The following discussion centers around the results obtained with Abaqus/Standard. The results of the Abaqus/Explicit simulation are in close agreement with those obtained with Abaqus/Standard for both the node-to-surface and surface-to-surface contact pair formulations.
Figure 2 shows the deformed configuration after Step 2 of the analysis. Figure 3 and Figure 4 show contour plots of plastic strain and the von Mises stress at the end of Step 2 for
the fully coupled analysis using CAX4RT
elements. These plots show good agreement between the results using the two contact
formulations in Abaqus/Standard. The plastic deformation is most severe near the surface of the workpiece, where plastic
strains exceed 100%. The peak stresses occur in the region where the diameter of the
workpiece narrows down due to deformation and also along the contact surface. Figure 5 compares nodal temperatures obtained at the end of Step 2 using the surface-to-surface
contact formulation in Abaqus/Standard with those obtained using kinematic contact in Abaqus/Explicit. In both cases CAX4RT elements are used.
The results from both of the analyses match very well even though mass scaling is used in
Abaqus/Explicit for computational savings. The peak temperature occurs at the surface of the workpiece
because of plastic deformation and frictional heating. The peak temperature occurs
immediately after the radial reduction zone of the die. This is expected for two reasons.
First, the material that is heated by dissipative processes in the reduction zone will cool
by conduction as the material progresses through the postreduction zone. Second, frictional
heating is largest in the reduction zone because of the larger values of shear stress in
that zone.
Similar results were obtained with the two types of stabilization
considered. Adaptive automatic stabilization is generally preferred because it
is easier to use. It is often necessary to specify a nondefault damping factor
for the stabilization approach with a constant damping factor; whereas, with an
adaptive damping factor, the default settings are typically appropriate.
Figure 6
compares results of a thermally coupled analysis with an adiabatic analysis
using the surface-to-surface contact formulation in
Abaqus/Standard.
If we ignore the zone of extreme distortion at the end of the bar, the
temperature increase on the surface is not as large for the adiabatic analysis
because of the absence of frictional heating. As expected, the temperature
field contours for the adiabatic heating analysis, shown in
Figure 6,
are very similar to the contours for plastic strain from the thermally coupled
analysis, shown in
Figure 3.
As noted earlier, excellent agreement is observed for the results obtained
with
Abaqus/Explicit
(using both the default and enhanced hourglass control) and
Abaqus/Standard.
Figure 7
compares the effects of ALE adaptive meshing
on the element quality. The results obtained with
ALE adaptive meshing show significantly
reduced mesh distortion. The material point in the bar that experiences the
largest temperature rise during the course of the simulation is indicated (node
2029 in the model without adaptivity).
Figure 8
compares the results obtained for the temperature history of this material
point using
Abaqus/Explicit
with the results obtained using the two contact formulations in
Abaqus/Standard.
Again, a very good match between the results is obtained.