By Ionut Ghionea
Ionut Ghionea, Lecturer, Faculty of Engineering, University Politehnica of Bucharest
The finite element method (FEM) has become a widely used and indispensable engineering tool for critically analyzing new component and product designs. Since its introduction, continuous updates by most suppliers have made the FEM technique even more accurate and easier to apply. To appreciate just how much FEM has improved recently, its capabilities are illustrated in an example of a fixture design for attaching a wedge to two principal bolts on planar surfaces. The fixture contains a circular eccentric gear (cam) and a two-arm bridle which clearly shows that the cam’s working profile is a circular arc.
The scope of the finite-element analysis for this device is to identify the zones with high stresses and their values. This does not consider the stresses that result from the technological processes when the piece is machined, or the rigidity of supports and tightening elements.
The assembly consists of a bedplate, abutment bolts, a holder with a spherical head, a cam, an attachment flange for gripping cams, and associated hardware, Fig.1.
Fig. 1. The fixture device in isometric view.
The holder actuates the cam and fixes the piece on the device while friction forces hold the eccentric gear in place. To simplify the FEM calculus and explanations, the coiled spring is not represented. Bending, tension or compression stresses are applied to the components as the device is actuated.
This analysis uses the Generative Structural Analysis module from the CATIA software package. Also, the 3D modeling of the device and its assembly require two other modules: Part Design and Assembly Design. A very important step in the FEM analysis process addresses how the device’s components are assembled using numerous constraints of the following types: coincidence, surface contact, linear contact, offset and fix, Fig. 2.
Fig. 2. Fragment of the assembly constraints list.
In this example, these constraints apply:
Coincidence constraints between the axes of the swell pin and of the cam hole.
Coincidence constraints between the axes of the dowel screw and its corresponding nuts.
Linear-contact constraints between the active surface of the cam and the guide’s planar surface, and between the tightening curved surface from the bridle’s end and the piece’s planar surface.
Surface-contact constraint between the supporting surface of abutment bolts and the bedplate.
Each component is made of steel, with appropriate material properties applied: Young modulus (2 X 1011 N/m2), Poisson ratio (0.266), density (7860 kg/m3), thermal expansion (1.17 X 10-5 K) and yield strength (2.5 X 108 N/m2).
Using the module Generative Structural Analysis, a node network discretization is done for each component, establishing the dimension, the type of each finite element and the tolerance
between the real model and the discretized one, Fig. 3. The finite element type is chosen as Linear because a Parabolic element type could extend calculation time excessively. (Later, the effect of this choice will be examined.)
Fig. 3. Node network discretization.
Using the assembly constraints, the next step involves setting the physical constraints, necessary in the simulation of the tensile stresses, generated by the application of a force on the holder. Thus, the physical constraints are chosen after the assembly constraints and they are of these following types: Fastened Connection Property, Pressure Fitting Connection Property and Contact Connection Property. A small section of these physical constraints is shown, Fig 4, along with some of their symbols positioned on the respective components.
As an example, the coincidence assembly constraints between the swell pin axis and the axis of the cam hole become physical constraints of type Fastened Connection Property. The coincidence assembly constraints between the abutment bolt axes and the corresponding axes drilled in the bedplate become physical constraints of type Pressure Fitting Connection Property. Also, the surface contact assembly constraint between the guide and the bedplate become a physical constraint of type Contact Connection Property.
Fig. 4. Fragment of the physical constraints list and symbols.
The next step in this application consists of adding a fixing restraint (Clamp), positioned on the base surface of the bedplate. In this step we establish the applied load on the holder, a Distributed Force of 600 N value. This force has the device’s working direction (holder-cam-bridle), tightening the piece. The specification tree, positioned on the left side of the CATIA interface, will show the sub-elements “Clamp.1” and “Distributed Force.1”, Fig. 5.
Fig. 5. Application of the fixing restraint and the loading force.
Launching of the finite-element analysis process can begin after these preliminary stages (choosing the discretization values and imposing constraints and loads) The procedure is very specific to the CATIA software. Finally, the specification tree is completed with the sub-element Static Case Solution, which may contain different solutions depending on the instruments used: Deformation, Von Mises Stress, Displacement, Principal Stress and Precision.
To determine the tensions caused by the applied loading force, use the Von Mises Stress results. Use of the Image Extrema instrument allows highlighting (locating) the minimum and maximum tension values, at a global or local level. The specification tree, Fig. 6, presents the sub-elements “Von Mises Stress” and “Extrema” which shows on the device’s 3D assembly model some indicators of the extreme values. This figure also shows the node network discretization.
Fig. 6. Representation of the Von Mises results and the localization of the extreme tensions.
From the colors and values palette, which correspond to the Von Mises model representation, you can see the maximum tension in the assembly is 2.63 X 107 N/m2, located on the holder, in the joint area between its end and the cam. The first analysis shows an error of 45.81%, but this result is too inaccurate, so an assembly-node network-discretization refinement is necessary, followed by another analysis process, applying the instrument New Adaptivity Entity.
Fig. 7. Tension representation and values for cam.
In this analysis, the user imposed a 20% error after three iterations, but in the second step of analysis, the error is decreased only to 26.57%. That eror reduction is accompanied by a maximum tension increase on the holder, in the same area of joint: 5.18 X 107 N/m2. If these values (error percent and tension) are not acecptable, another node-network discretization refinement will be required, using the finite element type Parabolic, which will further decrease the percentage of error.
Results of analysis
The CATIA facility shows tension for each component (Figs. 7, 8 and 9) indicating tensions in colors-and-values palettes for these three components.
Fig. 8. Tension representation and values for bridle.
Fig. 9. Tension representation and values for dowel screw.
• For the cam, the most stressed areas are: the assembly hole with the holder (3.11 X 107 N/m2), the assembly hole with the swell pin (1.1 _ 107 N/m2) and the contact surface with the guide.
• For the bridle, the most stressed areas are: the surfaces of the assembly hole with the swell pin (2.25 _ 107 N/m2) and the planar contact surface with the conical pocket washer (3.35 _ 106 N/m2). On the contact area with the piece, the bridle presents tensions of 1.1 _ 105 N/m2.
• For the dowel screw, the most stressed areas are at the upper end, in the proximity of the assembling zone with the nuts (6.66 _ 106 N/m2).
• The assembly zone with the bedplate is stressed to a tension of 6.17 _ 106 N/m2. Thus, the tension distribution along the dowel screw indicates that it is loaded and bent.
: Design World :
Filed Under: FEA software