|
NONLINEAR STRESS ANALYSIS AND OPTIMIZATION OF A WELDED PLATE STEEL PRO/ENGINEER ASSEMBLY |
|||
| Andrew J. Bax Chris Andersen DRD Technology Corporation Tulsa, Oklahoma |
Shane Vander Kooi
Link Manufacturing Ltd. Sioux Center, Iowa |
||
ABSTRACT
A plate steel weldment of a truck cab air suspension
was optimized using Pro/ENGINEER Release 15 and ANSYS Revision 5.1. The steel plate
components of the weldment were created in Pro/ENGINEER. Nonlinear contact between the
weldment and its adjacent bolted attachment surface is modeled and defined inside the
Pro/ENGINEER environment. No geometric modifications were made to the Pro/ENGINEER part or
assembly files for the analysis so as to maintain the full associativity with other
Pro/ENGINEER deliverables. The assembly was modeled using shell elements with weld
connections represented with stiff beam elements also defined within the Pro/ENGINEER
environment.
The objective of the design optimization was to
reduce the weight of the weldment without increasing the maximum stresses. The weight of
the weldment was reduced 20% without significantly increasing the maximum stresses. Since
the FEA is fully associative with Pro/ENGINEER, all deliverables including parts, part
drawings, assembly solid model, assembly drawings, bill of materials, and tool paths were
automatically updated after the mount was optimized.
INTRODUCTION
The
weldment is part of a truck cab air suspension. Component weight reductions are extremely
important so as to reduce the overall weight of the semi-truck tractor. Any weight
decreased in any part of the truck allows the truck operator to increase payload, and
therefore earnings, without violating road weight limits. The weldment that was optimized
is the lateral control mount from a truck cab air suspension.
This weldment was already in production, but it was desired to reduce the material costs
and weight of future versions of this mount. The weldment was subjected to static loading
representing a lateral control rod pushing or pulling (two load cases) while the truck
travels over various road conditions. Precise weld stresses were not the objective of the
analysis runs, but nominal weld stresses at the toe of the weld were calculated for model
evaluation.
A 3D representation of the truck cab air
suspension assembly is given in Figure 1. Key components include the lateral control mount
(shown in red), frame bracket (shown in green), and the lateral control rod (shown in
blue).
FIGURE 1 PLOT OF TRUCK CAB AIR SUSPENSION ASSEMBLY
FINITE ELEMENT MODELING
Geometry and Mesh Construction
Three-Dimensional solid geometry in Pro/ENGINEER was used
to create the finite element model for solution and postprocessing in ANSYS. Seven
Pro/ENGINEER parts were used to create the plate assembly.
Plots of the original solid model weldment from Pro/ENGINEER are contained in Figures 2.
Red portions of Figures 2 is modeled solely for finite element purposes and are used in
applying the boundary conditions to the model. Pro/MESH was utilized for extracting the
mid-planes of the solid model for shell meshing. The weld connections are represented by
beam elements created in Pro/MESH. The nonlinear contact between the mount and the
adjacent C-channel (portions of the C-channel are shown in red in the above mentioned
figures) is modeled with gap elements, also created in Pro/MESH (PTC, 1995).
FIGURE 2 BACK VIEW AND FRONT VIEW OF ORIGINAL DESIGN OF LATERAL CONTROL MOUNT ASSEMBLY
The welds for the mount are represented by beam
elements in all of the analyses (Bax, 1995). Initially, test cases were run to check the
method of modeling the connection between shell elements with beams. These beams span the
distance between nodes of the shell elements created when meshing the midplanes of the
weldment. The modulus of the beam elements in the model was varied by two orders of
magnitude above and below that of plate steel. Checking deflections and stresses in the
model showed that the stress contours and displacements did not significantly change for
moduli above that of steel. However, for the test cases in which the modulus was
decreased, significant changes (>10%) in the stresses and displacements were observed.
Therefore, for the analysis runs, a stiffness equal to that of steel was utilized. (i.e.
the beams must reasonably represent the stiffness of the weld, or be stiffer). The
"weld" beams had the cross-sectional properties of circular steel rods that have
a radius of 0.005 meters. Figure 3 contains a close-up view of the beam/shell weld
connection used for the analyses.
The welded joints represent geometric
discontinuities at which the model stresses are not meaningful. Nevertheless, the stresses
at these locations are expected to be locations of maximum stress, so an approach to
evaluate these stresses was needed. The approach suggested by Gurney (1976) was used as a
basis for evaluating the weld stresses. This approach is based on the concept that
stresses at the toe of the weld can be used to predict the local stress concentrations in
the weld through a scale factor based on the joint classification. Datum curves were added
to the Pro/ENGINEER parts of the weldment so that the surfaces of the assembly parts are
divided into two or more regions. Some of the regions represent material which is welded,
while the remaining region(s) represent material that is not welded. Different material
properties are assigned to the different regions so that the weld regions can be easily
unselected in postprocessing.
The stresses in the weld connections are evaluated by reviewing the stresses adjacent to
the unselected weld elements which represent stresses at the toe of the welds.
Material Properties
Isotropic material properties were used for the optimization analyses on the weldment equivalent to 210,000 MPa and a Poisson Ratio equal to 0.3.
FIGURE 3 DETAILED VIEW OF WELD CONNECTION
All loading for the assembly was applied inside
Pro/MESH. The lateral control mount was fully restrained around the two bolt holes at a
diameter of 0.0286 meters representing support given by the adjacent washer that is not
modeled. The adjacent C-channel section that is modeled is fully restrained and provides
support when the gap elements between the mount and C-channel are closed.
Two load cases are modeled for the weldment. For
both load cases, the loads are equal and opposite in magnitude. The reciprocating load is
11,110 newtons, equally distributed around the circumference of the control arm mounting
hole, and has a line of action 3.9 degrees from the horizon. Figure 4 contains the lateral
control mount and color coded load case arrows for a graphical check of the loading.
FIGURE 4 LOAD CASES APPLIED TO MOUNT
Key
Assumptions
PRESENTATION AND DISCUSSION
OF RESULTS
As stated previously, regions of the model that are normally part of weld geometry are unselected, for postprocessing. This allows the stress contour plots provided to report nominal stresses at the toe of the welds. These nominal stresses provide a basis for comparing the effects from design changes on stresses near the welds. Figure 5 shows the first principal stress contours on the lateral control mount for Load Case 1 for the top and bottom of the shell surfaces, respectively. Figure 6 is the first principal stress contours on the lateral control mount for Load Case 2 for the top and bottom of the shell surfaces, respectively.
The stress contours in Figures 5 and 6 are from the initial design of the weldment that is known to have sufficient working life. 
FIGURE 5 FIRST PRINCIPAL STRESS
FOR TOP OF SHELLS AND BOTTOM OF SHELLS FOR LOAD CASE 1
FIGURE 6 FIRST PRINCIPAL STRESS FOR TOP OF SHELLS AND BOTTOM OF SHELLS FOR LOAD CASE 2
FIGURE 7 FIRST SET OF DESIGN
CHANGES TO LATERAL CONTROL MOUNT ASSEMBLY
FIGURE 8 FIRST PRINCIPAL STRESSES FOR BOTTOM OF SHELLS AFTER FIRST DESIGN MODIFICATION FOR LOAD CASE 1.
A second set of design modifications was performed and are shown on the Pro/ENGINEER drawing of Figure 9. The first principal stress contours for this second design change are shown in Figure 10. This contour plot can be directly compared to Figure 5 of the initial design to see the effects of this change. Again, there was little change in the stress levels while reducing the weight of the part by a total of 20%.
FIGURE 9 SECOND SET OF DESIGN CHANGES TO LATERAL CONTROL MOUNT ASSEMBLY
FIGURE 10 FIRST PRINCIPAL STRESSES FOR BOTTOM OF SHELLS AFTER SECOND
DESIGN MODIFICATION FOR LOAD CASE 1
CONCLUSION
No
geometric modifications were made to the Pro/ENGINEER assembly described in this paper so
as to guarantee full associativity between the drawings, parts, manufacturing, and other
Pro/ENGINEER deliverables.
These assemblies can be and were further optimized for weight and shape. This model shows
that finite element shell modeling with nonlinear contact can be performed on Pro/ENGINEER
assemblies.
ADDITIONAL WORK TO BE PERFORMED
The nominal
stresses reported at the toe of the welds are accurate as the local error estimation in
these areas range from 5-15%. Detailed, accurate weld stresses would require
three-dimensional solid geometry with some estimate of the residual stresses incurred from
the welding operation. That approach, however, would involve longer, more expensive
analysis runs that may slow down the design process. Previous work (Gurney) with welded
structures suggest a methodology of evaluating welds at the toe for fatigue design. This
approach allows for faster analysis runs due to simpler geometry and smaller model size
from which design changes can be quickly made. In order to utilize this approach, scale
factors for calculating weld stresses from stresses at the toe of the welds must be
determined. This could be accomplished by generating a S-N curve for this
weldment. For a
given loading, ANSYS could be used to calculate the corresponding stresses while fatigue
testing could be done to obtain the number of cycles. A range of loadings could be tested
to fully define the S-N curve. This curve could then be used as a design tool for future
design modifications to this weldment.
After acquiring some correlation among other similar
weldments, this S-N curve could
possibly be applied to a wide range of similar weldments that are constructed using the
same weld techniques.
Plasticity is not considered for this analysis.
Some of the stresses shown in this report may be above yield while, in reality, local
yielding would have occurred which redistributes the load over a larger portion of the
model. Often, plasticity needs to be included in the analysis when stresses significantly
higher than yield are encountered. Further analysis on this weldment could include
plasticity in the future.
REFERENCES
Bax, A. J., 1995, ANSYS/ProFEA - For Pro/ENGINEER Release 15, Revision 4, DRD Corporation, Tulsa, OK.
Gurney, T.R., 1976, ³Fatigue Design Rules for Welded Steel Joints², The Welding Institute Research Bulletin, Vol. 17, pp. 115-124.
Parametric Technology Corporation, Release 15 Pro/MESH Userıs Guide, 1995, Waltham, MA.