
abaqus_spec.Preprint.ATTR.contact='NO';

The part section

V=[ 1 1 1; 1 0 1;  1 1 0; 1 0 0; 0 1 1; 0 0 1; 0 1 0; 0 0 0];

nodeIds=(1:1:size(V,1));
E=[5 6 8 7 1 2 4 3];
elementIds=(1:1:size(E,1));

% Node
abaqus_spec.Part{1}.COMMENT='This section defines the part geometry in terms of nodes and elements';
abaqus_spec.Part{1}.ATTR.name='Cube';
abaqus_spec.Part{1}.Node={nodeIds(:),V};

% Element
abaqus_spec.Part{1}.Element{1}.ATTR.type='C3D8R';
abaqus_spec.Part{1}.Element{1}.VAL={elementIds(:),E};

%Element sets
abaqus_spec.Part{1}.Elset{1}.ATTR.elset='Set-1';
abaqus_spec.Part{1}.Elset{1}.VAL=1;

%Node sets
abaqus_spec.Part{1}.Nset{2}.ATTR.nset='Set-2';
abaqus_spec.Part{1}.Nset{2}.VAL=1:1:size(V,1);

%Node sets using "generate"
abaqus_spec.Part{1}.Nset{1}.ATTR.nset='Set-1';
abaqus_spec.Part{1}.Nset{1}.ATTR.generate='';
abaqus_spec.Part{1}.Nset{1}.VAL=[1 size(V,1) 1];

%Sections
abaqus_spec.Part{1}.Solid_section.ATTR.elset='Set-1';
abaqus_spec.Part{1}.Solid_section.ATTR.material='Elastic';

% abaqus_spec.Part{1}.Shell_section.ATTR.elset='Set-1';
% abaqus_spec.Part{1}.Shell_section.ATTR.material='Material-1';
% % abaqus_spec.Part{1}.Shell_section.VAL=[10 5]; %Use numerical data
% abaqus_spec.Part{1}.Shell_section.VAL='10., 5'; %Use custom text data

The assembly section

abaqus_spec.Assembly.ATTR.name='Assembly-1';

abaqus_spec.Assembly.Instance{1}.ATTR.name='Cube-1';
abaqus_spec.Assembly.Instance{1}.ATTR.part='Cube';

% abaqus_spec.Assembly.Instance{2}.ATTR.name='Clot-1';
% abaqus_spec.Assembly.Instance{2}.ATTR.part='Clot';


abaqus_spec.Assembly.Nset{1}.ATTR.nset='Set-1';
abaqus_spec.Assembly.Nset{1}.ATTR.instance='Cube-1';
abaqus_spec.Assembly.Nset{1}.ATTR.generate='';
abaqus_spec.Assembly.Nset{1}.VAL=[1 4 1];

abaqus_spec.Assembly.Nset{2}.ATTR.nset='Set-3';
abaqus_spec.Assembly.Nset{2}.ATTR.instance='Cube-1';
abaqus_spec.Assembly.Nset{2}.ATTR.generate='';
abaqus_spec.Assembly.Nset{2}.VAL=[5 7 1];

abaqus_spec.Assembly.Nset{3}.ATTR.nset='Set-4';
abaqus_spec.Assembly.Nset{3}.ATTR.instance='Cube-1';
abaqus_spec.Assembly.Nset{3}.ATTR.generate='';
abaqus_spec.Assembly.Nset{3}.VAL=[2 6 2];

abaqus_spec.Assembly.Nset{4}.ATTR.nset='Set-5';
abaqus_spec.Assembly.Nset{4}.ATTR.instance='Cube-1';
abaqus_spec.Assembly.Nset{4}.VAL=[3 4 7];

abaqus_spec.Assembly.Nset{5}.ATTR.nset='origin';
abaqus_spec.Assembly.Nset{5}.ATTR.instance='Cube-1';
abaqus_spec.Assembly.Nset{5}.VAL=8;

abaqus_spec.Assembly.Nset{6}.ATTR.nset='all';
abaqus_spec.Assembly.Nset{6}.ATTR.instance='Cube-1';
% abaqus_spec.Assembly.Nset{6}.ATTR.generate='';
abaqus_spec.Assembly.Nset{6}.VAL=1:size(V,1);

abaqus_spec.Assembly.Surface{1}.ATTR.type='ELEMENT';
abaqus_spec.Assembly.Surface{1}.ATTR.name='innerSurface';
elemSetsInner={[1 2 3 4],[4 5 6 7]};
elemSetSideInner=[1 2];
valCell=cell(numel(elemSetsInner),1);
for qs=1:1:numel(elemSetsInner)
    surfaceElementSetName=['elementSetInnerSurface',num2str(qs)];
    abaqus_spec.Assembly.Elset{qs}.ATTR.elset=surfaceElementSetName;
    abaqus_spec.Assembly.Elset{qs}.ATTR.internal=''; %Remains hidden uppon import
    abaqus_spec.Assembly.Elset{qs}.ATTR.instance='Cube-1';
    abaqus_spec.Assembly.Elset{qs}.VAL=elemSetsInner{qs};

    sidePick=elemSetSideInner(qs);
    valCell{qs}={[surfaceElementSetName,', S',num2str(sidePick)]};
end
abaqus_spec.Assembly.Surface{1}.VAL=valCell;

Equation constraint

% *Equation
% 2
% X(n-1), 1, 1.
% XControlN, 1, -1.

%%--> Constraints
abaqus_spec.Assembly.COMMENT='Constraint 1';
abaqus_spec.Assembly.Equation.VAL=['2' newline 'X(n-1), ',  '1, 1.' newline 'XContN, ' '1, -1.'];

The material section

% *Material, name=Material-1
% *Hyperelastic, neo hooke
%  0.03,1.

abaqus_spec.Material.ATTR.name='Neo-Hooke';
abaqus_spec.Material.Hyperelastic.VAL=[0.03 1];
abaqus_spec.Material.Hyperelastic.ATTR.neo_hooke='';
abaqus_spec.Material.ATTR.name='Elastic';
abaqus_spec.Material.Elastic=[0.5 0.49];

Orientation

% *Orientation, name=Ori-1, system=RECTANGULAR
% Ori-1-DiscOrient
% 2, 90.
abaqus_spec.Orientation.ATTR.name='Ori-1';
abaqus_spec.Orientation.ATTR.system='RECTANGULAR';
abaqus_spec.Orientation.VAL=['Ori-1-DiscOrient' newline vec2strIntDouble([2 90],'%i')];

Contact pair

%%--> Contact pair
abaqus_spec.contact_pair{1}.ATTR.interaction='user-1';
abaqus_spec.contact_pair{1}.ATTR.type='node to surface';
abaqus_spec.contact_pair{1}.ATTR.adjust='0.0';
abaqus_spec.contact_pair{1}.VAL='AORTA-ASSEMBLY.OUTER, AORTA1-ASSEMBLY.OUTERX';

% surface interaction
abaqus_spec.surface_interaction{1}.ATTR.name='user-1';
abaqus_spec.surface_interaction{1}.ATTR.user='';
abaqus_spec.surface_interaction{1}.ATTR.properties='7';
abaqus_spec.surface_interaction{1}.ATTR.unsymm='';
abaqus_spec.surface_interaction{1}.ATTR.DEPVAR='13';
abaqus_spec.surface_interaction{1}.CSTM=', '; %Line with just comma

%Wrap to max width of 8 entries
t=vec2strIntDouble([0.2, 0.2, 0.05, 0.05,150,1000,0.0],'%6.7e');
t=strwrap(t,8,', ',1);
abaqus_spec.surface_interaction{1}.VAL=t;

The step section

abaqus_spec.Step.ATTR.name='Step-1';
abaqus_spec.Step.ATTR.nlgeom='YES';
abaqus_spec.Step.Static=[0.1 1 1e-5 0.1];

% Boundary
abaqus_spec.Step.Boundary{1}.VAL={'Set-1',[1 1],0.1};
abaqus_spec.Step.Boundary{2}.VAL={repmat({'origin'},3,1) [1 1; 2 2; 3 3]};
abaqus_spec.Step.Boundary{3}.VAL={'Set-3',[1,1]};
abaqus_spec.Step.Boundary{4}.VAL={'Set-4',[2,2]};
abaqus_spec.Step.Boundary{5}.VAL={'Set-5',[3,3]};

% Loads
% ** LOADS
% **
% ** Name: Load-1   Type: Pressure
% *Dsload
% Surf-1, P, 0.00533
% **
abaqus_spec.Step.Dsload{1}.VAL={'Surf-1','P',0.00533};

%Output
abaqus_spec.Step.Restart.ATTR.write='';
abaqus_spec.Step.Restart.ATTR.frequency=0;

abaqus_spec.Step.Output{1}.ATTR.field='';
abaqus_spec.Step.Output{1}.ATTR.variable='PRESELECT';
abaqus_spec.Step.Output{2}.ATTR.history='';
abaqus_spec.Step.Output{2}.ATTR.variable='PRESELECT';
abaqus_spec.Step.Node_print.ATTR.nset='all';
abaqus_spec.Step.Node_print.ATTR.frequency = 1;
abaqus_spec.Step.Node_print.VAL='COORD';
abaqus_spec.Step.El_print.VAL='S';

% * NODE SET, set=yoursetname, frequency = 1
% U

Using field names with spaces in them

To code for field names with spaces use an underscore i.e. _ instead of a space. For instance to code for: * some stuff with spaces 5 One needs:

abaqus_spec.some_stuff_with_spaces=5; % a fieldname containing spaces

Creating the INP file

You can use abaqusStruct2inp to write the structure data to a file.

%Create file name for INP file
defaultFolder = fileparts(fileparts(mfilename('fullpath')));
savePath=fullfile(defaultFolder,'data','temp');
fileName=fullfile(savePath,'tempModel.inp');
[~,fileNamePart,~]=fileparts(fileName);

[T]=abaqusStruct2inp(abaqus_spec,fileName);

View the inp file

edit(fileName);

GIBBON www.gibboncode.org

Kevin Mattheus Moerman, [email protected]

GIBBON footer text

License: https://github.com/gibbonCode/GIBBON/blob/master/LICENSE

GIBBON: The Geometry and Image-based Bioengineering add-On. A toolbox for image segmentation, image-based modeling, meshing, and finite element analysis.

This program is free software: you can redistribute it and/or modify it under the terms of the GNU General Public License as published by the Free Software Foundation, either version 3 of the License, or (at your option) any later version.

This program is distributed in the hope that it will be useful, but WITHOUT ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the GNU General Public License for more details.

You should have received a copy of the GNU General Public License along with this program. If not, see http://www.gnu.org/licenses/.