Chapter 3 Advanced Contact Advanced Solid Body Contact

Chapter 3 Advanced Contact

Advanced Solid Body Contact Options Chapter Overview ANSYS Workbench – Simulation • Training Manual The various advanced solid body contact options will be discussed in detail in this chapter: – Most of these advanced options are only applicable to contact involving solid body faces, not surface bodies. – It is assumed that the user has already covered Chapter 2 Nonlinear Structural prior to this chapter. • The following will be covered in this Chapter: – – – • Contact Formulations Contact Vs. Target, Symmetric/Asymmetric Behaviors Reviewing results Pinball Region, Status Interface Treatment , offset, adjust to touch Friction The capabilities described in this Chapter are generally applicable to ANSYS Structural licenses and above. – Exceptions will be noted accordingly February 4, 2005 Inventory #002177 3 -2

Advanced Solid Body Contact Options A. Contact Training Manual – They do not interpenetrate. – They can transmit compressive normal forces and tangential friction forces. – They often do not transmit tensile normal forces. • They are therefore free to separate and move away from each other. • Contact is a changing-status nonlinearity. That is, the stiffness of the system depends on the contact status, whether parts are touching or separated. ANSYS Workbench – Simulation Description of Contact: • When two separate surfaces touch each other such that they become mutually tangent, they are said to be in contact. • In the common physical sense, surfaces that are in contact have these characteristics: February 4, 2005 Inventory #002177 3 -3

Advanced Solid Body Contact Options … Enforcing Impenetrability Condition Training Manual – When the program prevents interpenetration, we say that it enforces contact compatibility. – Simulation offers several different contact algorithms to enforce compatibility at the contact interface. F Penetration occurs when contact compatibility is not enforced. Contact Target F ANSYS Workbench – Simulation How compatibility is enforced in a contact region: • Physical contacting bodies do not interpenetrate. Therefore, the program must establish a relationship between the two surfaces to prevent them from passing through each other in the analysis. February 4, 2005 Inventory #002177 3 -4

Advanced Solid Body Contact Options … Contact Algorithm: Penalty-based Training Manual – Both of these are penalty-based contact formulations: Here, for a finite contact force Fnormal, there is a concept of contact stiffness knormal. The higher the contact stiffness, the lower the penetration xpenetration, as shown in the figure below • Ideally, for an infinite knormal, one would get zero penetration. This is not numerically possible with penalty-based methods, but as long as xpenetration is small or negligible, the solution results will be accurate. Fn ANSYS Workbench – Simulation • For nonlinear solid body contact of faces, Pure Penalty or Augmented Lagrange formulations can be used: xp February 4, 2005 Inventory #002177 3 -5

Advanced Solid Body Contact Options … Contact Algorithm: Penalty-based Training Manual Pure Penalty: Augmented Lagrange: • Because of the extra term l, the augmented Lagrange method is less sensitive to the magnitude of the contact stiffness knormal. ANSYS Workbench – Simulation • The main difference between Pure Penalty and Augmented Lagrange methods is that the latter augments the contact force (pressure) calculations: February 4, 2005 Inventory #002177 3 -6

Advanced Solid Body Contact Options … Contact Stiffness Training Manual – A large value of stiffness gives better accuracy, but the problem may become more difficult to convergence. • If the contact stiffness is too large, the model may oscillate, with contacting surfaces bouncing off of each other F F Fcontact Iteration n+1 F Iteration n+2 ANSYS Workbench – Simulation • The Normal Contact Stiffness knormal is the most important parameter affecting both accuracy and convergence behavior. February 4, 2005 Inventory #002177 3 -7

Advanced Solid Body Contact Options … Contact Stiffness Training Manual – The user may input a “Normal Stiffness Factor” with “ 1. 0” being the default. The lower the factor, the lower the contact stiffness. • Some general guidelines on selection of Normal Stiffness for contact problems: – For bulk-dominated problems: Use “Program Controlled” or manually enter a “Normal Stiffness Factor” of “ 1” – For bending-dominated problems: Manually enter a “Normal Stiffness Factor” of “ 0. 01” to “ 0. 1” ANSYS Workbench – Simulation • The default Normal Stiffness is automatically determined by Simulation. The user may enter a user-supplied value manually • The user may also have Simulation update the contact stiffness between each equilibrium iteration or substep. February 4, 2005 Inventory #002177 3 -8

Advanced Solid Body Contact Options … Contact Stiffness • As is apparent from the above table, the lower the contact stiffness factor, the higher the penetration. However, it also often makes the solution faster/easier to converge (fewer iterations) ANSYS Workbench – Simulation • Example showing effect of contact stiffness: Training Manual • The “Normal Lagrange” method will be discussed next. February 4, 2005 Inventory #002177 3 -9

Advanced Solid Body Contact Options … Contact Algorithm: Lagrange-based Training Manual – The Normal Lagrange algorithm adds an extra degree of freedom (contact pressure) to satisfy contact compatibility. Consequently, instead of resolving contact force as contact stiffness and penetration, contact force (contact pressure) is solved for explicitly as an extra DOF. • Enforces zero/nearly-zero penetration with pressure DOF • Does not require a normal contact stiffness (zero elastic slip) • Requires Direct Solver, which can be more computationally expensive F ANSYS Workbench – Simulation • Another available option is Lagrange multiplier algorithm: February 4, 2005 Inventory #002177 3 -10

Advanced Solid Body Contact Options … Contact Chattering Training Manual – If no penetration is allowed (left), then the contact status is either open or closed (a step function). This can sometimes make convergence more difficult because contact points may oscillate between open/closed status. This is called chattering – If some slight penetration is allowed (right), it can make it easier to converge since contact is no longer a step change. Contact Status Open Penetration Gap Closed Normal Lagrange Method Open Penetration Closed Gap ANSYS Workbench – Simulation • Chattering is an issue which often occurs with Normal Lagrange method Penetration Penalty-Based Method February 4, 2005 Inventory #002177 3 -11

Advanced Solid Body Contact Options … Contact Algorithm: MPC-based Training Manual – MPC, or Multi-Point Constraint, internally adds constraint equations to “tie” the displacements between contacting surfaces – This approach is not penalty-based or Lagrange multiplierbased. It is a direct, efficient way of relating surfaces of contact regions which are bonded. – Large-deformation effects also are supported with MPC-based bonded contact ANSYS Workbench – Simulation • For the specific case of “Bonded” type of contact, the MPC formulation is available. February 4, 2005 Inventory #002177 3 -12

Advanced Solid Body Contact Options … Tangential Behavior Training Manual – Similar to the impenetrability condition, in the tangential direction, the two bodies should not slide relative to each other if they are “sticking” – A penalty algorithm is always used in the tangential direction – Tangential contact stiffness and sliding distance are the analogous parameters: If “sticking”: where xsliding ideally is zero for sticking, although some slip is allowed in the penalty-based method. ANSYS Workbench – Simulation • The aforementioned options relate contact in the normal direction. If friction or rough/bonded contact is defined, a similar situation exists in the tangential direction. – Unlike the Normal Contact Stiffness, the Tangential Contact Stiffness cannot directly be changed by the user. February 4, 2005 Inventory #002177 3 -13

Advanced Solid Body Contact Options … Contact Algorithm Summary Training Manual 1 Tangential stiffness is not directly input by user – The “Normal Lagrange” method is named as such because Lagrange multiplier formulation is used in the Normal direction while penalty-based method is used in the tangential direction. ANSYS Workbench – Simulation • A summary of the contact algorithms available in Simulation is listed below: February 4, 2005 Inventory #002177 3 -14

Advanced Solid Body Contact Options … Solid Body Contact Options Although “Pure Penalty” is the default in Simulation, “Augmented Lagrange” is recommended for general frictionless or frictional contact in large-deformation problems. – Augmented Lagrange formulation adds an additional control of the automatically reducing the amount of penetration, so that is why it is preferred in general nonlinear problems • The “Normal Stiffness” is the contact stiffness knormal explained earlier, used only for “Pure Penalty” or “Augmented Lagrange” – This is a relative factor. The use of 1. 0 is recommended for general bulk deformationdominated problems. For bending-dominated situations, a smaller value of 0. 1 may be useful if convergence difficulties are encountered. ANSYS Workbench – Simulation • Training Manual – The contact stiffness can also be automatically adjusted during the solution. If difficulties arise, the stiffness will be reduced automatically. February 4, 2005 Inventory #002177 3 -15

Advanced Solid Body Contact Options … Comparison of Formulations Training Manual ANSYS Workbench – Simulation • The table below summarizes some pros (+) and cons (-) with different contact formulations: – Note that some topics, such as symmetric contact or contact detection, will be discussed shortly February 4, 2005 Inventory #002177 3 -16

Advanced Solid Body Contact Options … Comparison of Formulations Training Manual – This provides good results since the contact stiffness is high, resulting in small/negligible penetration. – MPC formulation is a good alternative for bonded contact because of its many nice features. • For frictionless or frictional contact, consider using either Augmented Lagrange or Normal Lagrange methods. – The Augmented Lagrange method is recommended, as noted previously, because of its attractive features and flexibility. – The Normal Lagrange method can be used if the user does not want to bother with Normal Stiffness value and wants zero penetration. However, note that the Direct Solver must be used, which may limit the size of the models solved. ANSYS Workbench – Simulation • For bonded contact, Simulation uses Pure Penalty formulation with large Normal Stiffness by default. February 4, 2005 Inventory #002177 3 -17

Advanced Solid Body Contact Options B. Contact vs. Target Training Manual – In Simulation, under each “Contact Region, ” the Contact and Target surfaces are shown. The normals of the Contact surfaces are displayed in red while those of the Target surfaces are shown in blue. – The Contact and Target surfaces designate which two pairs of surfaces can come into contact with one another. ANSYS Workbench – Simulation • Internally, the designation of Contact and Target surfaces can be very important February 4, 2005 Inventory #002177 3 -18

Advanced Solid Body Contact Options … Symmetric/Asymmetric Behavior Training Manual – This means that the Contact surfaces are constrained from penetrating the Target surfaces and the Target surfaces are constrained from penetrating the Contact surfaces. • If the user wishes, Asymmetric Behavior can be used – For Asymmetric or Auto-Asymmetric Behavior, only the Contact surfaces are constrained from penetrating the Target surfaces. – In Auto-Asymmetric Behavior, the Contact and Target surface designation may be reversed internally – Although it is noted that surfaces are constrained from penetrating each other, recall that with Penalty-based methods, some small penetration may occur. ANSYS Workbench – Simulation • By default, ANSYS uses Symmetric Behavior. February 4, 2005 Inventory #002177 3 -19

Advanced Solid Body Contact Options … Symmetric/Asymmetric Behavior Training Manual – On the left, the top red mesh is the mesh on the Contact side. The nodes cannot penetrate the Target surface, so contact is established correctly – On the right, the bottom red mesh is the Contact surface whereas the top is the Target. Because the nodes of the Contact cannot penetrate the Target, too much actual penetration occurs. Contact Surface Target Surface Contact Surface ANSYS Workbench – Simulation • For Asymmetric Behavior, the nodes of the Contact surface cannot penetrate the Target surface. This is a very important rule to remember. Consider the following: February 4, 2005 Inventory #002177 3 -20

Advanced Solid Body Contact Options … Contact vs. Target Designation Training Manual – If a convex surface comes into contact with a flat or concave surface, the flat or concave surface should be the Target surface. – If one surface has a coarse mesh and the other a fine mesh, the surface with the coarse mesh should be the Target surface. – If one surface is stiffer than the other, the stiffer surface should be the Target surface. – If one surface is higher order and the other is lower order, the lower order surface should be the Target surface. ANSYS Workbench – Simulation • Because of the fact that, for Asymmetric Behavior, the Contact surface cannot penetrate the Target surface but the inverse is not necessarily true, there are some guidelines in proper selection of contact surfaces: – If one surface is larger than the other, the larger surface should be the Target surface. February 4, 2005 Inventory #002177 3 -21

Advanced Solid Body Contact Options … Symmetric/Asymmetric Summary Training Manual – Only Pure Penalty and Augmented Lagrange formulations actually support Symmetric Behavior. – Normal Lagrange and MPC require Asymmetric Behavior. • Because of the nature of the equations, Symmetric Behavior would be overconstraining the model mathematically, so Auto. Asymmetric Behavior is used when Symmetric Behavior selected. – It is always good for the user to follow the general rules of thumb in selecting Contact and Target surfaces noted on the previous slide for any situation below where Asymmetric Behavior is used. ANSYS Workbench – Simulation • There are some important things to note: February 4, 2005 Inventory #002177 3 -22

Advanced Solid Body Contact Options … Reviewing Results Training Manual – For Symmetric Behavior, results are reported for both Contact and Target surfaces. – For any resulting Asymmetric Behavior, results are only available on Contact surfaces. • When viewing the Contact Tool worksheet, the user may select Contact or Target surfaces to review results. – For Auto-Asymmetric Behavior, the results may be reported on either the Contact or Target ANSYS Workbench – Simulation • The table on the previous slide alluded to an important factor in reviewing Contact Tool results – For Asymmetric Behavior, zero results are reported for Target February 4, 2005 Inventory #002177 3 -23

Advanced Solid Body Contact Options … Reviewing Results, Example 1 Training Manual – This results in auto-asymmetric behavior. Since it is automatic, Simulation may reverse the Contact and Target specification. – When reviewing Contact Tool results, one can see that the Contact side reports no (zero) results while the Target side reports true Contact Pressure. Contact Surface Target Surface ANSYS Workbench – Simulation • For example, consider the case below of Normal Lagrange Formulation with Symmetric Behavior specified. February 4, 2005 Inventory #002177 3 -24

Advanced Solid Body Contact Options … Reviewing Results, Example 2 Training Manual – This results in true symmetric behavior, so both set of surfaces are constrained from penetrating each other – However, results are reported on both Contact and Target surfaces. This means that the “true” contact pressure is an average of both results. Contact Surface Target Surface ANSYS Workbench – Simulation • In another situation, Augmented Lagrange Formulation with Symmetric Behavior is used February 4, 2005 Inventory #002177 3 -25

Advanced Solid Body Contact Options … Reviewing Results Training Manual – Easier to set up (Default in Simulation) – More computationally expensive. – Interpreting data such as actual contact pressure can be more difficult • Results are reported on both sets of surfaces • Asymmetric Behavior: – Simulation can automatically perform this designation (Auto. Asymmetric) or… – User can designate the appropriate surface(s) for contact and target manually. • Selection of inappropriate Contact vs. Target may affect results. ANSYS Workbench – Simulation • Symmetric Behavior: – Reviewing results is easy and straightforward. All data is on the contact side. February 4, 2005 Inventory #002177 3 -26

Advanced Solid Body Contact Options … Contact Detection Points Training Manual – Pure Penalty and Augmented Lagrange Formulations use integration point detection. This results in more detection points (10 in this example on left) – Normal Lagrange and MPC Formulation use nodal detection (normal direction from Target). This results in fewer detection points (6 in the example on right) – Nodal detection may handle contact at edges slightly better, but a localized, finer mesh will alleviate this situation with integration point detection. Integration Point Detection Nodal Detection ANSYS Workbench – Simulation • One additional note worth mentioning is that contact is detected differently, depending on the formulation used: February 4, 2005 Inventory #002177 3 -27

Advanced Solid Body Contact Options … Contact Detection Points Training Manual – The figure on the bottom illustrates this case: Contact Surface The target can penetrate the contact surface. Target Surface • On the other hand, there are more contact detection points if integration points are used, so each contact detection method has its pros and cons. ANSYS Workbench – Simulation • For Asymmetric Behavior, the integration point detection may allow some penetration at edges because of the location of contact detection points. February 4, 2005 Inventory #002177 3 -28

Advanced Solid Body Contact Options C. Pinball Region Training Manual – Provides computational efficiency in contact calculations. The Pinball Region differentiates “near” and “far” open contact when searching for which possible elements can contact each other in a given Contact Region. – Determines the amount of allowable gap for bonded contact. If MPC Formulation is active, it also affects how many nodes will be included in the MPC equations. – Determines the depth at which initial penetration will be resolved if present ANSYS Workbench – Simulation • The Pinball Region is a very useful concept to understand. There are several uses for the Pinball Region: February 4, 2005 Inventory #002177 3 -29

Advanced Solid Body Contact Options … Pinball Region Training Manual – If a node on a Target surface is within this sphere, Simulation considers it to be in “near” contact and will monitor its relationship to the contact detection point more closely (i. e. , when and whether contact is established). Nodes on target surfaces outside of this sphere will not be monitored as closely for that particular contact detection point. – If Bonded Behavior is specified within a gap smaller than the Pinball Radius, Simulation will still treat that region as bonded Pinball radius ANSYS Workbench – Simulation • The Pinball Region can be thought of as a sphere surrounding each contact detection point February 4, 2005 Inventory #002177 3 -30

Advanced Solid Body Contact Options … Pinball Region Training Manual – The user can change the Pinball Radius directly in the Details View of any Contact branch – The Pinball sphere will be visualized on the Contact Region label. Use the Label icon to move the annotation By specifying a Pinball Radius, one can visually confirm whether or not a gap will be ignored in Bonded Behavior. The Pinball Region can also be important in initial interference problems or large-deformation problems. ANSYS Workbench – Simulation • The size of the Pinball Region for each contact detection point is determined automatically by default. February 4, 2005 Inventory #002177 3 -31

Advanced Solid Body Contact Options D. Interface Treatment Training Manual • For Frictional or Frictionless Behavior, bodies can come in and out of contact with one another. Consequently, an initial gap is not automatically ignored since that may represent the geometry. • However, the finite element method does not allow for rigidbody motion in a static structural analysis. If an initial gap is present and a force loading is applied, initial contact may not be established, and one part may “fly away” relative to another part. ANSYS Workbench – Simulation • In the previous section, it was noted that for Bonded Behavior, a large enough Pinball Radius may allow any gap between Contact and Target surfaces to be ignored February 4, 2005 Inventory #002177 3 -32

Advanced Solid Body Contact Options … Contact Offset Training Manual – On the left is the original model (mesh). The top red mesh is the body associated with the Contact surfaces – The Contact surface can be offset by a certain amount, as shown on the right in light green. This will allow for initial contact to be established. ANSYS Workbench – Simulation • To alleviate situations where a clearance or gap is modeled but needs to be ignored to establish initial contact for Frictional or Frictionless Behavior, the Interface Treatment can internally offset the Contact surfaces by a specified amount. February 4, 2005 Inventory #002177 3 -33

Advanced Solid Body Contact Options … Contact Offset Training Manual • This slight modification may be an allowable approximation in some cases, so it is a useful tool to establish initial contact in static analyses without having to modify the CAD geometry. ANSYS Workbench – Simulation • Note that using this method will actually change the geometry since a “rigid” region will exist between the actual mesh and the offset Contact surface. February 4, 2005 Inventory #002177 3 -34

Advanced Solid Body Contact Options … Interface Treatment Training Manual – “Adjusted to Touch” will let Simulation determine what contact offset amount is needed to close the gap and establish initial contact. Note that the size of the Pinball Region will affect this automatic method, so ensure that the Pinball Radius is greater than the smallest gap distance. – “Add Offset” allows the user to specify a positive or negative distance to offset the contact surface. A positive value will tend to close a gap while a negative value will tend to open a gap. • This can be used to model initial interference fits without modifying the geometry. Model the geometry in just-touching position and change the positive distance value to the interference value. ANSYS Workbench – Simulation • In the Details view, the user can select “Adjusted to Touch” or “Add Offset” February 4, 2005 Inventory #002177 3 -35

February 4, 2005 Inventory #002177 3 -36

Workshop 3 A Contact Stiffness Bolted Joint Assembly

Advanced Solid Body Contact Options E. Workshop 3 A - Contact Stiffness Goal – In this workshop, our goal is to study the effect that contact stiffness specification has on convergence and result accuracy. • Model Description 3 D bolted assembly - 4 parts: – Bracket – Bushing – Nut – Bolt Loads and Boundary Conditions: – One fixed support – 45, 000 N Bolt preload ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -38

Advanced Solid Body Contact Options …Workshop 3 A - Contact Stiffness Training Manual • Start an ANSYS Workbench session. Browse for and open “Bolted_Joint_ws 03 A. wbdb” project file. – • This project contains a Design Modeler (DM) geometry file “Bolted_Joint_ws 03 A. agdb” and a Simulation (S) file “Bolted_Joint_ws 03 A. dsdb”. Highlight the “Bolted_Joint_ws 03 A” file and open a Simulation Session. ANSYS Workbench – Simulation Steps to Follow: February 4, 2005 Inventory #002177 3 -39

Advanced Solid Body Contact Options …Workshop 3 A - Contact Stiffness Review the contents of the model Highlight each item in the “Geometry” and “Contact” branches of the Project tree to become familiar with the model. Also, review the specifications in the Details Window for each highlighted item. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -40

Advanced Solid Body Contact Options …Workshop 3 A - Contact Stiffness Review the contents of the model (cont’d): Note especially Contact Region 6. It will be used to evaluate the pressure profile at the bushing-bracket interface after the bolt preload closes this gap. Region 6 is initially set up as an asymmetric frictionless pair using the Pure Penalty method. Recall that this algorithm depends on a contact stiffness and a very small penetration to generate forces at the interface to prevent penetration once contact is established. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -41

Advanced Solid Body Contact Options …Workshop 3 A - Contact Stiffness Review the Solution Information Branch The red lighting bolts in the Solution branch indicates an incomplete Solution run. By highlighting the “Solution Information branch and scrolling down to near the end of the output, we can see that there was an unconverged solution with the current specifications. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -42

Advanced Solid Body Contact Options …Workshop 3 A - Contact Stiffness In the Details of “Solution Information” Window, switch Solver Output to Force Convergence. This displays the same convergence data in graphical form. Note, the force convergence value oscillates up and down between iterations well above the acceptable convergence criteria. After two automatic bisections, substep 1 converges. However, substep 2 ultimately fails to converge. ANSYS Workbench – Simulation • Review the Solution Information Branch (cont’d) Training Manual February 4, 2005 Inventory #002177 3 -43

Advanced Solid Body Contact Options …Workshop 3 A - Contact Stiffness Review the Solution Information Branch (cont’d): Return to the Solver Output and scroll up the solution information worksheet to the last recorded bisection attempt. This bisection was followed shortly thereafter by a warning message about an abrupt contact status change for a contact element associated with real constant ID 15. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -44

Advanced Solid Body Contact Options …Workshop 3 A - Contact Stiffness Review the Solution Information Branch (cont’d): Again, scroll further up the solution information worksheet (near the top of the file) to find the contact specifications and calculations. The contact pair associated with the warning (real constant set 15) is the manually generated asymmetric pair for Contact Region 6. Note the large default contact stiffness (0. 923 e 6) being used. This is an order of magnitude larger then the elastic modulus of the underlying geometry. Given the relatively low stiffness of the bracket feature in this model, it is possible that the contact stiffness being used is too high for this application. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -45

Advanced Solid Body Contact Options …Workshop 3 A - Contact Stiffness We will attempt to achieve a successful convergence by adjusting the normal stiffness of Contact Region 6 downward based on the feedback reviewed in the unconverged output. • Without changing any specifications in the current tree, duplicate the Model branch as follows: • – In the existing Project tree, highlight “Bolted_Joint_ws 03 A” model – RMB – Duplicate Rename the new model branch to reflect the change that will be made – • “Bolted_Joint_ws 03 A, Norm Stiff Factor = 1 e-3” This will enable us to run a modified analysis without losing the existing information. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -46

Advanced Solid Body Contact Options …Workshop 3 A - Contact Stiffness Under the newly created model branch, highlight “Contact Region 6” • In the Details Window: • – Change the normal stiffness specification from “Program Controlled” to “Manual” – Change the normal stiffness factor from the default (1) to “ 1 e-3”. Highlight the Solution branch for this model and RMB to execute a new Solve ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -47

Advanced Solid Body Contact Options …Workshop 3 A - Contact Stiffness The solution now converges successfully in 11 iterations and no bisections. This is ideal. Bisections are a helpful automatic adjustment to achieve a converged solution, but they are not efficient as all the CPU time from the last successfully converged solution leading up to the bisection is wasted. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -48

Advanced Solid Body Contact Options …Workshop 3 A - Contact Stiffness Review the Solution Information of the successful run. Verify that the modified contact stiffness was used as expected. • Note: A second loadstep with one iteration was run automatically. This is because of the presence of bolt pretension. The first load step calculates the necessary assembly interference needed to generate the prescribed preload. The interference used in the analysis is reported as an “Adjustment” value in Details of “Pretension Bolt Load” window, along with the resulting reaction force. The second load step locks the bolt pretension element into this calculated adjustment to achieve the bolt pretension load. The calculated reaction force should match the initially applied preload. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -49

Advanced Solid Body Contact Options …Workshop 3 A - Contact Stiffness Review Contact Results at the bushing-bracket interface (nut side): • Open the Contact Tool Folder and Select Contact Region 6 – – Highlight the Pressure Results Repeat for Contact Penetration Is “ 1 e-3” an acceptable normal stiffness factor for this model? ANSYS Workbench – Simulation • Training Manual The best way to ensure an accurate result with a standard contact pair is to perform a sensitivity study with different stiffness values, stiffness updating schemes and algorithms until results converge to the same “correct” answer. Too high a stiffness can produce divergence, too low a stiffness can produce convergence but possible over penetration, an excessive bolt pretension adjustment and ultimately an inaccurate prediction of surface February 4, 2005 contact pressure profile. Inventory #002177 3 -50

Advanced Solid Body Contact Options …Workshop 3 A - Contact Stiffness Consider the following sensitivity study on the effects of changes to contact stiffness: For this model, as stiffness increases, contact penetration and the required bolt pretension adjustment decrease as expected. The maximum pressure also decreases. This is because the load is redistributing across a larger bearing area resulting in an overall decrease in maximum bearing pressure on the bushingbracket interface. Notice also the trend toward more iterations and longer run times as stiffness is increased. It is also worth noting the benefit of using the automatic stiffness updating tool between iterations to achieve convergence at the default normal stiffness factor =1. 0. ANSYS Workbench – Simulation • Training Manual Specifying the right contact stiffness is highly problem dependent and is always a balance between quality of results (accuracy) and cost (run time). Based on this study, a normal stiffness factor of 0. 10 would be satisfactory. The Augmented Lagrange algorithm has proven to provide more robust contact solutions February 4, 2005 with many applications and is recommended for standard frictionless contact. Inventory #002177 3 -51

February 4, 2005 Inventory #002177 3 -52

Advanced Solid Body Contact Options F. Frictional Contact Options Training Manual • In general, the tangential or sliding behavior of two contacting bodies may be frictionless or involve friction. – Frictionless behavior allows the bodies to slide relative to one another without any resistance. – When friction is included, shear forces can develop between the two bodies. • Frictional contact may be used with small-deflection or large-deflection analyses ANSYS Workbench – Simulation • In addition to the above, frictional contact is available with ANSYS Structural licenses and above. February 4, 2005 Inventory #002177 3 -53

Advanced Solid Body Contact Options … Frictional Contact Options Training Manual where m is the coefficient of static friction – Once the tangential force Ftangential exceeds the above value, sliding will occur Fn Ft m Fn ANSYS Workbench – Simulation • Friction is accounted for with Coulomb’s Law: February 4, 2005 Inventory #002177 3 -54

Advanced Solid Body Contact Options … Frictional Contact Options Training Manual • For frictional contact, a “friction coefficient” must be input – A Friction Coefficient m of 0. 0 results in the same behavior as “frictionless” contact – The contact formulation, as noted earlier, is recommended to be set to “Augmented Lagrange” ANSYS Workbench – Simulation • In addition to the above, frictional contact is available with ANSYS Structural licenses and above. February 4, 2005 Inventory #002177 3 -55

Advanced Solid Body Contact Options … Reviewing Results Training Manual – Contact Frictional Stress and Contact Sliding Distance can be reviewed to get a better understanding of frictional effects – For Contact Status, “Sticking” vs. “Sliding” results differentiate which contacting areas are moving ANSYS Workbench – Simulation • If frictional contact is present, additional contact output is available February 4, 2005 Inventory #002177 3 -56

Advanced Solid Body Contact Options … Summary of Contact in Simulation Training Manual – General contact behavior is defined as the interaction between parts, where contact forces are transmitted between two parts. – With contact, parts cannot penetrate through each other. They may be able to separate or slide with respect to each other. – Simulation uses three types of algorithms available to the user: Augmented Lagrange, Pure Penalty, and Normal Lagrange. MPC formulation is used only for bonded contact. • Penalty-based methods formulate contact as [K]{x}, so there is a concept of contact stiffness and some allowable penetration • Normal Lagrange solves contact pressure as a DOF directly, so there is no contact stiffness or penetration, although the solver selection becomes limited because of the unique formulation. ANSYS Workbench – Simulation • In Simulation, the user can solve contact problems: – Friction describes the tangential behavior between two moving parts. With friction defined, parts can only slide relative to one another if the tangential force exceeds the product of the normal force and coefficient of friction. February 4, 2005 Inventory #002177 3 -57

February 4, 2005 Inventory #002177 3 -58

Workshop 3 B Contact Friction Bolted Joint Assembly with Friction

Advanced Solid Body Contact Options G. Workshop 3 B - Contact Friction Goal – In this workshop, we will investigate common strategies for using frictional contact. Model Description 3 D bolted assembly - 4 parts: – Bracket – Bushing – Nut – Bolt Loads and Boundary Conditions: – One fixed support – 45, 000 N Bolt preload (along bolt axis) – 35, 000 N Bearing force ANSYS Workbench – Simulation • Training Manual (perpendicular to bolt axis) Due to the excessive run times associated with this model, all the simulations have been solved in advance. We will compare and contrast the difference between these runs. February 4, 2005 Inventory #002177 3 -60

Advanced Solid Body Contact Options …Workshop 3 B - Contact Friction Training Manual • Start an ANSYS Workbench session. Browse for and open “Bolted_Joint_ws 03 B. wbdb” project file. – • This project contains a Design Modeler (DM) geometry file “Bolted_Joint_ws 03. agdb” and a Simulation (S) file “Bolted_Joint_ws 03 B. dsdb”. Highlight the “Bolted_Joint_ws 03 B, frictionless” file and open a Simulation Session. ANSYS Workbench – Simulation Steps to Follow: February 4, 2005 Inventory #002177 3 -61

Advanced Solid Body Contact Options …Workshop 3 B - Contact Friction Review “Bolted_Joint_ws 03 B, frictionless” branch A 35, 000 N bearing load has been added to the bolted assembly model from previous workshop. Note: The bearing load option applies a variable distribution of force to the bushing surface. The first branch at the top of the project tree represents an initial attempt to simulate the structural response to the additional bearing load. Based on lessons learned in the previous workshop, the nonbonded contact specifications have been set to use the Aug. Lagrange algorithm, with a manually defined stiffness factor of 0. 1 and automatic stiffness updating between iterations. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -62

Advanced Solid Body Contact Options …Workshop 3 B - Contact Friction Review Bolted_Joint_ws 03 B, frictionless branch (cont’d) The green check marks in the Solution branch indicate a “successful” solution. Notice the two load steps were solve within one substep. This was the default initial specification as indicated in the solution output worksheet. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -63

Advanced Solid Body Contact Options …Workshop 3 B - Contact Friction Review Bolted_Joint_ws 03 B, frictionless branch (cont’d) Despite the clean solution output, with no errors, a review of the displacement results show that the first run is not correct. The addition of the bearing load pushes the bushing thru the bracket at the nut side of the assembly without resistance. Also the bonded contact pairs at the bolt head end prevent free sliding of the bushing perpendicular to the bolt. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -64

Advanced Solid Body Contact Options …Workshop 3 B - Contact Friction Review Bolted_Joint_ws 03 B, friction A number of contact related changes were made for the second run to correctly simulate the relative displacement of the parts under load. Carefully review the following changes in the second branch. • Contact Regions 1, 2, 3, 4 and 6: Change behavior to “Frictional” with a coefficient of friction of 0. 2. • Contact Region 5 represents the bolt to nut interface and will remain bonded. • Create a new frictionless contact region (#7) between the bolt and hole in bracket adjacent to the nut. • Add Frictional Stress to Solution Information branch for each of the regions except #5 (bonded) and #7 (frictionless). For region 7 we add “Number (of elements) Contacting” to help monitor solution progress. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -65

Advanced Solid Body Contact Options …Workshop 3 B - Contact Friction Review Bolted_Joint_ws 03 B, friction (cont’d) The second simulation converges successfully, this time with multiple substeps between load steps. This is by design. Friction is path dependent and result accuracy is inversely proportional to time increment size. Notice in the solution output that a nominal 5 substeps with a maximum of 20 is specified by default. Had this model experienced convergence trouble, autotime stepping would have adjusted the timestep size down to a minimum of 1/20 as necessary to resolve the problem. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -66

Advanced Solid Body Contact Options …Workshop 3 B - Contact Friction Review Bolted_Joint_ws 03 B, friction branch (cont’d) With the addition of contact friction, the results now reflect the correct response to the bearing load applied to the bushing perpendicular to the bolt axis. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -67

Advanced Solid Body Contact Options …Workshop 3 B - Contact Friction Review Bolted_Joint_ws 03 B, friction branch (cont’d) From the solution information branch, plot the number of elements in contact for Region #7. Notice that none of these elements come in contact indicating that the frictional resistance generated between bracket and bushing under the bolt preload is enough to resist the bear load. This pair is still useful, however, for evaluating the gap between the bolt and hole after the bearing load is applied. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -68

Advanced Solid Body Contact Options …Workshop 3 B - Contact Friction ANSYS Workbench – Simulation • Training Manual Review Bolted_Joint_ws 03 B, friction branch (cont’d) Plot the contact frictional stresses saved to the Solution Information Branch These results look qualitatively correct, but how accurate are they? Two basic but important aspects to consider when modeling friction is quality of mesh (especially on the curved surfaces) and time increment size (substeps) used. February 4, 2005 Inventory #002177 3 -69

Advanced Solid Body Contact Options …Workshop 3 B - Contact Friction Review Bolted_Joint_ws 03 B, friction branch (cont’d) Now that the model is producing qualitatively correct answers, consider the effect of mesh refinement in critical areas. Return to the Project page, highlight the “Bolted_Joint_ws 03 B, friction” simulation and enter the FE Environment to evaluate more closely the mesh quality of this model. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -70

Advanced Solid Body Contact Options …Workshop 3 B - Contact Friction Review Bolted_Joint_ws 03 B, friction branch (cont’d) FE Modeler opens with an Import Summary page listing all the FE statistics associated with this model. Under “Views”, highlight the “Contacts” option. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -71

Advanced Solid Body Contact Options …Workshop 3 B - Contact Friction Review Bolted_Joint_ws 03 B, friction branch (cont’d) Select the region representing the bolt-bushing interface (region #4). After zooming in on a plot of the Y -Z plane, (looking in negative X direction) notice how poorly the curved surfaces are represented by elements on these surfaces. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -72

Advanced Solid Body Contact Options …Workshop 3 B - Contact Friction Returning to Simulation, review “Bolted_Joint_ws 03 B, friction 2” branch Note the strategic mesh refinement and sizing that has been added to improve quality of results ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -73

Advanced Solid Body Contact Options …Workshop 3 B - Contact Friction Review Bolted_Joint_ws 03 B, friction 2 (cont’d) The third simulation converges successfully in a very similar pattern to previous run, except with considerably longer CPU time (in seconds) reflective of the larger DOF count (previous runs were in the order of 1500!) ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -74

Advanced Solid Body Contact Options …Workshop 3 B - Contact Friction Review Bolted_Joint_ws 03 B, friction 2 (cont’d). Plot relevant results and compare qualitatively and quantitatively and with previous run. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -75

Advanced Solid Body Contact Options …Workshop 3 B - Contact Friction Review Bolted_Joint_ws 03 B, friction 3 (cont’d) The last simulation is the same model as Bolted_Joint_03 B, friction 2 only using smaller time step size. This will force the solver to use at least a time step size of 1/10 with a minimum of 1/200 if necessary. Another useful but expensive option available to help with unconverged solutions involving friction is activation of full Newton-Raphson with unsymmetric matrices of elements. “NROPT, UNSYMM” This offers a more robust formulation of the stiffness matrix but should only be used to overcome convergence trouble. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 3 -76

Advanced Solid Body Contact Options …Workshop 3 B - Contact Friction Compare contact frictional stresses from the last three runs Course mesh, 3 substeps CPU Time = 1, 485 Refined mesh, 3 substeps CPU Time = 10, 974 Refined mesh, 10 substeps ANSYS Workbench – Simulation • Training Manual CPU Time = 26, 000 February 4, 2005 Inventory #002177 3 -77

February 4, 2005 Inventory #002177 3 -78