Technical Tips for Surface-to-Surface Contact Analysis in MES

Abstract

Mechanical Event Simulation (MES) provides the ability for moving parts to contact each other. While the software automates many of the parameters related to surface-to-surface contact, some models will benefit from adjustments by the user.

This paper consists of three sections. The first section outlines the basic steps involved in a contact analysis. The second section discusses contact parameters used in defining contact pairs. Since there is not a single set of values for the contact parameters that will provide an accurate solution for all models, the user must have a good understanding of the functionality of each parameter to determine a proper set of values for the given problem. The third section focuses on difficulties in contact analysis and provides several quick solutions to avoid or remove these difficulties.

1. Basic Steps of Contact Analysis

The basic steps for performing contact analysis are as follows:

1-1. Create the Geometry and Mesh

In order to perform an accurate contact analysis, a reasonably smooth contact surface and a uniform mesh over the contact surfaces are highly recommended. Furthermore, since surface mesh alignment can impact the performance of the whole analysis, surface meshing on each adjacent contact surface should be carefully done to achieve a better convergence rate. In linear contact, the mesh on the two surfaces should be perfectly matched to each other as shown in Figure 1 (a). However, in MES, a perfectly matched mesh could cause severe contact chattering. When this chattering occurs, it inevitably results in a very poor convergence rate. In order to avoid or at least minimize this problem, when small relative motion between the contact surfaces is expected, it is recommended that the mesh should have the nodes on one surface located in the middle of the nodes on the other surface as shown in Figure 1 (b).

Figure 1: Proper Mesh for Contact Analysis in
(a) Linear Stress Analysis and (b) Nonlinear/MES Stress Analysis

1-2. Identify and Define the Contact Pairs

Before the user starts a contact analysis, he or she must clearly identify where the contact interaction might occur during the given time frame. Contact pairs can be defined either by selecting two surfaces on the model, right-clicking and choosing "Surface-to-Surface Contact", or by right-clicking in the graphics area (with nothing selected), choosing "General Surface-to-Surface Contact" and manually filling in the Contact Pairs spreadsheet. Not only could multiple target surfaces interact with one master surface, but self contact is also possible in a large deformation problem such as a rubber elasticity analysis. In such cases, the user must define multiple contact pairs that cover all potential contact interaction. Once the potential contact pairs have been identified, the user specifies the master and target surfaces in the surface contact definition screen.

The contact pairs can consist of any two arbitrary surfaces. However, in order to speed up the contact search, the user should only specify the contact pairs that will definitely interact within the given event duration. Especially in problems that involve small amounts of sliding contact, the analysis will converge more rapidly if the number of contact elements is minimized. This can be achieved by specifying a contact radius, which will ensure that all generated contact elements have a length that is initially shorter than the contact radius. Provided the contact radius is larger than the distance the parts move relative to each other, contact will be maintained over the entire range of motion. (See the explanation of maximum initial distance in section 2-8.)

For cases where it is difficult for the user to predict the relative motion of contact pairs, the processor provides an automatic updating scheme to help the user set up the contact pairs efficiently with only a few contact surfaces covering the entire contact area. However, this may require a large amount of memory in a 3-D analysis. If the necessary memory is not available, the user must split the large contact surface into several smaller contact surfaces.

1-3. Determine the Master and Target Surfaces

The main purpose of the contact algorithm is to prevent the penetration of nodes on the target surface into the master surface. Therefore, determining the master and target surface is a very important step and should be considered very carefully. Since the choice of the master and target surfaces can impact the accuracy of the final solution and convergence rate, this topic will be discussed in detail in section 2.

1-4. Determine the Contact Parameters

The most difficult step in contact analysis is determining the proper contact parameters. When the user chooses the "Automatic" setting for a contact parameter, the processor calculates an appropriate value based on the initial contact surface geometry, the mesh and material constants. However, this default value may not be valid after the bodies undergo large deformation. When the contact part is expected to experience large deformation, the user should consider this before starting the analysis and determine an appropriate value. This issue will be discussed in section 2.

1-5. Determine the Nonlinear Solution Scheme and Capture Rate

The processor provides six types of nonlinear solution schemes (under the "Analysis: Parameters...: Advanced" menu, on the "Equilibrium" tab): modified Newton-Raphson (NR), full NR, combined NR, modified NR with line search (LS), full NR with LS and combined NR with LS. It is difficult to say which one is the best choice. However, normally full NR with or without LS is strongly recommended for a contact analysis.

1-6. Apply Necessary Loads and Constraints

Specify data needed for the analysis including loads, constraints and analysis parameters. Although it may be realistic to "leave parts free to fly around" and come into contact, some models can be improved by partially restraining the parts. For example, a pin passing through a yoke and clevis is free to rotate in reality, but will not usually rotate because there is no force to cause the pin to rotate. In this situation, applying constraints to prevent the pin from rotating can reduce the contact chattering that may occur if the pin tries to rotate. Likewise, the axial motion of the pin may be insignificant, so constraints to prevent axial motion can reduce the runtime.

1-7. Perform the Analysis

Analyze the model using the MES processor.

1-8. Review the Results

When two smooth bodies are in contact, the user expects a relatively smooth stress contour over the contact surfaces. However, due to the non-smoothness of the contact surface, this simple expectation may not be achieved with a coarse mesh. In such a case, the user may need to refine or modify the mesh in the problematic area and analyze the model again.

2. Contact Parameters

This section will discuss each contact parameter in detail. For simple models, the user may start the analysis after defining each contact pair and use the default settings provided by the processor. However, quite often, the user will need to experiment with the contact parameters to find an appropriate set for a particular model.

2-1. Contact Updating

In the main surface contact dialog, the user needs to be aware of the parameters in the "Contact Element Updating Parameters" section located in the right bottom of the dialog. These parameters control the updating of contact element parts; that is, when individual contact elements are added to the analysis (because the surfaces are in close proximity), and when individual contact elements are removed from consideration. For example, two gears meshing need to only consider the contact elements for the teeth that are in contact. The contact elements between the other teeth can be removed from the analysis until those teeth approach each other.

Three options are available in the "Updating" drop-down box, "Never", "User-defined" and "Automatic". The "Never" option will not allow regenerating or updating of contact element parts. The "User-specified" option allows the advanced user to explicitly specify the frequency and radius of contact search to regenerate contact element parts. If the "Automatic" option is selected, the radius and the frequency are varied according to the relative motion of the two contact surfaces. A linear acceleration assumption is used to calculate the contact radius. A frequency of 10 times per second is used as the initial frequency.

The best scenario for the "Automatic" option is when two bodies experience large relative motion while they are in contact such as sliding, in which the possible contact area or range should cover all of the contact surfaces for the event duration, but the time history of the relative motion of two contact surfaces is not known. The "User-defined" option can also be used for the above case, but the user must know the relative motion of the contact surfaces so that contact is not lost. The "Never" option along with a maximum initial distance is the best choice when two contact bodies undergo very small relative motion during the analysis. It can save time used in updating the contact element part and reduces the amount of contact elements in each part.

2-2. Contact Type

MES provides two major types of contact surface setup; point-to-surface and surface-to-surface. This can be specified by clicking in the "Parameters" column for each contact pair. The resulting dialog will contain a "Contact type" drop-down box in the "Parameters" section. Point-to-surface contact indicates that the nodes on the target part/surface cannot pass through the surface on the master part/surface. Note that this does not prevent the nodes on the master part/surface from passing through the surface of the target part/surface. Surface-to-surface contact provides better contact detection, but at the expense of generating more contact elements. It indicates that the nodes on the target part/surface cannot pass through the surface defined by the nodes on the master part/surface (just like point-to-surface contact), and the nodes on the master part/surface cannot pass through the surface on the target part/surface.

When determining which type of contact to use, the mesh, geometry and material should be carefully considered. The "Automatic" option will review these factors and provide the best setting for the given problem. However, the "Automatic" option may not pick the best contact type when large deformation occurs in the analysis. In this case, to check the validity of the setup done by the "Automatic" option, the user will need to do a test using the following procedure (algorithm is a simplified version of the procedure used by the processor):

Figure 2: Flow Chart for Determining the Contact Type

2-3. Contact Stiffness

MES will either calculate the contact stiffness for the model or the user can specify a value for the contact stiffness. This can be done by clicking "Parameters: Advanced". If the user wants to specify the contact stiffness, activate the "User-specified contact stiffness" checkbox in the "General" tab and specify the appropriate value in the "Contact stiffness" field. In both cases, the value keeps constant and is independent of the contact status. If the stiffness is too small, large penetration of nodes into the master surface is inevitable. If the stiffness is too large, the geometric boundary condition over the contact area is exactly fulfilled, but quite often the equilibrium iteration becomes unstable. High values of contact stiffness will lead to ill–conditioning of the global stiffness matrix and result in poor convergence. When the wrong value is chosen, there is no way to adjust the contact stiffness to avoid these two cases during calculation, so the user must stop the analysis and change the contact parameters to proceed.

In order to minimize this circumstance, MES provides adaptive contact stiffness. This is a smart way to adjust the contact stiffness during the analysis based on the current contact status. The basic rule that is widely used in selecting contact stiffness is the one-tenth rule. This rule states that contact stiffness is normally no larger than one tenth of the smallest Young’s modulus of the materials in the contact pair. However, this is not perfectly applicable to every contact problem.

When the "User-specified contact stiffness" checkbox is not activated, MES will calculate the contact stiffness using the following equation (for 2-D):

f_s is the scaling parameter and the default value is 0.1. E is the smaller of the Young's modulus for the two materials in the contact pair. L is the dimension of the contact line and S is the area of the element. In 3-D, L and S are simply replaced with S and V, where S is the contact surface and V is the volume of the element. The ratio, L²/S, is calculated from the element base in both the target and contact surfaces and then averaged. A value of 1.0 is used for this ratio when contact with beam or truss elements is involved.

2-4. Adaptive Contact Stiffness

The automatic contact adjusting algorithm is adapted to avoid unrealistic results from an improper contact stiffness. It is selected by activating the "Use adaptive contact stiffness method" checkbox. Even using the automatic calculation option, the chosen value might not be good enough to prevent large penetration or contact chattering when the contact surfaces experience large deformation or two contact surfaces are under very high compression for a very short time. MES monitors the contact status in each iteration and adjusts it when any problems such as negative penetration into master surfaces or contact chattering are detected.

2-5. Contact Tolerance

Contact distance is defined as the separation between the two surfaces when they come into contact. Determining the proper contact distance is one of the most important steps in obtaining a high-quality solution and fast convergence. A large contact distance might cause a numerical problem and very unrealistic contact results. A small value could lead to failure in detecting the target node and large negative penetration. One tenth of the smallest dimension of the surface mesh is generally recommended.

MES has two options for specifying a contact distance. The first option is for the user to specify the contact tolerance. Normally, the contact tolerance should be smaller than the physical gap between the parts; this indicates that there is no interference at the beginning of the analysis. But to simulate an initial interference or press fit, the contact tolerance can be adjusted to give the desired amount of interference. In this situation, it is typical to see the time step be reduced at the beginning of the analysis until the parts come into their new equilibrium.

The second option (and the default) for specifying the contact tolerance is to let the processor calculate it automatically. If the "User-specified contact tolerance" checkbox is not activated in the "General" tab of the "Controls and Parameters for Contact Pair" dialog, and if an initial physical gap between the two contact surfaces exists, a contact distance will be calculated based on each surface geometry, curvature and mesh size. Once it has been calculated, this value will remain constant for each contact pair in order to avoid any discontinuity introduced by a sudden change in the contact force at the element boundary.

Normally, the value calculated from the automatic setting is less than the real physical gap so that contact does not occur until a load is applied. However, when one of the contact surfaces has a "high" initial velocity (i.e., without constraints, gravitational force is high enough to make "high" initial velocity), an initial contact interaction with a contact tolerance larger than the initial gap is highly recommended. This can be obtained by relocating the moving part closer to the other part than the contact interaction distance. This can save analysis time and improve convergence when two parts start in contact. But when the moving part has complex motion such as rotation about an arbitrary axis, the user must perform calculations to determine the location of the target nodes when contact will occur.

2-6. Contact with Friction

MES uses the classical friction algorithm, so called, Coulomb friction. In the basic Coulomb friction model, two contact surfaces can resist shear stress up to a certain amount, determined from friction coefficients and normal contact pressure, before they experience relative sliding motion. The Coulomb friction model is defined as τ = µP, where µ is the friction coefficient and p is the normal contact pressure. MES provides an option for defining a static µ_s and dynamic µ_d friction coefficient. Once the shear stress exceeds µ_sP obtained from the static friction coefficient, the two surfaces start sliding and the shear stress becomes µ_dP where the dynamic friction coefficient is used. The friction coefficients can be any non-negative value less than 1.0. By default, MES assumes frictionless contact.

In frictionless contact, the element stiffness matrices are symmetric. Once friction is involved, the matrix becomes unsymmetric. Using an unsymmetric solver is computationally more expensive than using a symmetric solver. For the sake of efficiency, MES enforces symmetry of element stiffness so that the symmetric solver can be used for frictional contact.

When frictional contact is considered in the analysis, the solution process becomes highly vulnerable from the sliding process. Once the contact surfaces start sliding, the equilibrium state before the sliding is no longer valid and the processor must try to find a new equilibrium state during the solution process. Furthermore, poor convergence is possible due to the symmetry approximation.

2-7. Extend Contact Element Side Ghost Area

If the target node does not lie within the contact tolerance of an element on the master surface, then no contact is occurring. When the master surface has sharp edges, this leaves a "ghost area" where the target node can move without being in contact. This causes contact chatter. See Figure 3 (a). In order to avoid missing such contact, MES provides an additional contact parameter.

Figure 3: Target Node Does Not Lie within the Contact Search Territory

The parameter "Extend contact element sides" is selected in the "Parameters: Advanced: Geometry" tab. This input will enlarge the contact surface up to a specific value. See Figure 3 (b). If the "Automatic" option is selected, MES will calculate the value. If the "By specified amount" option is selected, the value must be specified by the user. The rule of thumb for selecting this value is the contact tolerance, but it can be any value smaller than the contact tolerance. When a contact surface has many sharp edges and large sliding motion, this value plays a very important role for better convergence.

2-8. Maximum Initial Distance

By default, the point-to-surface contact type generates contact elements between each node on the target surface and the surface of the master part/surface (and vice versa if using the surface-to-surface contact type). If the parts move significantly relative to each other, the automatic contact updating (section 2-1) is the best option to let the processor determine which points are actually in contact. But in cases where the parts have little motion relative to each other, a faster analysis can be obtained if the user can minimize the number of contact elements that get generated. This is where the "Maximum initial distance" input field under the "Parameters: Advanced: Geometry" tab comes into play. It specifies to create contact elements only if their initial length is less than the entered amount.

Imagine a pin inside a yoke and clevis. If the pin does not rotate relative to the yoke, then the left side of the pin will not make contact with the right side of the hole. Setting the "Contact Element Updating" to "Never" allows the "Maximum initial distance" field to be entered. Then, setting the maximum initial distance to a small distance -- such as the size of one element -- will create just enough contact elements to connect the pin to the hole at adjacent nodes. The result will be a smaller model and less checking of the contact element status, so the analysis will run faster.

3. Problems and Solutions

Definitions of some important contact parameters have been presented in the previous section. In this section, four difficulties that the user can confront in contact analysis will be discussed.

3-1. Large Deformation – Hyperelastic Model

Relatively small deformation is assumed when computing contact parameters except for the adaptive contact stiffness and contact group updating. When contact surfaces undergo large displacement or large deformation such as more than 50% strain even in the localized area, the basic assumption used in calculating contact parameters, such as master and target surfaces, contact type and contact extend area, may no longer be valid. The user may need to consider the deformed shape to capture the mesh and geometry changes when they choose the parameters.

Figure 4 (a) shows that the contact searching method fails to detect a proper target node after large deformation. Considering the initial geometry, point-to-surface contact appears to be a proper choice because the segments on the master surface are much larger than the segments on the target surface. However, after the target part deforms, the segment size of the target surface becomes bigger than the master surface. This leads to a situation where segment m1-m2 fails in detecting any target node and leads to lost contact and penetration of the target surface. In this circumstance, surface-to-surface contact is highly recommended. Regarding the extension of the contact area, when the initial contact surface is flat or has low curvature, the automatic setting to calculate the areas of extended contact produces a small extension. When the part deforms, the contact areas may open up, leaving a "ghost area" or hole in the contact in which the contact with the target node is not detected (see section 2-7). As shown in Figure 4 (b), the extended contact area is large enough in the original geometry to detect the target node. After experiencing large deformation, the extended contact area is not large enough to detect the target node at m2. This leads to failure in detecting s3. If the user expects large deformation of bodies where the contact surfaces are defined, the user needs to consider specifying a large number instead of using the automatic setting. However, the user-defined number should be smaller than the contact tolerance.

(a)

(b)

Figure 4: Failure in Contact Search after Large Deformation, (a) by Stretch of Element and (b) by Change of Curvature

3-2. Contact between Soft and Hard Material

In order to perform a contact analysis, the user first needs to identify the characteristics of the parts that will have contact interaction. When a very soft material is in contact with a metal, the one-tenth rule and stiffness calculation equation might fail in providing a proper value and cause serious contact chattering or large penetration. Even using the adaptive contact stiffness scheme, poor convergence is inevitable until a proper value is found by several iterations. In such cases, the user needs to explore some test cases with a simple 2-D contact model using the same material and loading conditions. Simply test several contact stiffnesses, increasing or decreasing from a relatively small number compared to the Young’s modulus of the soft material by a factor of 10 until the smallest value that doesn’t allow large penetration has been found. When the first test has been completed, check the convergence rate by simply counting the number of iterations. If the global convergence is not good and there is no large penetration, the stiffness value could be too large and needs to be reduced and tested again.

3-3. Part Moving Fast – Impact Problem

This is the most challenging problem in a contact analysis. Normally, it is considered an "impact" analysis rather than contact analysis. When a fast moving part interacts with other parts, high-frequency loads are introduced and a smaller time step is necessary. Furthermore, when the general MES time-integration method is adapted, high energy loss is inevitable which leads to over-damped behavior. The most common problem in this case is that one part penetrates the other part without contact initiation. This happens because the target node just skips the contact interaction zone as shown in Figure 5. (When two surfaces are farther apart than the "Contact interaction distance", contact is not checked on a node-by-node basis. So if the moving object moves from one side of the body but outside of the contact interaction distance to the other side of the body, the solver never sees that contact occurred.) One possible solution for this is using initial velocity for the moving part. If the velocity of the moving part right before it contacts the other part can be found, move that part into the contact active zone and apply an initial velocity. This helps avoid serious time reduction or pass through. Another solution is using a relatively smaller time step than the normally accepted one.

Figure 5: Skipping Contact Interaction Zone

3-4. Non-smooth Surface

Two issues originate from non-smoothness of the contact surface. The first one is poor convergence and the second is poor results. The normal vector of the contact force experiences a sudden change in direction when a target node travels across the element boundary and this is inevitable as long as discretized geometry is being considered. This non-smoothness can cause oscillation across the element boundary and the target node can become stuck in the element boundary. The best way to handle this problem is smoothing the contact surface by introducing more elements or adjusting the contact element side extension. It is quite difficult to obtain a fast converged solution, especially if the target surface has sharp convex edges. In order to avoid such a convergence problem, the user may need to smooth out the sharp edge by refining the mesh in the region where sudden curvature changes occur.

Non-smooth surfaces, quite often, lead to unacceptable answers. For example, when one circular ring is fitted inside of a second circular ring, one can expect a uniform stress contour along the contact surface. However, this is difficult to achieve without smoothing of the contact surfaces since the contact force is calculated from the relationship between master surfaces and target nodes that are not uniformly distributed over the master surfaces. In this case, the user should refine the mesh over the contact surface or redistribute the target nodes uniformly as shown below.

Figure 6: Non-smooth Contact Surface

In this section, ways to identify and resolve problems that can be encountered during contact analysis have been discussed. However, the user should understand that in highly nonlinear problems such as contact, the solution procedures are highly vulnerable to small factors that could be missed or ignored in consideration.

Conclusion

Many issues that might not show up in a normal nonlinear solution procedure could show up when contact is involved. The user may need to carefully check the material model settings and all contact parameters as suggested in the previous sections when they encounter convergence problems or poor results from a contact analysis.

Some models will solve fine with the automatic and default settings while other models may benefit from some changes. In general, these are the changes that have been found to be the most common:

• Use Full Newton (with or without line search) for the nonlinear solution scheme (section 1-5).
• For small relative motion between surfaces, adjust the mesh so that the nodes do not align on the adjacent parts (section 1-1) and set a maximum initial distance to minimize the number of contact elements generated (section 2-8).
• Set the contact type to point-to-surface, which can reduce the number of contact elements generated, provided the geometry is suitable for this contact type (section 2-2).
• For curved surfaces or sharp edges, the extend contact element sides parameter may affect the rate of convergence (section 2-7).
• Adjust the contact stiffness, which can help with the rate of convergence (harder to converge if contact is too stiff) and amount of penetration between the surfaces (soft contact stiffness results in more penetration) (section 2-3).

As with all FEA analyses, simplify where possible.