One-Step Inverse Analysis

One-step inverse analysis in Abaqus/Standard:

  • is used to obtain the initial shape of a sheet metal part given its final (deformed) configuration and a reference blank surface to which the initial configuration must conform;

  • neglects the history of the forming process by assuming proportional loading (Hencky’s deformation theory of plasticity);

  • provides an accurate method for trim line development in flanging operations by unfolding the flange onto the reference blank surface;

  • provides an estimate of plastic deformation induced during forming without detailed modeling of the forming process;

  • ignores the effects of frictional forces between the tools and the part;

  • is available only with shell elements;

  • is a static procedure that neglects inertia effects;

  • uses unsymmetric matrix storage and solution; and

  • is always geometrically nonlinear.

This page discusses:

 

See Also
*ONE-STEP INVERSE

Introduction

The one-step inverse method (Batoz et al.) has become a key analysis tool during the early stages of digital planning of sheet metal stamping processes. The method requires only prior knowledge of the final part design, the material properties, and the initial blank surface and thickness. Given this information, an inverse finite element method is used to compute the initial shape of the part on the blank surface (usually a flat surface). The method is particularly useful in the early stages of part design. You can use the method to, among other things, assess the formability of the part and estimate the blank size when tooling geometry is not yet available.

Another important application of the method is trim line development in sheet metal flanging operations. The one-step inverse method can be used to unfold the flange from its final (as designed) configuration onto an initial blank surface. The trim line can be identified from the perimeter of the unfolded flange. The current capabilities available in Abaqus/Standard are particularly suitable for flange unfolding applications as well as other forming operations with relatively simple boundary conditions, such as clamping a sheet edge.

One-step inverse analysis requires the following input:

  • Shell mesh of the final (deformed) configuration.

  • Shell section definition, including initial (undeformed) sheet thickness and material definition.

  • Mesh of the blank surface that acts as the constraint for the solution of the undeformed configuration.

  • Initial estimate of the undeformed configuration (usually based on geometric projection) to act as the initial guess for the nonlinear Newton method.

  • Node set representing the region of the model with prescribed boundary conditions based on the forming process; the boundary conditions should also be sufficient to prevent rigid body modes.

The one-step inverse method does not consider the intermediate history of the forming process. Instead, it assumes that a proportional loading path is followed between the initial and final configuration. In addition, the implementation of the method in Abaqus/Standard ignores the effect of friction forces on the part. Therefore, the accuracy of the results depends on the validity of these assumptions for a given forming process. The results of the analysis include the nodal coordinates in the initial configuration (as defined by an inverse displacement vector) and the material state (stress, plastic strain, thickness, etc.) in the final configuration. The method is supported only with shell elements.

Part Definition

The definition of the part requires that you specify a mesh of shell elements that conforms to the part geometry in its final configuration. In addition to the usual element connectivity and nodal coordinates, it is recommended that the nodal definition also include information about the nodal surface normals based on the geometry of the part. These normals are needed to evaluate curvature changes with respect to the undeformed configuration. If the nodal normals are not defined directly, Abaqus computes them by averaging the normals of the elements connected to the node.

Incrementation

One-step inverse analysis is always performed in one increment. If a material model includes plastic behavior, the analysis is performed first without taking plasticity into account. Next, this solution is used as a starting point in the analysis with the complete material model.

Controlling the Solution Accuracy

The one-step inverse method is an iterative procedure that requires a stopping criterion—a condition that, when satisfied, considers the solution of the current iteration to be the final converged solution. During the iterations of a one-step inverse analysis, Abaqus monitors the maximum incremental correction to the undeformed nodal coordinates. When this value becomes smaller than a correction tolerance, the solution is considered to have converged. The correction tolerance is determined as the product of the reference shell section thickness and a thickness ratio. The default value of the thickness ratio is 10–2 and can be modified using the field solution controls.

The default for the maximum number of equilibrium iterations is 16. You can modify this value using the time incrementation solution controls.

At every equilibrium iteration Abaqus performs line search iterations if the total norm of the residual vector is not decreased by a prescribed factor. The default value of the maximum number of line search iterations is 3, and the default value of the residual reduction factor is 1.0. You can modify these default values using the line search solution controls.

Initial Conditions

One-step inverse analysis uses an iterative Newton method to determine the undeformed configuration of the part given its final configuration. The undeformed configuration must conform to a surface (the blank surface) that acts as a constraint to the solution. The Newton method requires an initial estimate of the solution as a starting point in the iterative algorithm. You must define this initial configuration by specifying initial conditions for the unfolded coordinates of all nodes in the part (see Defining the Initial Configuration in a One-Step Inverse Analysis). The algorithm may fail to converge if this initial configuration is not sufficiently close to the final solution or if it violates the surface constraint significantly. Therefore, a good initial guess of the undeformed (or unfolded) configuration can be critical to the success of the method. A number of CAD packages offer tools to generate an initial guess based on geometric projections of a mesh over a surface.

In addition, initial values of temperatures, field variables, solution-dependent state variables, etc. can be specified, as described in Initial Conditions.

Boundary Conditions

To make the problem well posed, some of the nodes of the structure must be constrained. You can use fixed boundary conditions to indicate the constrained nodes (see Fixing Degrees of Freedom at a Point in an Abaqus/Standard Analysis). All of the degrees of freedom of the specified nodes are constrained based on their initial undeformed configuration, which was specified by initial conditions.

In the case of flange unfolding applications, there is usually a folding line that represents the intersection of the folded flange geometry and the reference blank surface. The nodes on the folding line should be constrained with a fixed boundary condition.

For other applications, such as deep drawing of a metal cup, you should define fixed boundary conditions for a set of nodes (for example, along the perimeter of the part), such that their displacements are fully prescribed from the difference between the nodal coordinates in the final configuration and the undeformed configuration (defined by the initial conditions). More complex boundary conditions that represent blank holding forces or draw beads are not supported.

Loads

No loads can be prescribed in a one-step inverse analysis.

Predefined Fields

The following predefined fields can be specified in a one-step inverse analysis, as described in Predefined Fields:

  • Although temperature is not a degree of freedom in a one-step inverse analysis, you can specify nodal temperatures. Any difference between the applied and initial temperatures causes thermal strain if a thermal expansion coefficient is given for the material (Thermal Expansion). The specified temperature also affects temperature-dependent material properties, if any.

  • You can specify values of user-defined field variables. These values affect only field variable–dependent material properties, if any.

Material Options

In one-step inverse analysis, isotropic elastic and elastic-plastic material models are supported (with transverse anisotropy is allowed; see Defining Transversely Isotropic Elasticity). Using other material models may lead to convergence difficulties.

Elements

The following shell element types are supported in a one-step inverse analysis to model the part: S3/S3R, S4, S4R, and STRI3 elements. You can use any element type to model the blank.

Constraints

You must define the blank surface on which you expect to position the (unknown) undeformed configuration of the part (see About Surfaces). The blank surface can be any type of surface that is allowed as a main surface in Abaqus/Standard contact calculations. The blank surface acts as a main surface in a no-separation contact pair definition, while the secondary surface must include all the elements of the part to be analyzed (see Using the No Separation Relationship). During the one-step inverse solution process, the no-separation contact constraint is applied only to the reference configuration of the part, thereby enforcing the solution of the undeformed configuration to be on this surface.

Output

In addition to the usual output variables available in Abaqus/Standard (see Abaqus/Standard Output Variable Identifiers), the following nodal variable is provided specifically for one-step inverse procedures:

UINV

Inverse displacement. The displacement from the specified final deformed configuration to the initial configuration.

Displacement U is always zero in a one-step inverse analysis.

Limitations

A one-step inverse analysis is subject to the following limitations:

  • Only one step is allowed in a one-step inverse analysis.

  • General shell section behavior cannot be used.

  • The model of the part must consist of connected regions.

Input File Template

HEADING
……
NODE
Data lines to specify nodal coordinates and (optional) normals in the final configuration
INITIAL CONDITIONS, TYPE=UNFOLD COORDINATE
Data lines to specify initial undeformed nodal coordinates
CONTACT PAIR, INTERACTION=interaction_property_name
secondary_surface_name, main_surface_name
SURFACE INTERACTION, NAME=interaction_property_name
SURFACE BEHAVIOR, NO SEPARATION
**
STEP (,NLGEOM)
ONE-STEP INVERSE, UNFOLD
BOUNDARY, FIXED
Data lines to describe fixed boundary conditions
END STEP

References

  1. Batoz,  J. L., Y. Q. Guo, and F. Mercier, “The Inverse Approach with Simple Triangular Shell Elements for Large Strain Predictions of Sheet Metal Forming Parts,” Engineering Computations, vol. 15, pp. 864–892, 1998.