The basic data file for the project is: Abaqus_Tutorial_Examples\Mech_001\Case1A\Data\Abaq_Mech_001_Case1a.inp.
The *PARAGEO CONVERSION Keyword is used to define that a conversion of the Abaqus mesh to ParaGeo geometry will be performed. This will generate a ParaGeo data file (.dat), geometry files (.geo and .geometry) and a history data file (.history).
Data File
|
|
*PARAGEO CONVERSION, TYPE=GEOMETRY, PARAGEO FILE=ParaGeo_Mech_001_Case1a
*CONVERSION OUTPUT, LEVEL=2, GEOMETRY=YES, MESH=YES
|
1Conversion TYPE is set to Geometry so that full geometry will be generated. 2The output data files with ParaGeo data will be named ParaGeo_Mech_001_Case1a.dat, ParaGeo_Mech_001_Case1a.geo and ParaGeo_Mech_001_Case1a.geometry 3*CONVERSION OUTPUT keyword is used to request: aDetailed conversion data print on the log (.res) file bOutput of a geometry plot file cOutput of a mesh plot file |
|
The keyword *UNITS is used to define the problem units. Note that default units are Pa, m, s, Celsius.
Data File
|
|
*UNITS, STRESS=MPa, LENGTH=m, TIME=s, TEMPERATURE=Celsius
|
1Stress units are changed to MPa. Other units are kept same as default units. |
|
Mesh data is defined in a separate file with extension .mesh which is read through the keyword *INCLUDE.
Nodal data, Node set data and Element data are defined in the .mesh file.
Include
Data File
|
|
*INCLUDE, INPUT=Abaq_Mech_001_Case1.mesh
|
1The file containing the mesh data is read through the command *INCLUDE 2The name of the mesh file is "Abaq_Mech_001_Case1.mesh" |
Nodal data
Data File
|
|
*NODE
1,0,0,0
2,1,0,0
3,0,1,0
4,1,1,0
5,0,2,0
6,1,2,0
7,0,3,0
8,1,3,0
9,0,4,0
10,1,4,0
11,0,5,0
12,1,5,0
13,0,6,0
14,1,6,0
15,0,7,0
16,1,7,0
17,0,8,0
18,1,8,0
19,0,9,0
20,1,9,0
21,0,10,0
22,1,10,0
|
1Nodal coordinates are provided for the 22 nodes that constitute the domain mesh. |
Nodal set data
Data File
|
|
*NSET, NSET=Base
1,2
*NSET, NSET=West
1,3, 5, 7, 9,11,13,15,17,19,21
*NSET, NSET=East
2, 4, 6, 8,10,12,14,16,18,20,22
*NSET, NSET=Top
21,22
|
1NSETs for all boundaries are defined. 2Each NSET will be converted to a ParaGeo Geometry_set |
Nodal set types
Data File
|
|
*NSET TYPE
Base, Line
Top, Line
West, Line
East, Line
|
1As they are not defined in *NSET keyword through parameter TYPE, *NSET TYPE keyword is used to define the type of geometry entities for each NSET |
Element data
Data File
|
|
*ELEMENT, TYPE=CPE4, ELSET=Sandstone
1, 1, 2, 4, 3
2, 3, 4, 6, 5
3, 5, 6, 8, 7
4, 7, 8, 10, 9
5, 9, 10, 12, 11
6, 11, 12, 14, 13
7, 13, 14, 16, 15
8, 15, 16, 18, 17
9, 17, 18, 20, 19
10, 19, 20, 22, 21
|
1Element topology for 10 quadrilateral elements (4 noded 2D plane strain) is provided. 2A single ELSET is defined for the whole geometry which is named sandstone. 3The ELSET will be converted to a geometry surface. |
|
The *SOLID SECTION data structure is used to create a ParaGeo group from an ELSET. Material is assigned to the solid section.
Material data is defined on a separate (.mat) file in ParaGeo format. This can be obtained from MATINA.
Solid Section
Data File
|
|
*SOLID SECTION, ELSET=Sandstone, MATERIAL=Sandstone
|
1The ELSET "Sandstone" will be converted to a ParaGeo group and will be assigned material named "Sandstone". |
Material
Data File
|
|
*MATERIAL, NAME=Sandstone, FILE=Sandstone.mat
|
1Material named "Sandstone" is read from a material file named "Sandstone.mat" 2Note that the material file should be placed into the same folder as the main datafile. |
Material data
Data File
|
|
* Material_data NUM=1
Material_name "Sandstone"
Units IDM=4
"MPa"
"m"
"s"
"Celsius"
Isotropic_elastic_properties IDM=2
1000
0.200
Grain_density 2710
Porosity 0.35
|
1Material_data is defined on a separate material file (.mat) in ParaGeo format. 2The material is defined with units "MPa", "m", "s" and "Celsius". When MPa and m units are specified the mass is automatically evaluated in the appropriate units using the grain density specified in standard units (Kg/m3). 3The elastic material is defined as isotropic so that only Young's modulus and Poisson's ratio is required 4The initial reference porosity (0.35) may change during the simulation due to large deformations. |
|
The *BOUNDARY keyword is used to prescribe some or all displacement freedoms for geometry sets. It will generate ParaGeo Support_data data structure.
Data File
|
|
*BOUNDARY
Base, 2,2,0
East, 1,1,0
West, 1,1,0
|
1Side boundaries (East and West) have zero displacement prescribed in X direction (degree freedom number 1). 2Base has zero prescribed displacement in Y direction (degree freedom number 2). |
In addition a *BOUNDARY keyword with parameter TYPE=NORMAL STRESS is used to define a load of 10 MPa to the top surface. This will generate a ParaGeo Global_loads corresponding to the load and a Load_case_control_data which is used to indicate which loads are active. Note that an alternative method to define a load on the top surface would be using *TOP SURFACE keyword.
In order to define the loading rate an *AMPLITUDE keyword is used to define a loading curve. Note that this must be defined prior to the *BOUNDARY in order to allow curve assignment (otherwise the code will consider that the assigned curve is not defined).
Amplitude
Data File
|
|
*AMPLITUDE, NAME=LOADING_CURVE
0.0,0.0,1.0,1.0
|
1An amplitude curve to define a gradual increase on the load from t=0 (no load applied) to t=1 (load is fully applied) is defined. |
Stress Load
Data File
|
|
*BOUNDARY, NAME=Load, AMPLITUDE=LOADING_CURVE, TYPE=NORMAL STRESS
Top, 10
|
1TYPE is set to NORMAL STRESS to define stress boundary conditions. 2The previously defined amplitude curve named LOADING_CURVE is assigned to define the rate of stress applied. 3A load of 10 MPa is defined for NSET "Top". |
|
High definition history data is used to both:
1Construct graphs of key variables for result interpretation. 2Monitor the dynamics in the solution for quasi-static analysis.
Two methods are usually adopted for monitoring dynamic response in quasi-static analysis using a dynamic solver:
1Visualization of time histories of the kinetic and elastic strain energy. These provide a global measure of the dynamic response for the complete problem domain. 2Visualization of point values of displacement, velocity or stress at specific points within the problem domain. These provide a local measure of dynamic response and can identify small regions of active deformation which exhibit a dynamic response within a largely quasi-static domain. This localized dynamic response may be difficult to discern using the global measures when the majority of the domain is behaving quasi-statically.
History point
The *HISTORY POINT keyword is used to generate ParaGeo History_point data structure which is output to ParaGeo_Mech_001_Case1a .history file. It allows creation of time history sets of specific results for individual points. The time history data is written as an ASCII file in comma delimited column format to: datafile_number.hdh where datafile is the data file name and number is the History_point set number. Note that *HISTORY POINT keywords will generate History_point data structures which are automatically numbered in order of appearance starting at number 1.
Several History_point data structures may be specified and additional sets may be added during the analysis.
Data File
|
|
*HISTORY POINT, NAME=Set1, TIME=0.01, ACTIVE=ACTIVE
*GROUPS
Sandstone
*POINTS
0.5, 0.01
0.5, 9.99
*DISPLACEMENT
Disp_y
*STRESS
Strs_yy
|
1*HISTORY POINT is named "Set1". 2The values are output at time increments of 0.01 Ma (problem units). 3Sub-keyword *GROUPS is used to assign the history set to group "Sandstone". 4The sub-keyword *POINTS is used to define the coordinates of the history points which are:
Point
|
X-Coordinate
|
Y-Coordinate
|
1
|
0.5
|
0.01
|
2
|
0.5
|
9.99
|
5The values output are: (a) Displacement in Y-Direction (b) Stress in Y-Direction
|
History global
The *HISTORY GLOBAL keyword is used to generate ParaGeo History_global data structure which is output to ParaGeo_Mech_001_Case1a .history file. This creates a time history set with quantities that are applicable to the complete domain; e.g. total kinetic energy. The time history data is written as an ASCII file in comma delimited column format to: datafile_000.hdh where datafile is the data file name.
Data File
|
|
*HISTORY GLOBAL, TIME=0.01
External, Kinetic, Elastic
|
1The values are output at time increments of 0.01. 2The values output are: (a) Work done by External Loads (b) Elastic strain energy (c) Kinetic energy
|
|
The *CONTROLS keyword is used to convert to ParaGeo Control_data data structure. In this case it defines the solution algorithm and output requirements for the geomechanical field. Several *CONTROLS keywords can be defined to set up different data. Keywords *STEP and *END STEP are used to indicate the beginning and end of a simulation step / stage so that data defined in between them will belong to that step / stage. Several stages in the analysis may be defined; e.g. stage 1 may be an initialization step and stage 2 may be a loading step. For each pair of *STEP and *END STEP the conversion will generate a ParaGeo Control_data structure.
Data File
|
|
*STEP, NAME=Loading
**
* CONTROLS, FIELD=DISPLACEMENT, CRITICAL FACTOR=0.7, SOLVER=EXPLICIT, POROUS FLOW=Dry
* CONTROLS, FIELD=GLOBAL, DURATION=2.0, PLOT TIME=0.05, PLOT STEP=-1, SCREEN STEP=500
**
*END STEP
|
1A single simulation stage / step is defined for the problem which is named "Loading". This is indicated by the *STEP and *END STEP keywords 2*CONTROLS with FIELD=DISPLACEMENT is used to set geomechanical field parameters. Data defined is: a.Explicit solver b.Critical time step factor of 0.7 c.Porous flow type set to dry (porous material with zero pore pressure, in other words, saturation equals zero) 3*CONTROLS with FIELD=GLOBAL is used to set general stage parameters. Data defined is: a.Duration for stage is set to 2 Ma b.Plot output is performed every 0.05 Ma c.Plot output at the end of simulation stage is ensured (PLOT STEP=-1) d.Print of simulation information to the command prompt is performed every 500 steps. |
|
|
