THREE-DIMENSIONAL MODELING OF A BOLTED CONNECTION

by

David H. Johnson, P.E.
Richard B. Englund, P.E.
Brian C. McAnlis
Kevin C. Sari
Penn State-Erie, Erie PA

and David Colombet
ANSYS Inc., Canonsburg, PA

ABSTRACT

Two-dimensional, axisymmetric models are used to study the interaction and stresses developed in the threads of a bolted connection. One problematic issue with this approach is that the 2D model simulates the threads as separate rings of material, not as the actual continuous helix. Therefore, two-dimensional modeling cannot simulate the conditions of joint tightening and sliding along the helical thread flanks when the nut is turned. In addition, the analyst must justify the 2D axisymmetric assumption as appropriate to this truly three-dimensional system. This paper presents the modeling technique used to create a "mostly-brick" meshed 3D model of a nut and bolt joint.

INTRODUCTION

There are several theories about what happens when a threaded connection is loaded axially. The most widely accepted theory claims that the first engaged thread tends to take more than its share of the load. The load then tapers off over the next few threads. This theory is generally accepted and is supported in previous FEA simulations ^[1]. This paper describes the approach used to model a 2D and a 3D threaded connection using ANSYS 5.5.

BACKGROUND

Thread load distribution and thread stresses have been studied widely for about a century. Analyses may be conveniently divided into three categories: analytical, experimental, and finite element. Of the many examples in the literature on this topic, a few are mentioned here to give the flavor of what prior work has been performed on threads. Two examples of analytical investigations are Sopwith^[2] who performed a detailed analysis, primarily of thread deformations, by theory of elasticity methods, and Wang and Marshek^[3] who modeled threads as a series and parallel network of springs. Significant simplifying assumptions were made in each case to make the analysis possible; indeed the analysis of Wang and Marshek is effectively an axisymmetric simplification of the physical system. Experimental determination of thread stresses was performed by Hetenyi^[4] using the "stress freezing" photoelastic method. In this method, a physical model is constructed from the photoelastic material, the part placed in an oven and the loads applied, the part heated and then allowed to cool, freezing the stresses into the part. After cooling, a two-dimensional slice is removed from the photoelastic part, the slice examined in a polariscope, and the stresses determined from the fringe pattern. The results obtained are indeed from a three-dimensional object but are lineally elastic since the strains are relieved when the object is sectioned.

Many finite element analyses of threaded connections have been performed, and results published. An early analysis by O'Hara^[5] examined a single thread in some detail, followed by an axisymmetric model of an entire threaded connection. By present standards the models are crude, and the models linear elastic, but the predicted distribution of load from thread to thread along the length of the engaged threads is similar to that predicted by prior experimental models and much more recent finite element analyses. The analysis by Englund and Johnson^[1] used a much more detailed, but still axisymmetric model which gave similar results and relied on similar assumptions. Neither the analytical nor finite element analyses performed to date have shown conclusively whether the axisymmetric assumption is accurate, and the experimental methods employed provide no information on the post-yield behavior of actual threads. Limits on computing power have forced the axisymmetric assumption onto prior analysts yet it is not known whether a two-dimensional model is an adequate approximation of the load distribution since the threads are clearly helical rather than axisymmetric rings. A three-dimensional model is needed to confirm or deny the validity of these prior assumptions.

TWO-DIMENSIONAL MODEL

The axisymmetric, two-dimensional, threaded connection was modeled using a radius root thread profile, Figure 1. This model represents a 2.75 in. diameter, 3 pitch threaded bolt and nut.

Figure 1. Axisymmetric Geometry

A simplification of the thread run out modeled a chamfer, placed at the last thread to the unthreaded bolt shank. This feature caused a slight stress concentration due to the sharp corner at the chamfer, but it was not near the area of interest, i.e., at the first engaged thread. The first nut thread was also chamfered, representing the normal practice of removing the "feather edge" at the nut face.

The model was meshed with 2D higher-order quadrilateral, PLANE82. A quadrilateral mesh with these elements (having mid-side nodes) adequately approximates curved boundaries with lower mesh error and fewer elements than lower-order quadrilaterals or triangle elements. In order to achieve a geometry in the threaded region that could be completely meshed with quadrilateral elements, the construction was carefully planned, making sure that all the areas were four-sided. A smaller mesh size was used around the thread roots and flanks because this was the region of the most interest. The areas away from the roots and flanks were left with a coarser mesh to cut down on total element count and run time (see Figure 2). A few triangle shaped elements were used, above the threads, in the transition to the bolt shank mesh.

Figure 2. Element Mesh

After the 2D model was completely meshed and refined to the desired extent, a tensile load was applied to the bolt shank and a constraint was applied to the nut in only the axial direction, illustrated by the node plot in Figure 3. At the interface of bolt and nut flanks, contact elements were included to allow sliding and opening of the interface. Flexible body-to-flexible body contact and target element pairs of CONTA172 and TARGE169 element types were used in the thread flank interface. The contact elements included a friction coefficient of 0.1. The materials of both the nut and bolt were common steel with an elastic modulus of 29 x 10⁶ psi (200 GPa). However, the bolt material was permitted to yield based upon a bilinear, kinematic hardening stress-strain rule. The yield point was defined at 48,000 psi (331 MPa) and the tangent modulus after yield was 340,000 psi (2.34 GPa).

Figure 3. Nodes and Boundary Conditions

This model was then solved in a nonlinear, static analysis with loads applied gradually. Large deformation effects were included along with the material plasticity and contact elements with friction, as discussed above. The axial load on the bolt shank was incremented from 10,000 lb_f (44.5 kN) to 90,000 lb_f (400 kN) in equal load steps of 10,000 lb_f (44.5 kN). Each load increment was linearly ramped over 20 substeps from the previous level to the next level. Automatic time stepping was activated. No solution convergence problems were encountered. A plot of the equivalent (von Mises) stress at the final load state is shown in Figure 4.

Figure 4. Equivalent Stress

As expected, the equivalent stress plot showed a high level of stress around the first few engaged threads then tapering off on the remaining threads. Minimal yielding occurred in the bolt in the root above the first engaged thread during the last two load steps. The newest contact elements provide interesting graphical results of contact pressure. Figure 5 shows the highest contact pressure at the first engaged thread and the pressure decreases in the remaining engaged threads.

Figure 5. Contact Element Pressure

This two-dimensional model illustrates the typical information used to evaluate the interaction between the threads of a nut and bolt. However, the two-dimensional model does not consider the helical shape of the thread flank and nor can it simulate the tightening of the connection when the nut is turned with a wrench. To allow these simulations and to measure the validity of the two-dimensional approximation, a three-dimensional model was attempted.

THREE-DIMENSIONAL MODEL

As a preface to the discussion of 3D modeling, the reader should know that this work was performed as un-funded research using the ANSYS University-High license. As such, the maximum model size is restricted to 32,000 nodes or 32,000 elements. Therefore, the modeling effort presented below is intended to produce a useful mesh, populated with a high percentage of SOLID45 brick-shaped elements. The authors realize that accuracy will be sacrificed by using these lower-order elements, but within the limitations of the university license, there is no better alternative available.

The modeling of a three-dimensional threaded connection required several attempts in order to achieve a model close to the desired results. The first attempt involved modeling a cylinder with a square center region. When modeling a simple cylinder or disk, using a square core, and dividing the surrounding region into 4 equal parts (see Figure 6) allows an all-quadrilateral or an all-brick element mesh.

Figure 6. Quadrilateral Meshing of Circle

Unfortunately, when this technique was attempted for the bolt model, the result was a helical region with rectangular faces that did not match up, producing volumes that could not be meshed with bricks. Figure 7 shows the base volumes as a translucent image. The problem faces are darker and opaque. These two rectangular areas have only a triangle region in common. Attempting to force a brick mesh into these volumes results in a meshing failure.

Figure 7. Helical Volume with a Square Core

Another method of modeling a 3D threaded connection was attempted. This second method involved using direct definition of the nodes in order to achieve a volume that was completely brick meshable. A problem with this method also occurred. At the centerline of the bolt, the nodes were lining up in a vertical direction, which resulted in an unacceptable element shape. After this attempt, it was decided to go back to the model of a cylinder with a square core. It was found that this model could have a brick meshable thread region and cylinder, but the square core could not be meshed with bricks (see Figure 8). Since the square core was at the very center of the model, away from the area of interest at the thread roots and flanks, a brick mesh was assumed unnecessary. A pyramid transition element was used where the brick mesh of the cylinder met the square core. These transition elements would then allow a regular tetrahedral mesh to be used at the very center of the square core. This brick-to-pyramid-to-tetrahedral mesh was able to mesh the bolt section of the threaded connection very well. The higher-order 20-node brick element, SOLID95, allows these various element shapes and was chosen for the 3D model meshing.

Figure 8. Bolt with Square Core

When modeling the helical nut of the threaded connection was attempted, another problem occurred. The nut was modeled by sweeping a profile of the thread 360 degrees around a desired helical path. These volumes were then copied in the vertical direction a number of times to achieve the desired thickness of the nut. All of these volumes were able to be meshed by bricks, but the resulting geometry was undesirable. At the top and bottom of the nut there was a sharp vertical face that was left over from the helical sweep. If these sharp vertical faces were left in the model, a very high stress concentration would surely result, especially at the top of the nut. It was concluded that a horizontal cut, through the entire nut, placed at the bottom of the sharp vertical face would eliminate this undesirable geometry and provide a flat face where the nut would rest against a washer. After this cut was performed, some irregular and sliver volumes resulted. Figure 9 shows these difficult volumes as opaque. These volumes could not be meshed by bricks. However, they were able to be meshed by tetrahedra, by including the transition of pyramid shapes, and that is what was done. The result was a mostly-clean geometry for the nut with several irregular and sliver volumes on the top. The bottom of the nut was not modified since it was assumed that the stresses would be low far away from the first engaged threads.

Figure 9. Face of 3D Nut Geometry

A useful fact to consider at this point was that during solution a tetrahedral element formed from the SOLID95 brick is less efficient than the SOLID92 tetrahedral. Before solving this model, the preprocessing operation, TCHG, converted the SOLID95 tetrahedral into more efficient SOLID92 tets, leaving the SOLID95 pyramids at the brick-to-tet transition regions. Figure 10 shows the element mesh and includes a sliced, close-up, capped view of the first engaged threads. The slice through the elements near the nut face shows the irregular outlines of the pyramid-to-tetrahedral transition mesh. The final step of the model construction was creating contact pairs between the engaged nut and bolt thread flanks. This process turned out to be not quite as simple as just running the "Contact Wizard". The problem encountered arose from the fact that some of the element faces on the nut flank were higher-order, either SOLID95 or SOLID92, while others were lower-order quad faces of SOLID45 elements. The choices for 3D contact elements were CONTA173 (lower-order element), CONTA174 (higher-order element), and the TARGE170 which is the compatible target for both of the 3D contact elements types. The initial attempt to create contact pairs on the engaged thread flanks produced an error in forming the proper TARGE170 faces. For that step of modeling, the nut thread flanks had been selected as the target faces. It seems that the TARGE170 element could not be used for a set of element faces that included both lower-order, SOLID45, and higher-order, SOLID92 and SOLID95, element faces.

Figure 10. 3D Element Mesh

The problem was resolved by switching the selection of contact and target faces. Luckily, all the faces on the bolt thread flanks were exclusively lower-order quad faces on SOLID45 elements and could be used for the creation of the TARGE170 elements. On the opposite side, the nut thread flanks, a mixture of CONTA173 and CONTA174 elements were used: CONTA173 on the lower-order faces of the SOLID45 mesh and CONTA174 on the higher-order triangular faces of the SOLID92 and SOLID95 mesh. Figure 11 shows the contact pairs on the bolt and nut thread flanks, on the left and right, respectively. All the contact and target elements shared the same real constant number which means that every target element checks every contact element, each iteration. This is unnecessary when you consider that a target element in the last engaged thread should never come into contact with a contact element in the first engaged thread. However, for future studies of turning the nut on the bolt, a very sophisticated overlapping of target/contact pairs would be necessary to subdivide the thread flank regions into local sections. This was not attempted for the initial 3D study of the nut and bolt interaction.

Figure 11. Target and Contact Elements

After all this modeling work, the system was meshed with the following result:

The contact elements were assigned a 0.1 coefficient of friction and element options including: unsymmetric matrices because of the friction, reasonable time/load predictions, and standard operation. Choice of the appropriate solver was the final issue before attempting to analyze this problem. While the PCG solver is recommended^[6] in many contact element solutions when unsymmetric matrices are present (for contact with dominant friction), it is not applicable. The ANSYS solution processor will automatically select the SPARSE solver which demands large memory, similar to the PCG solver. The ICCG solver is suitable for problems with unsymmetric matrices, but has had very little testing in a structural contact analysis. ICCG is used most often in acoustics and may be very sensitive to status changes in contact elements^[7]. The frontal solver for a problem of this size is very slow and creates a very large triangularized matrix file, although its RAM demand is the lowest of all the solvers. Assuming that friction would not dominate the solution, the PCG solver was used. Although this model was meshed with as much refinement as possible within the limitations of the university license, solution failure was the outcome. In consultation with the ANSYS contact development engineers^[8], the coarse, flat facets of the lower order brick elements on the thread flanks were blamed for the difficulties in attaining a converged solution. At ANSYS Inc., on an unrestricted license, the model was converted to SOLID95 and SOLID92, eliminating the lower-order SOLID45 brick element types. In addition, the lower-order contact elements, CONTA173, were entirely replaced with higher-order CONTA174 elements. This model, with 64,507 nodes and 40,556 elements, did yield a successful, converged solution. The three-dimensional model was solved in two load steps. In the first step, a small axial displacement was imposed on the bolt shank. This permitted a stable startup for this problem, allowing the contact elements to engage properly. In the second load step, the imposed displacements on the bolt shank were deleted and were replaced with a traction surface load. Figure 12 shows the equivalent stress on the bolt resulting from an axial load of 90,000 lb_f (400 kN) on the bolt shank.

Figure 12. Equivalent Stress in 3D Bolt

As the two-dimensional model showed in Figure 4, the highest stress occurs at the first engaged thread. However, in the three-dimensional model, a high stress spot is visible at the contact location corresponding to the chamfered, feather-edge of the nut. This result is curious and leads to questioning of the mesh quality in that region. Likewise, the contact element pressure result (see Figure 13) shows a high pressure spot at the same location.

Figure 13. Contact Pressure in 3D Model

CONCLUSIONS

The three-dimensional model of the nut and bolt proved to be challenging to solve and, in spite of obtaining a converged solution, the results of the three-dimensional study indicate that further mesh refinement is needed in the region of the first engaged thread on the bolt. On a positive note, comparison of the equivalent stress in the two- and three-dimensional models is quite favorable. Figures 4 and 12 are scaled to the same stress contour intervals. If we remove the high stress "spot" on Figure 12, we see very similar distribution of stress on the engaged threads. The contact pressure distribution agrees when comparing Figures 5 and 13. In observing the contact pressure in the second and third engaged threads, both the two- and three-dimensional models exhibit similar responses. Based on the results presented in this paper, further work is recommended, investigating the thread stress distribution with mesh refinement in the region around the first engaged threads. After establishing a more accurate model, studies of turning the nut can be performed, as well as determining the quality of the two-dimensional, axisymmetric approach for modeling the stresses in engaged threads.

REFERENCES

[1] Englund, R.B. and D.H. Johnson, "Finite Element Analysis of a Threaded Connection Compared to Experimental and Theoretical Research", Journal of Engineering Technology, Vol. 14, No. 2, Fall 1997, pp. 42-47.

[2] Sopwith, D. G., "The Distribution of Load in Screw-Thread," Institution of Mechanical Engineers, Proceedings, Vol. 159, No. 45, pp. 373-383, 1948.

[3] Wang, W., and Marshek, K. M., "Determination of the Load Distribution in a Threaded Connector Having Dissimilar Materials and Varying Thread Stiffness," Journal of Engineering for Industry, Vol 117, pp 1-8, 1995.

[4] Hetenyi, M., "A Photoelastic Study of Bolt and Nut Fastenings," Transactions of the ASME, Vol 65, pp. A93-A100, 1943.

[5] O'Hara, P., "Finite Element Analysis of Threaded Connections", Proceedings of Army Symposium on Solid Mechanics, Army Materials and Mechanics Research Center AMMRC, MS 74-8, pp. 99-119, 1974.

[6] ANSYS Command Reference Manual, Release 5.5, 10th edition, Sept. 1998, ANSYS Inc., EQSLV command.

[7] Personal communication with Krishna Raichur and Yongyi Zhu, ANSYS Inc., Customer Support and Development Groups, January 21-28, 2000.

[8] Personal communication with David Colombet and Yongyi Zhu, ANSYS Inc., Development Groups, February and March, 2000.

[More Clients]

[Home]