Bonded Contact between Shell Faces in ANSYS® Mechanical (Workbench) v14.5
ANSYS Mechanical (Workbench) has many settings for contact between surface body (shell) faces. This article examines a setup to employ with bonded contact across a gap between surface body midplanes in large deflection nonlinear analysis.
Figure 1: WB Mechanical Model with Parallel Flat Surface Bodies
Creation of a Bonded Contact Pair between Surface Body Faces
If surface bodies are created on the midplane of the thin solids that they approximate, the surface bodies that lie on top of each other will have a gap between the midplanes. The gap size will often be greater than the tolerance used in the automatic creation of contact pairs when geometry is imported into Workbench Mechanical. Either the tolerance employed in the creation of contact pairs will have to be modified, and the contact pairs regenerated, or manual contact pairs will need to be created between overlapping surface bodies.
Figure 2: Surface Bodies with Thickness and Shell Mesh
|Figure 3: Surface Body Thickness|
Figure 2 above shows a pair of surface bodies, and the mesh that results when they have been meshed with shell elements. The shell thicknesses entered for the surface bodies in the model close the gap between the surface bodies so that they touch on a pair of faces. In this example, there is a 4 mm gap between the surface bodies. These surface bodies are intended to lie on the midplanes of the shell elements, so in the example, both surface bodies have been set to a thickness of 4 mm, as illustrated in Figure 3 to the right. The upper image in Figure 2 shows a thickened view of the shell elements, so that closure of the gap is illustrated.
|Figure 4: Orientation of Contact and Target Shell Face Normals|
As can be seen in Figure 1 above, the “Top” of each of these surface bodies happens to face in the –Y direction in the global coordinate system. Consequently, the Contact and Target surfaces do not face each other. To get the contact pair to work, the Details settings for Contact Shell Face and for Target Shell Face for the contact pair can either be left as “Program Controlled”, or set by the user to choices of Top and Bottom, so that the red Contact face and the blue Target face will look towards each other. This is required to get the resulting target and contact elements in ANSYS to attach to each other without implied penetration and solution failure.
Continuing with the Details definition of the contact pair, the contact will be set to Bonded, which permits both Symmetric contact with penalty-based formulations, and Asymmetric contact with all formulations. In the present example, a Symmetric behavior is selected.
|Figure 5: Definition and Advanced Contact Settings|
In Figure 5, the Formulation has been set to “Augmented Lagrangian” although a Penalty setting has also been satisfactory in testing. The Detection Method has been set to “Nodal-Projected Normal From Contact” which was found to produce deflection and stress plots that were preferable to those resulting from alternative settings.
Figure 6 below shows the Detection Method choices in a drop-down listing. Users may want to experiment with the consequences of these various choices. The Projected choice is a relatively new addition to ANSYS.
|Figure 6: Detection Method Alternatives|
Figure 7 shows equivalent stress and Y deflection with Detection Method “Nodal-Projected Normal From Contact”.
Figure 7: Equivalent Stress and Deflection with the
“Nodal-Projected Normal From Contact” Detection Method
Contrast this with Figure 8, the consequence with “Program Determined”. The deflection plot has similar amplitude, but the stress does not show the Figure 7 result, where “thick” region stresses are higher at outer layers, and smaller at the bonded interface, which acts like the mid-plane of an 8mm thick shell.
Figure 8: Equivalent Stress and Deflection with the “Program Determined” Detection Method
For this reason, the “Nodal-Projected Normal From Contact” of Figure 7 will be preferred.
Other Detail settings in the Advanced section in Figure 5 have been left as Program Determined in this example, although users may prefer to increase the Normal Stiffness factor, and to set a Pinball Region manually.
Loading on the Model
The edge at one end of the surface body pair was fixed, and a force was applied to the other end.
Figure 9: Loads on the Surface Bodies
The force has components in the Global X and Y directions:
Figure 10: Force Components
The Analysis Settings for this example were set to perform a Large Displacement analysis, with non-default Output Controls set to output contact information that would make it possible to measure the force transmitted across the contact pair in the model. Force Results probes are not satisfied until Contact Miscellaneous is set to “Yes”.
Figure 11: Analysis Settings--Large Displacement with Extra Output Controls
As is often the case in finite element analysis, if users are unsure whether a Large Displacement analysis is warranted, a model can be run with Large Displacement activated, and if Large Displacement was not required, convergence usually adds just one additional iteration.
Outputs from the Example Model
Many postprocessing objects were added to the test model, in order to observe the consequences of contact pair options on deflections, stresses, force reactions across the contact, and Contact Tool outputs:
Figure 12: Solution Objects
In Figure 12, two of the three Force Reaction objects were suppressed—“Contact (Underlying Element) choice produced near-zero numbers, and Contact (Contact Element) had unsatisfied inputs in most cases. The “Target (Underlying Element)” choice produced a force result matching the edge input forces applied.
|Figure 13: Contact Tool Results|
Contact Tool results were requested on the “Contact” side only, so although a symmetric bonded contact was requested, a result is only plotted on the lower body. Because the Top of the lower body faces the –Y direction, results are plotted on the -Y side face of the thickened view of the lower surface body. Figure 13 shows Status, Frictional Stress, Pressure and Sliding Distance. The pressure and sliding distance values are non-zero because of the finite penalty stiffness values in the contact elements.
After a survey of settings for a contact pair between the faces of two surface bodies, observing stress, deflection, contact, and force reaction results in a large displacement model, it was found that satisfactory results were seen when a face-to-face contact pair between the surface bodies was set to Bonded, Symmetric, and a Detection Method of “Nodal-Projected Normal from Contact”. The force across the contact pair could be measured with a Force Reaction probe for the contact pair, with Extraction set to “Target (Underlying Element)”.
Figure 14: Contact Pair Inputs and Outputs
The above Figure 14 setting for Shell Thickness Effect did not have a substantial effect on results, but was set to “Yes” to capture the offset of the contact surface from the midplane, which might have a stronger effect with thicker shells. The Behavior entry in the Definition section could have been “Asymmetric” or “Program Controlled” but was set “Symmetric” so that the finite size of the contact and target elements would leave less disconnection at the ends of the contact zone, and would cope better with variant element sizes on the contact and target faces.
Users could try optional settings for many of the Details in the contact pair settings, including assignment of the Contact Body and the Target Body, and manual assignment of the Contact Shell Face, Target Shell Face, and Pinball Region size. In the present example, adequate results were realized with many Program Controlled settings.
Convergence did not become an issue with these settings for the present Large Displacement example. The Analysis Settings had tightened Nonlinear Controls settings for Force Convergence and for Displacement Convergence in this example, although these are generally at the discretion of the user.
Users should keep in mind that may of the complications of contacts with Surface Bodies and their shell elements are avoided with Thin Surface method solid meshing with SOLSH190 elements of solid bodies.