formability

1. Chapter 55: Square Cup Deep Drawing using Forming Limit Diagram
55
Square Cup Deep Drawing
using Forming Limit Diagram
PART 1. Explicit Forming
 Summary
1098

Introduction

Modeling Details

Results
1099
1101
1104
PART 2. Implicit Spring Back
 Introduction
1108

Modeling Details

Results

Input File(s)

Reference
1110
1112
1112
1108

2. 1098 MD Demonstration Problems
CHAPTER 55
Summary
Title
Chapter 55: Square Cup Deep Drawing using Forming Limit Diagram
Features
• Failure criterion based on the Forming Limit Diagram
• Springback: Explicit -> Implicit switching
Geometry
Punch
Clamp
Sheet
Die
Material properties
• Sheet Metal (aluminum sheet): Anisotropic Materials under Plane Stress Conditions
Exx = 71.0 GPa,  = 0.33
Stress constant = 0.0 MPa, Hardening modulus = 576.79 MPa
Strain offset = 0.01658, Exponent for power-law hardening = 0.3593
Lankford parameters: R0 = 0.71, R45 = 0.58, R90 = 0.70
• Punch, Die, and Clamp: Rigid
Analysis characteristics
Transient explicit dynamic analysis (SOL 700 explicit single precision)
Nonlinear implicit static analysis (SOL 700 implicit double precision)
Boundary conditions
• Explicit: Fixed boundary condition of Die and Clamp
• Implicit Springback: Fixed at the center point of the plate
Element types
4-node shell elements
FE results
Stress Contour Plot, Forming Limit Diagram and more
Explicit Forming
Implicit Spring Back
Element will fail
at next step
80.00%
FLD at Mid. Surface
FLD with Safety margin
Major True Strain (%)
60.00%
40.00%
20.00%
0.00%
-30.00%
-20.00%
-10.00%
0.00%
-20.00%
Minor True Strain (%)
10.00%
20.00%

3. CHAPTER 55 1099
Square Cup Deep Drawing using Forming Limit Diagram
PART 1. Explicit Forming
Introduction
This is a sheet metal forming example of a plate with anisotropic behavior that is drawn through a square hole by
means of a punch. This particular example has experimental results from a verification problem of the 1993
NUMISHEET Conference held in Japan. The results are obtained at single punch depth (20 mm punch travel) for an
aluminum alloy plate. The material is seen to be anisotropic in its planar directions; i.e., the material behavior is
different for all directions in the plane of the sheet metal as well as in the out of plane direction. The data obtained
from the NUMISHEET Conference is as follows:
Aluminum Alloy
Thickness = 0.81 mm
Young’s modulus = 71 GPa
Poisson’s ratio = 0.33
Density = 2700 kg/m3
Yield stress = 135.3 MPa
Stress = 576.79 * (0.01658 + p)0.3593 MPa
Lankford parameters: R0 = 0.71, R45 = 0.58, R90 = 0.70
Friction coefficient = 0.162
The size of the plate modeled was 0.15 x 0.15 (in meters). No strain-rate dependency effects were included in the
material data, so the metal sheet was analyzed without these effects. The dimensions of the plate, die, punch, and clamp
are all given in Figure 55-1.
SOL 700 Entries Included
SOL 700
TSTEPNL
DYPARAM,LSDYNA,BINARY,D3PLOT
CSPH
PSPH
EOSGRUN
SPHDEF
TIC
MATD010
PSOLIDD
MATD003

4. 1100 MD Demonstration Problems
CHAPTER 55
Figure 55-1
Dimensions of Plate, Die, Punch, and Clamp (in Millimeters)

5. CHAPTER 55 1101
Square Cup Deep Drawing using Forming Limit Diagram
Modeling Details
Punch
Clamp
Sheet
Die
Z
X
Figure 55-2
Y
SOL 700 Model (Exploded View)
The SOL 700 model is shown in Figure 55-2. The main parts in the finite element model are:
•
•
•
•
sheet metal
punch
die
clamp
Sheet Metal
The SOL 700 material model for sheet metals is a highly sophisticated model and includes full anisotropic behavior,
strain-rate effects, and customized output options that are dependent on material choice. Since not all of the materials
can be derived from the simplified set given by the NUMISHEET organization, most participants in the conference
used an isotropic material model. In reality, the process is definitely anisotropic and effects due to these differences
can be seen in the transverse direction. For materials displaying in-plane anisotropic behavior, the effect would be even
more noticeable. The parameters on the MAT190 (refer to the MD Nastran Quick Reference Guide) specify planar
anisotropic behavior and are as follows (for the aluminum sheet):
• MATD190 elastic material properties.
• Isotropic behavior was assumed in the elastic range:
Exx = 71.0 GPa
= 0.33

6. 1102 MD Demonstration Problems
CHAPTER 55
• Planar anisotropic yielding and isotropic hardening were assumed in the plastic range:
A = Stress constant = 0.0 MPa
B = Hardening modulus = 576.79 MPa
C = Strain offset = 0.01658
n = Exponent for power-law hardening = 0.3593
• Lankford parameters:
R0 = 0.71
R45 = 0.58
R90 = 0.70
Punch, Die, and Clamp
These three components provide the constraints and driving displacement for the analysis and are modeled as rigid
bodies. Contact is then specified with the metal sheet using the friction coefficient values provided. The three contact
types are specified as following:
• Contact between the punch and the sheet
• Contact between the die and sheet
• Contact between the clamp and sheet
Finally, the punch is given a scaled downward velocity providing the driving displacement for the analysis.
Input File
SOL 700,NLTRAN stop=1
SOL 700 is an executive control entry and activates an explicit nonlinear transient analysis.
Case control section is below:
DLOAD = 1
IC = 1
SPC = 1
BCONTACT = 1
TSTEPNL = 1
The bulk entry section starts:
BEGIN BULK
$
TSTEPNL 1
$
DYPARAM LSDYNA
20
2.0E-3
BINARY
D3PLOT
0.002

7. CHAPTER 55 1103
Square Cup Deep Drawing using Forming Limit Diagram
TSTEPNL is a SOL 700 bulk data entry which describes the number of Time Steps (20) and Time Increment (2.00 ms)
of the simulation. The end time is the product of the two entries. Notice here the Time Increment is only used for the
first step. The actual number of Time Increments and the exact value of the Time Steps are determined by SOL 700
during the analysis. The time step is a function of the smallest element dimension during the simulation.
LSDYNA,BINARY,D3PLOT option of DYPARAM entry controls the output time steps of d3plot binary file. The result
plots at every 0.002 seconds are stored in d3plot binary file.
Bulk data entries that define properties for shell elements
PSHELL1 1
+
.81
1
BLT
Gauss
MATD020 2
1
1.0
4
210.E9
7
+
0.3
The MATD020 entry defines the rigid material property. In the example, the clamp, die, and punch are modeled by the
rigid materials.
MATD190 1
2.7E-4 7.1E7
0.33
2.0
+
6.0
.71
.58
.70
+
2.0
77
+
1.0
0.0
+
0.0
1.0
TABLED1,77,,,,,,,,+
+,-100.0,196.67,0.0,30.,30.,45.,40.,47.,+
+,50.,45.,ENDT
576.79E3.3593
.01658
0
0.0
0.0
+
+
+
+
The MATD190 entry defines an anisotropic material developed by Barlat and Lian (1989) for modeling sheets under
plane stress conditions and with Forming Limit Diagram failure criteria. This material allows the use of the Lankford
parameters for the definition of the anisotropy.
In the model, Gosh’s hardening rule is used:
n
Y  p  = k  0 + p  – p
The forming limit diagram is defined in by TABLED1 as shown above.
All fields are set for the coefficients of equations. See MD Nastran Quick Reference Guide for details.
SPCD2,1,RIGID,MR2,3,0,100,1.0,,+
+
TABLED1,100,,,,,,,,+
+,0.0,-1000.,0.02,-1000.,ENDT

8. 1104 MD Demonstration Problems
CHAPTER 55
The SPCD2 entry defines imposed nodal motion on a node, a set of nodes or nodes of a rigid body. The rigid punch is
moving downward at 1000 m/s from 0 to 0.02 seconds.
FORCE
9999
MR3
-19.6E6
1.
The FORCE entry defines a force on the grid point as well as rigids. Since the forces on the rigid body are not yet
supported by the Nastran input processor, TODYNA and ENDDYNA entries are used in conjunction with the FORCE
entry to by-pass the IFP (Input File Processor) and directly access SOL 700.
BCTABLE
1
SLAVE
1
0
0.162
0.
0
3
0.
0
SS1WAY
0.162
0.
0
+
+
The BCBODY entry defines a flexible or rigid contact body in 2-D or 3-D. Although SOL 700 only supports flexible
contact in BCTABLE, the rigid contact can be applied using the rigid material of contact bodies. In this example, all
contact body pairs are given 0.162 static and kinetic friction coefficients. The surface-to-surface, one way contact
method is used for all contact definitions.
BCBODY
..
$
BSURF
..
1
1
DEFORM
1
1
THRU
1600
The BCBODY entry defines a flexible or rigid contact body in 2-D and 3-D.
The BSURF entry defines a contact surface or body by element IDs. All elements with the specified IDs define a
contact body.
$
GRID
..
GRID
$
CQUAD4
..
CQUAD4
1
-75.
75.
0.0
4528
-8.33333-37.0067-75.405
1
1
1
2
43
42
4468
63
4527
4273
4274
4528
Results
To verify the result of MD Nastran, the major and minor principal strains at 0.015seconds are compared with those of
Numisheet and Dytran results in Figure 55-3 and Figure 55-4. Left plots of each figure were represented by

9. CHAPTER 55 1105
Square Cup Deep Drawing using Forming Limit Diagram
Makinouchi et al. (1993). The data in the plots were obtained from several companies which did the same test. MD
Nastran gave a solution well within the spread of experimental values.
Major Principal Strain
2.50E-01
2.00E-01
Strain
1.50E-01
1.00E-01
5.00E-02
0.00E+00
0
20
40
60
80
100
120
Distance from Center Along Line OB
Figure 55-3
Comparison of Major Principal Strain Along Line OB
(Numisheet and Dytran Results vs. MD Nastran SOL 700)
Minor Principal Strain
0.00E+00
0
20
40
60
80
-5.00E-02
Strain
-1.00E-01
-1.50E-01
-2.00E-01
-2.50E-01
Distance from Center Along Line OB
Figure 55-4
Comparison of Minor Principal Strain Along Line OB
(Numisheet and Dytran Results vs. MD Nastran SOL 700)
100
120

10. 1106 MD Demonstration Problems
CHAPTER 55
80.00%
Element will fail
at next step
FLD at Mid. Surface
FLD with Safety margin
Major True Strain (%)
60.00%
40.00%
20.00%
-30.00%
-20.00%
-10.00%
0.00%
0.00%
10.00%
20.00%
-20.00%
Minor True Strain (%)
Figure 55-5
Forming Limit Diagram Along Line OB at 0.019 Seconds

11. CHAPTER 55 1107
Square Cup Deep Drawing using Forming Limit Diagram
t = 0.000 seconds
t = 0.004 seconds
t = 0.008 seconds
t = 0.012 seconds
t = 0.016 seconds
Figure 55-6
t = 0.020 seconds
Maximum Principal Strain Contour Plots at Mid Surface at Various Times
Note that the FLD diagram correctly predicts the failure of elements at t = 0.019 as shown in the stress fringe plots.

12. 1108 MD Demonstration Problems
CHAPTER 55
PART 2. Implicit Spring Back
Introduction
Springback refers to an event in which there is elastic strain recovery after the punch is removed. This deformation
can alter the final desired shape significantly. In an explicit dynamic analysis, it can take some time before the
workpiece comes to a rest, so the springback simulation is performed using the implicit solver to speed up this part of
the analysis. Using explicit-implicit switching available in SOL 700, the residual deformations after sheet metal
forming are computed and used as a pre-condition for springback analysis. Because, in this example, there was a
failure at around 0.019 seconds in the sheet metal as shown in Part 1, the explicit simulation was terminated at 0.018
seconds. The initial condition, including the final stresses and deformation and the element connectivity of the explicit
run are transferred to the implicit run. The analysis scheme is described below.
SOL 700 Explicit
(Use SEQROUT Entry)
Generate jid.dytr.nastin
SOL 700 Implicit
(Include jid.dytr.nastin)
(Use SPRBCK Entry)
Figure 55-7
Analysis Scheme
SOL 700 Entries Included
SOL 700
MATD036
SEQROUT
SPRBCK
Modeling Details
The model of explicit run is the same as Part 1. In the implicit run, only the sheet metal is used.
Input File
Explicit Input File
BEGIN BULK
$
TSTEPNL 1
10
1.8E-3

13. CHAPTER 55 1109
Square Cup Deep Drawing using Forming Limit Diagram
As mentioned above, the end time of simulation is assigned to 0.018 seconds.
SEQROUT 10
BCPROP 10
1
The SEQROUT entry generates the jid.dytr.nastin file at the end of simulation. The nastin file includes the
final deformations and stresses of the assigned part. The nastin file can be used for a subsequent explicit or implicit
SOL 700 run. In the example, only the result for Part 10 which includes the sheet metal is written out to the nastin
file.
Implicit Input File
BEGIN BULK
$
TSTEPNL 1
10
1.8E-3
As mentioned above, the end time of simulation is assigned to 0.018 seconds.
Because all information of nodes and element connectivity is in jid.dytr.nastin file, Grid and CQUAD entries are
removed in the implicit input. Only one point boundary condition at the center and SPRBCK entry are added in the
input file.
Since MATD190 is not available in the implicit analysis, MATD036 is used instead of MATD190. MATD036 and
MATD190 are identical material models except that FLD is supported only in MATD190.
MATD036 1
+
6.0
+
2.0
+
+
2.7E-4
.71
7.1E7
.58
0.33
.70
2.0
1.0
0.0
0.0
1.0
576.79E3.3593
.01658
0
+
0.0
0.0
+
+
+
MATD036 is only different in the failure criteria using FLD. Others are the same as MATD190 in the explicit
simulations of Part 1 and 2.
SPRBCK
+
+
+
1
2
1
0.005
200
1
100
0.0
1.0E-2
1
1.00E-3
0.10
+
+
+
SPRBCK activates the implicit spring back analysis. Nonlinear with BFGS updates solver type is used in the example.
See MD Nastran Quick Reference Guide for other fields.
SPC1
1
123456
841
Only one point at the center of the sheet metal is fixed to prevent singular condition in the implicit simulation.

14. 1110 MD Demonstration Problems
CHAPTER 55
Results
The springback simulation from explicit to implicit runs works fine. The results of explicit and implicit analyses are
shown in Figures 55-8 to 55-10. Figure 55-8 shows the displacement contours at the start of analysis and at the end of
analysis. Note that the initial deformation of the plate grids in the implicit analysis is set to zero because the final
deformation of explicit analysis is applied to the initial location of grid points in the springback implicit analysis. In
Figure 55-9 the initial stress condition of springback implicit analysis is perfectly coincident with the final stage of
explicit analysis. The initial stress of implicit analysis causes the additional deformation in the springback implicit
analysis.
:
Explicit Simulation
t = 0.000 seconds
t = 0.018 seconds (end of explicit run)
Because the final results are applied as
the initial condition for implicit
simulation, the initial deformation of
implicit simulation is set to 0.
Implicit Simulation
Initial condition of implicit run
Figure 55-8
Final result of implicit run
Vertical (Z-direction) Displacement Contour Plot

15. CHAPTER 55 1111
Square Cup Deep Drawing using Forming Limit Diagram
Explicit Simulation
t = 0.000 seconds
t = 0.018 seconds (end of explicit run)
Because the final results are applied as the
initial condition of implicit simulation, the
initial stress of implicit simulation is the same
as the final stress of the explicit simulation.
Implicit Simulation
Initial condition of implicit run
Figure 55-9
Final residual stress of implicit run
von Mises Stress Contour Plot
The location of each grid point along the diagonal line of the plate at the end of the explicit and the springback analysis
is plotted in Figure 55-10; the maximum difference between these curves is around 0.756 mm. The centers of the
implicit and explicit sheet are positioned to have the same position as a reference, hence the largest differences tend
to appear at the ends of the sheet.

16. 1112 MD Demonstration Problems
CHAPTER 55
at the end of explicit run
5
-100
-80
-60
-40
-20
0
20
40
60
80
0
100
-5
-10
-15
Deformation to vertical direction
at the end of implicit run
-20
Distance from center
Figure 55-10
Comparison of Vertical Displacements (z-direction) After Explicit and Springback
Simulations Along Diagonal Line of Plate
Input File(s)
File
Description
nug_55a.dat
MD Nastran input file of explicit square cup deep drawing analysis using
Forming Limit Diagram.
nug_55b.dat
MD Nastran explicit input file for springback analysis.
nug_55c.dat
MD Nastran implicit input file for springback analysis
nug_55d.dat
MD Nastran stress and deformation information of explicit analysis for input
to implicit analysis
Reference
Makinouchi, A., Nakamachi, E., Onate, E., and Wagoner, R. H., “Numerical Simulation of 3-D Sheet Metal Forming
Processes, Verification of Simulation with Experiment,” NUMISHEET 1993 2nd International Conference.