Upsetting of a cylindrical billet: coupled temperature-displacement and
adiabatic analysis
This example illustrates coupled temperature-displacement analysis
in a metal forming application.
The case studied in this example is an
extension of the standard test case that is defined in Lippmann (1979); thus,
some verification of the results is available by comparison with the numerical
results presented in that reference. The example is that of a small, circular
billet of metal that is reduced in length by 60%. Here the problem is analyzed
as a viscoplastic case, including heating of the billet by plastic work. Such
analysis is often important in manufacturing processes, especially when
significant temperature rises degrade the material. The problem is also
analyzed in
Abaqus/Standard
using a porous metal material model. The same problem is used in
Upsetting of a cylindrical billet: quasi-static analysis with mesh-to-mesh solution mapping (Abaqus/Standard) and adaptive meshing (Abaqus/Explicit)
to illustrate mesh rezoning in
Abaqus/Standard
and adaptive meshing in
Abaqus/Explicit.
The specimen is shown in
Figure 1:
a circular billet, 30 mm long, with a radius of 10 mm, compressed between flat,
rough, rigid dies. All surfaces of the billet are assumed to be fully
insulated: this thermal boundary condition is chosen to maximize the
temperature rise.
The finite element model is axisymmetric and includes the top half of the
billet only since the middle surface of the billet is a plane of symmetry. In
Abaqus/Standard
elements of type CAX8RT, 8-node quadrilaterals with reduced integration that allow for
fully coupled temperature-displacement analysis, are used. A regular mesh with
six elements in each direction is used, as shown in
Figure 1.
In addition, the billet is modeled with CAX4RT elements in a 12 × 12 mesh for both
Abaqus/Standard
and
Abaqus/Explicit
analyses.
The contact between the top and the lateral exterior surfaces of the billet
and the rigid die is modeled with a contact pair. The billet surface is defined
by means of an element-based surface. The rigid die is modeled as an analytical
rigid surface or as an element-based rigid surface. The mechanical interaction
between the contact surfaces is assumed to be nonintermittent, rough frictional
contact in
Abaqus/Standard.
Therefore, the contact property includes two additional specifications: a
no-separation contact pressure-overclosure relationship to ensure that
separation does not occur once contact has been established and rough friction
to enforce a no-slip constraint once contact has been established. In
Abaqus/Explicit
the friction coefficient between the billet and the rigid die is 1.0.
The problem is also solved in
Abaqus/Standard
with the first-order fully coupled temperature-displacement CAX4T elements in a 12 × 12 mesh. Similarly, the problem is solved
using CAX8RT elements and user subroutines
UMAT and
UMATHT to illustrate the use of these subroutines.
No mesh convergence studies have been performed, but the comparison with
results given in Lippmann (1979) suggests that these meshes provide accuracy
similar to the best of those analyses.
The
Abaqus/Explicit
simulations are performed both with and without adaptive meshing.
Material
The material definition is basically that given in Lippmann (1979), except
that the metal is assumed to be rate dependent. The thermal properties are
added, with values that correspond to a typical steel, as well as the data for
the porous metal plasticity model. The material properties are then as follows:
Young's modulus:
200 GPa
Poisson's ratio:
0.3
Thermal expansion coefficient:
1.2×10−5 per °C
Initial static yield stress:
700 MPa
Work hardening rate:
300 MPa
Strain rate dependence:
;
/s,
Specific heat:
586 J/(kg°C)
Density:
7833 kg/m3
Conductivity:
52 J/(m-s-°C)
Porous material parameters:
Initial relative density:
0.95 (
0.05)
Since the problem definition in
Abaqus/Standard
assumes that the dies are completely rough, no tangential slipping is allowed
wherever the metal contacts the die.
Boundary conditions and loading
The kinematic boundary conditions are symmetry on the axis (nodes at
0,
in node set AXIS, have
0
prescribed) and symmetry about 0
(all nodes at 0,
in node set MIDDLE, have
0
prescribed). To avoid overconstraint, the node on the top surface of the billet
that lies on the symmetry axis is not part of the node set
AXIS: the radial motion of this node is
already constrained by a no-slip frictional constraint (see
Common Difficulties Associated with Contact Modeling in Abaqus/Standard
and
Common Difficulties Associated with Contact Modeling Using Contact Pairs in Abaqus/Explicit).
The rigid body reference node for the rigid surface that defines the die is
constrained to have no rotation or -displacement,
and its -displacement
is prescribed to move 9 mm down the axis at constant velocity. The reaction
force at the rigid reference node corresponds to the total force applied by the
die.
The thermal boundary conditions are that all external surfaces are insulated
(no heat flux allowed). This condition is chosen because it is the most extreme
case: it must provide the largest temperature rises possible, since no heat can
be removed from the specimen.
One of the controls for the automatic time incrementation scheme in
Abaqus/Standard
is the limit on the maximum temperature change allowed to occur in any
increment. It is set to 100°C, which is a large value and indicates that we are
not restricting the time increments because of accuracy considerations in
integrating the heat transfer equations. In fact, the automatic time
incrementation scheme will choose fairly small increments because of the severe
nonlinearity present in the problem and the resultant need for several
iterations per increment even with a relatively large number of increments. The
maximum allowable temperature change in an increment is set to a large value to
obtain a reasonable solution at low cost.
In
Abaqus/Explicit
the automatic time incrementation scheme is used to ensure numerical stability
and to advance the solution in time. Mass scaling is used to reduce the
computational cost of the analysis.
The amplitude is applied linearly over the step because the default
amplitude variation for a transient, coupled temperature-displacement analysis
is a step function, but here we want the die to move down at a constant
velocity.
Two versions of the analysis are run: a slow upsetting, where the upsetting
occurs in 100 seconds, and a fast upsetting, where the event takes 0.1 second.
Both versions are analyzed with the coupled temperature-displacement procedure.
The fast upsetting is also run in
Abaqus/Standard
as an adiabatic static stress analysis. The time period values are specified
with the respective procedure options. The adiabatic stress analysis is
performed in the same time frame as the fast upsetting case. In all cases
analyzed with
Abaqus/Standard
an initial time increment of 1.5% of the time period is used; that is, 1.5
seconds in the slow case and 0.0015 second in the fast case. This value is
chosen because it will result in a nominal axial strain of about 1% per
increment, and experience suggests that such increment sizes are generally
suitable for cases like this.
Results and discussion
The results of the
Abaqus/Standard
simulations are discussed first, beginning with the results for the
viscoplastic fully dense material. The results of the slow upsetting are
illustrated in
Figure 2
to
Figure 4.
The results for the fast upsetting coupled temperature-displacement analysis
are illustrated in
Figure 5
to
Figure 7;
those for the adiabatic static stress analysis are shown in
Figure 8
and
Figure 9.
Figure 2
and
Figure 5
show the configuration that is predicted at 60% upsetting. The configuration
for the adiabatic analysis is not shown since it is almost identical to the
fast upsetting coupled case. Both the slow and the fast upsetting cases show
the folding of the top outside surface of the billet onto the die, as well as
the severe straining of the middle of the specimen. The second figure in each
series (Figure 3
for the slow case,
Figure 6
for the fast case, and
Figure 8
for the adiabatic case) shows the equivalent plastic strain in the billet. Peak
strains of around 180% occur in the center of the specimen. The third figure in
each series (Figure 4
for the slow case,
Figure 7
for the fast case, and
Figure 9
for the adiabatic case) shows the temperature distributions, which are
noticeably different between the slow and fast upsetting cases. In the slow
case there is time for the heat to diffuse (the 60% upsetting takes place in
100 sec, on a specimen where a typical length is 10 mm), so the temperature
distribution at 100 sec is quite uniform, varying only between 180°C and 185°C
through the billet. In contrast, the fast upsetting occurs too quickly for the
heat to diffuse. In this case the middle of the top surface of the specimen
remains at 0°C at the end of the event, while the center of the specimen heats
up to almost 600°C. There is no significant difference in temperatures between
the fast coupled case and the adiabatic case. In the outer top section of the
billet there are differences that are a result of the severe distortion of the
elements in that region and the lack of dissipation of generated heat. The
temperature in the rest of the billet compares well. This example illustrates
the advantage of an adiabatic analysis, since a good representation of the
results is obtained in about 60% of the computer time required for the fully
coupled analysis.
The results of the slow and fast upsetting of the billet modeled with the
porous metal plasticity model are shown in
Figure 10
to
Figure 15.
The deformed configuration is identical to that of
Figure 2
and
Figure 5.
The extent of growth/closure of the voids in the specimen at the end of the
analysis is shown in
Figure 10
and
Figure 13.
The porous material is almost fully compacted near the center of the billet
because of the compressive nature of the stress field in that region; on the
other hand, the corner element is folded up and stretched out near the outer
top portion of the billet, increasing the void volume fraction to almost 0.1
(or 10%) and indicating that tearing of the material is likely. The equivalent
plastic strain is shown in
Figure 11
(slow upsetting) and
Figure 14
(fast upsetting) for the porous material;
Figure 12
and
Figure 15
show the temperature distribution for the slow and the fast upsetting of the
porous metal. The porous metal needs less external work to achieve the same
deformation compared to a fully dense metal. Consequently, there is less
plastic work being dissipated as heat; hence, the temperature increase is not
as much as that of fully dense metal. This effect is more pronounced in the
fast upsetting problem, where the specimen heats up to only 510°C, compared to
about 600°C for fully dense metal.
Figure 16
to
Figure 18
show predictions of total upsetting force versus displacement of the die. In
Figure 16
the slow upsetting viscoplastic and porous plasticity results are compared with
several elastic-plastic and rigid-plastic results that were collected by
Lippmann (1979) and slow viscoplastic results obtained by Taylor (1981). There
is general agreement between all the rate-independent results, and these
correspond to the slow viscoplastic results of the present example and of those
found by Taylor (1981). In
Figure 17
rate dependence of the yield stress is investigated. The fast viscoplastic and
porous plasticity results show significantly higher force values throughout the
event than the slow results. This effect can be estimated easily. A nominal
strain rate of 6 sec is maintained throughout the event. With the viscoplastic
model that is used, this effect increases the yield stress by 68%. This factor
is very close to the load amplification factor that appears in
Figure 17.
Figure 18
shows that the force versus displacement prediction of the fast viscoplastic
adiabatic analysis agrees well with the fully coupled results.
Two cases using an element-based rigid surface to model the die are also
considered in
Abaqus/Standard.
To define the element-based rigid surface, the elements are assigned to rigid
bodies using an isothermal rigid body constraint. The results agree very well
with the case when the analytical rigid surface is used.
The automatic load incrementation results suggest that overall nominal
strain increments of about 2% per increment were obtained, which is slightly
better than what was anticipated in the initial time increment suggestion.
These values are typical for problems of this class and are useful guidelines
for estimating the computational effort required for such cases.
The results obtained with
Abaqus/Explicit
compare well with those obtained with
Abaqus/Standard,
as illustrated in
Figure 19,
which compares the results obtained with
Abaqus/Explicit
(without adaptive meshing) for the total upsetting force versus the
displacement of the die against the same results obtained with
Abaqus/Standard.
The agreement between the two solutions is excellent. Similar agreement is
obtained with the results obtained from the
Abaqus/Explicit
simulation using adaptive meshing. The mesh distortion is significantly reduced
in this case, as illustrated in
Figure 20.
Fast upsetting case with 144 CGAX4T elements, using the fully dense material and an element-based
rigid surface for the die with surface-to-surface contact.
Fast upsetting case with fully dense material modeled with CAX4RT elements and without adaptive meshing; penalty mechanical
contact.
References
Lippmann, H., Metal
Forming
Plasticity, Springer-Verlag, Berlin, 1979.
Taylor, L.M., “A
Finite Element Analysis for Large Deformation Metal Forming Problems Involving
Contact and Friction,” Ph.D. Thesis, U. of
Texas at
Austin, 1981.
Figures
Figure 1. Axisymmetric upsetting example: geometry and mesh (element type CAX8RT). Figure 2. Deformed configuration at 60% upsetting: slow case, coupled
temperature-displacement analysis,
Abaqus/Standard. Figure 3. Plastic strain at 60% upsetting: slow case, coupled
temperature-displacement analysis,
Abaqus/Standard. Figure 4. Temperature at 60% upsetting: slow case, coupled
temperature-displacement analysis,
Abaqus/Standard. Figure 5. Deformed configuration at 60% upsetting: fast case, coupled
temperature-displacement analysis,
Abaqus/Standard. Figure 6. Plastic strain at 60% upsetting: fast case, coupled
temperature-displacement analysis,
Abaqus/Standard. Figure 7. Temperature at 60% upsetting: fast case, coupled
temperature-displacement analysis,
Abaqus/Standard. Figure 8. Plastic strain at 60% upsetting: fast case, adiabatic stress analysis,
Abaqus/Standard. Figure 9. Temperature at 60% upsetting: fast case, adiabatic stress analysis,
Abaqus/Standard. Figure 10. Void volume fraction at 60% upsetting: porous material, slow coupled
temperature-displacement analysis,
Abaqus/Standard. Figure 11. Plastic strain at 60% upsetting: porous material, slow coupled
temperature-displacement analysis,
Abaqus/Standard. Figure 12. Temperature at 60% upsetting: porous material, slow coupled
temperature-displacement analysis,
Abaqus/Standard. Figure 13. Void volume fraction at 60% upsetting: porous material, fast coupled
temperature-displacement analysis,
Abaqus/Standard. Figure 14. Plastic strain at 60% upsetting: porous material, fast coupled
temperature-displacement analysis,
Abaqus/Standard. Figure 15. Temperature at 60% upsetting: porous material, fast coupled
temperature-displacement analysis,
Abaqus/Standard. Figure 16. Force-deflection response for slow cylinder upsetting,
Abaqus/Standard. Figure 17. Rate dependence of the force-deflection response,
Abaqus/Standard. Figure 18. Force-deflection response: adiabatic versus fully coupled analysis,
Abaqus/Standard. Figure 19. Force-deflection response:
Abaqus/Explicit
versus
Abaqus/Standard. Figure 20. Deformed configuration at 60% upsetting: slow case,
Abaqus/Explicit
(without adaptive meshing, left; with adaptive meshing, right).
