|
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
Loads and Boundary ConditionsAll 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
- The load from the control arm is applied as an even distribution
around the lateral control mount hole.
- Fatigue and dynamic loads are neglected.
- All materials are modeled as linear elastic.
- No weld fillet geometry or residual weld stresses are modeled.
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.
The weldment was then optimized by adding more
Pro/ENGINEER cut and slot features. An initial set of design modifications
was implemented while keeping in mind additional manufacturing costs that
may be incurred by having a radical design change. These modifications are
shown in the drawing of Figure 7. The first principal stress contours for
the first design change are shown in Figure 8. This contour plot can be
directly compared to Figure 5 of the initial design to see the effects of
the design change. Effectively, there was little change in the stress levels
while initially reducing the weight of the part by 9%.
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 User¹s Guide,
1995, Waltham, MA.
|