SPRINGBACK

The SPRINGBACK under Process template is used to simulate the springback of the blank after drawing simulation, as shown in Figure 8.2.107. The user can also add springback stage in multi stage simulation, as illustrated in Figure 8.2.108. Springback process consists of four pages. For information about General and Blank, refer to Section 8.2.4 Forming.

Figure 8.2.107  Springback analysis

 

Figure 8.2.108  New springback stage

 

8.2.7.1  BOUNDARY CONDITION

The Boundary Condition page is illustrated in Figure 8.2.109. This page enables the user to define springback constraints. Refer to Section 8.2.4.3 for detailed description on definition of springback constraints.

 

Figure 8.2.109  Springback boundary condition

 

CONSTRAINTS

 

Allow the user to select three nodes to constrain rigid displacement of blank during springback analysis. The first selected node is constrained in X, Y, Z direction. The second selected node is constrained in Y, Z direction. The third selected node is constrained in Z direction. The relationship of location for these three constraints is illustrated in Figure 8.2.110.

 

Figure 8.2.110 Springback constraints definition

 

8.2.7.2  CONTROL

Set control parameters for springback analysis, as illustrated in Figure 8.2.111.

 

GENERAL

 

      SHELL WARPING STIFFNESS (BWC): Default is set as 2, i.e. Belytschko-Tsay

   

      ADVANCED…: Advanced parameter setting.

Figure 8.2.111  Springback control parameters interface

 

 

IMPLICIT ANALYSIS

 

Allow to user to select approach of springback analysis: single step springback or multiple step springback analysis. Multiple step springback is set as default option. Single step springback analysis usually leads to good result. However, converged result may not be obtained using single step springback analysis for relatively flexible part. The user is recommended to conduct springback analysis using multiple step approach. Detailed descriptions for setting up single or multiple step springback analysis is described in LS-DYNA User’s Manual.

 

      INITIAL TIME STEP SIZE (DT0): Initial time step size of springback analysis. Default value is 0.001.    

 

NUMBER OF IMPLICIT STEP (NSBS): Number of implicit step. Set to 1 if single step implicit analysis is performed. If the value is greater than 1, multiple implicit analysis is used.

 

ADVANCED…: Set advanced parameter of implicit analysis. See Figure 8.2.112 for the list of parameters.

Figure 8.2.112  Advanced parameter for Implicit Analysis

 

 

COARSENING MESH

Allow the user to use coarsening mesh technique during springback analysis. During drawing simulation, adaptive mesh is adopted to refine blank mesh to capture details on tooling. Adaptive meshing increases model size and posses challenge to the convergence in springback analysis. This option merges the refine mesh on the flat areas to reduce model size. It reduces convergence problem and shorten the computing time.

 

ANGLE: Set the angle criteria for merge neighboring elements. If difference of element normal angle between adjacent elements is less than the given criteria, these elements are merged. Default angle is 8°.

 

CHECKING MESH

This function allows the user to check mesh quality during Springback analysis. The user can check adaptive constraints, minimum aspect ratio, minimum and maximum allowable interior angle and minimum element size.

 

FIXING BAD ELEMENT

This function enables solver to automatically repair distorted elements and output the relevant information into text file. It helps to increase precision of springback analysis, as well as improving convergence.