5.1.13 *MATRIX INPUT

Product: ABAQUS/Standard

Features tested

This section contains tests for direct input of sparse matrices in ABAQUS/Standard. The *MATRIX INPUT option is used to input data for matrices, and the *MATRIX ASSEMBLE option is used to identify the matrices as stiffnesses. Tests contain simple geometries with the *STATIC procedure.

I. Linear perturbation analysis of a truss model

A linear perturbation analysis is performed for a two-dimensional truss structure modeled with matrices.

Element tested

T2D2

Problem description

Model:

Some of the truss elements are replaced by sparse matrices representing stiffness.

Material:

Young's modulus = 2.0 × 10¹¹, Poisson's ratio = 0.3.

Boundary conditions:

The truss model is simply supported with a hinge support on one end and a roller support on the other end. The nodes with boundary conditions are part of the matrices.

Loading:

Concentrated loads are applied at nodes that are either part of the matrices or shared between a matrix and an element.

Results and discussion

Displacements and loads from the matrix-based model are compared to the element-based model.

Input file

truss_matrix.inp

Truss model with matrix.

II. Multiple load case analysis of a beam model with EQUATION and MPC

A multiple load case analysis is performed for a two-dimensional beam model consisting of beam elements and matrices connected by kinematic constraints. For verification purposes, each load case is also analyzed in a separate step.

Element tested

B22

Problem description

Model:

Two beams, each consisting of one beam element and one matrix, are used. The first beam has a TIE MPC between a beam element node and a matrix node. The second beam has an *EQUATION between a beam element node and a matrix node.

Material:

Young's modulus = 2.81 × 10⁷, Poisson's ratio = 0.3.

Boundary conditions:

The beams are fixed at one end and free at the other end. The boundary conditions remain the same for all steps and load cases.

Loading:

A concentrated load and moment are applied at the free end at a node that is part of the matrix for each beam. Each load is applied in a separate step and also as separate load cases in the multiple load case step.

Results and discussion

Results from the matrix-based model are compared to an element-based model for each load case.

Input file

mpceqn_matrix.inp

Beam model with *EQUATION and *MPC at matrix nodes.

III. Large-sliding contact with node-based contact surface

Large-sliding contact is simulated by moving a single two-dimensional continuum element represented by a matrix over other elements.

Element tested

CPE4

Problem description

Model:

The model contains two CPE4 elements and a matrix representing a CPE4 element. Contact is modeled with a node-based slave surface on the matrix nodes and an element-based master surface over the continuum elements.

Material:

Young's modulus = 3.0 × 10⁷, Poisson's ratio = 0.0, friction coefficient = 0.1.

Boundary conditions:

The continuum elements underlying the master surface are fully supported. Matrix nodes are pressed against the continuum element in the first step to simulate normal contact. In the second step, matrix nodes are moved tangent to the master surface to simulate large sliding.

Results and discussion

The displacement solution indicates that the contact constraints are satisfied exactly.

Input files

contact_matrix.inp

Large-sliding contact model with matrix and two-dimensional continuum elements.

contact_stiff.inp

Matrix representing stiffness for a CPE4 element.

IV. Three-dimensional model with predefined temperatures and distributed surface loads

This problem demonstrates how to apply surface loads and predefined temperatures in matrix-based models.

Element tested

C3D6

Problem description

Model:

A cube is modeled with a C3D6 element and a matrix representing another C3D6 element. The element shares nodes with the matrix. Surface elements are defined on the matrix nodes to apply surface loads.

Material:

Young's modulus = 3.0 × 10⁶, Poisson's ratio = 0.3.

Boundary conditions:

Boundary conditions are applied to all nodes in different directions.

Loading:

Surface loads are applied to various faces of the cube. Predefined temperatures are applied for thermal straining.

Results and discussion

Surface loads over the matrix nodes give the same results as the element-based model. Predefined temperatures at nodes shared between the matrix and the element produce correct thermal strains in the element. No effect is observed on the matrix behavior due to predefined temperatures at the matrix nodes.

Input files

tempdsl_matrix.inp

Three-dimensional model with surface loads and predefined temperatures.

tempdsl_stiff.inp

Matrix representing the stiffness for the C3D6 element.

V. Tip loading of a diving board

A static analysis is performed with concentrated loads at the free end of a diving board.

Elements tested

B31 S4R

Problem description

Model:

The diving board is modeled using shell elements. The support for the diving board consisting of shell and beam elements is replaced by a sparse stiffness matrix.

Material:

Young's modulus = 3.0 × 10⁷, Poisson's ratio = 0.29.

Boundary conditions:

Nodes 5, 6, 7, 8, 70, 71, 72, 73, 210, and 213 (part of the matrix) are constrained in all six degrees of freedom.

Loading:

The free end of the diving board is loaded with concentrated loads at the corner nodes.

Results and discussion

The analysis provides displacements for the diving board and reaction forces at the boundary nodes on the matrix. The results match those obtained from an element-based model.

Input files

divingboard_matrix.inp

Diving board with support modeled through matrix.

divingboard_stiff.mtx

Matrix representing stiffness for diving board support.

divingboard_ele.inp

Diving board with support modeled using elements.