yongyi zhu——ANSYS接触摸拟的最佳解决方案

2020-02-27 939浏览

1.Best Practices for Contact Modeling using ANSYS This presentation contains ANSYS, Inc. proprietary information. It is not to be distributed to others. Yongyi Zhu, PhD Research and Development Fellow July, 2017 1 © 2016 ANSYS, Inc. July 19, 2017
2.Why are these best practices important? • Contact is the most common source of nonlinearity and is often the most difficulty to solve! • With typical structural problems, the presence of nonlinear contact can often be the biggest reason for increased solution times. • Poorly defined contact may lead to unstable contact conditions. These conditions usually mean bad convergence and lost time. • With ideal contact conditions, contact results converge much more quickly and the results tend to be smoother. 2 © 2016 ANSYS, Inc. July 19, 2017
3.What this presentation will cover • Section 1: Contact Model Setup andVerification:– Contact Generation and Management Tips • Section 2: Getting Ready for theSolver:– Mesh Quality & Mesh Sizing – Setting the Contact Formulation – Understanding the Effect of Contact Stiffness – Advantages of MPC Contact – Specifying Pinball Radius – Initial Interface Adjustment • Section 3: Dealing With Non Convergence – Diagnostic Tools – Contact Results Tool – Overcoming Rigid Body Motions – Procedure for Overcoming Convergence Difficulties 3 © 2016 ANSYS, Inc. July 19, 2017
4.Set the Right Units System • Always verify the model units. Bad units can results in inaccurate solution and bad convergence due to tolerance, precision, and numerical round off issues. • Checkoutoutput:– contact length is too small – elastic moduli or force/mass quantities is too big CONFIDENTIAL 4 © 2016 ANSYS, Inc.Tip:Select mm-N units for the most contact models. July 19, 2017
5.Mesh Quality • Poor mesh quality in solid elements can cause convergence problems. • A difficult contact problem may be diverging simply because of the mesh •Tip:Use aggressive shape checking for nonlinear contact problems. Poor Mesh Quality on Contact Surface Better Mesh Quality 5 © 2016 ANSYS, Inc. July 19, 2017
6.Mesh Sizing • On curved surfaces, or surfaces which deform to a curve, having sufficient contact elements to closely follow the curvature is essential for smooth results. • This is especially true for nonlinear contact • Use similar element sizes for the source and target sides. •Tip:Use Contact Sizing for sub-surface meshcontrol:Element size transitions very slowly! without contact sizing with contact sizing Too few elements Better set elements with similar mesh density 6 © 2016 ANSYS, Inc. July 19, 2017
7.Using Match Mesh Control 7 © 2016 ANSYS, Inc. Mesh generated as separate parts Use Contact Match controls to match mesh Node merge can be added as second step to make mesh conformal Tet Mesh OnlyTip:Match mesh feature aids accurate definition of contact interface and improves convergence July 19, 2017
8.Using the Worksheet The worksheet view is a great way to review all of the contact settings Rows can be sorted by clicking on column header Column Visibility can be controlled via RMB 8 © 2016 ANSYS, Inc. July 19, 2017
9.Using the Initial Contact Tool • Use the Initial Contact Tool to quickly learn about contact status before solving. • Inserted under Connection Folder • Information reported which pairs are open/closed, how much initial penetration, inactive pairs, etc. • Color coding to help user identify possible issues • Contour results such as status and Penetration can be calculated 9 © 2016 ANSYS, Inc. July 19, 2017
10.Section 2: Getting Ready for the SolverTip:Using Robust Defaults Robust defaults that solve the largest variety of contact situations is our goal In general the “Program Controlled” settings in Mechanical match the MAPDL solver defaults. Exceptions include Behavior(autoasymmetric) 10 © 2016 ANSYS, Inc. July 19, 2017
11.ContactDiscretization:Linear Hex vs Higher order Tet Surface-to-Surface 8-Nodes Hex Trends over time 10-nodes Tets 10-Nodes Tets More efficient Good for flat contact surfaces Only for simple geometries whenever structure mesh is possible 11 © 2016 ANSYS, Inc. July 19, 2017 Good for curve contact surfaces Good for Complex geometries with unstructure mesh Smoother results
13.Contact DetectionMethods:Notes • Surface integration point method allow for additional points to detect penetration between surfaces - Default method for Penalty and Augmented Lagrange method. – However it is poor when contact occurs at corners or edges. • Nodal based detection methods are default for MPC and Normal Lagrange method. – For contacts at corners (such as interference fit problems, threaded connector models), best results are obtained when either Nodal – Normal to Target (or) Normal for Contact. • Nodal – Projected Normal From Contact – For true surface-surface contacts, it provides good results with minimal contact pressure spikes at nodes – Convergence behavior is also better if mesh is adequately discretized at contact surfaces. – For best performance, use similar mesh size for both contact and target surfaces. 13 © 2016 ANSYS, Inc. July 19, 2017
14.Contact DetectionMethods:Notes • Nodal – Projected Normal From Contact – Always use Projection method for contact involving gasket layers so that stress and strain distribution near contacting edges is more smooth. – Always use Projection method for Acoustic FSI interaction. – Avoid using the projected contact in conjunction with MPC bonded contact when initial geometric gap/penetration exists. Close gap/penetration by issuing CNCH,MORPH or use the nodal detection method. – For 3D higher order elements, use Normal Lagrange in conjunction with projection based option for the best accuracy. 14 © 2016 ANSYS, Inc. Using Projected contact July 19, 2017 Unexpected spiky results Using Gauss detection
15.Understanding Contact Formulation • Augmented Lagrange (Default): Suitable for most problems. • PurePenalty:– Contact occurring only on Edge or Corner • MPC (Multi-Point Constraint): Ideal for all bonded/no-separation contact when there is no over-constraint • NormalLagrange:– Highest accuracy – Contact with material nonlinearities – Between shells or thin layers – Interference fit – Large Sliding 15 © 2016 ANSYS, Inc. July 19, 2017
16.ModelingContacts:Normal Lagrange Method Notes Penetration critical applications (accuracy). Contact with predominant material nonlinearity. Contact between shells or thin layers. Large sliding problem. Pretension bolts Small deformation due to small amount of loading. Contact at corners, edges. Suitable for solving threaded connectors, press fit joints, seals, etc. In which underlying stresses vary with contact stiffness. Convergence is still not achieved after several attempts by adjusting contact stiffness. 16 © 2016 ANSYS, Inc. July 19, 2017
17.Contact StiffnessFactor:Tips • For contacts with difficulty converging, lower the stiffness • For pretension problems, use a stiffness factor greater than one, because penetration can strongly influence the pretension forces. • Always set “Update Stiffness” to a frequency of “Each Iteration” (Default in WB Mechanical) • Aggressiveoptions:remedy chattering or preventing rigid body motion when initial contact conditions are not well posted. • When there is difficulty converging due to high penetration, increase the stiffness. 17 © 2016 ANSYS, Inc. July 19, 2017
18.ModelingContacts:MPC Method Notes • Use MPC contact for bonded and no-separation contact as much as possible unless overconstraints exist. • Ideal for shell-solid, shell-shell, and beam-shell contacts • Interface with small gap/penetration – It avoids spurious frequencies for modal analysis • Gaps are frequently encountered in CAD models – Seam Weld preparation – Suppressed auxiliary parts (e.g. seals) • Rather than modify the geometry to fill the gap, they can be accurately ignored when using MPC Contact or a fixed joint. – Joints/beam connection are recommended if convergence difficulties arise for large rotation problems. 18 © 2016 ANSYS, Inc. July 19, 2017
19.Viewing the MPC EquationsTip:Check overconstraints Contact status 19 © 2016 ANSYS, Inc. July 19, 2017 After the solution is done MPC equations and other “FE Connections” can be graphically viewed
20.Small Sliding vs Large Sliding Assumption • Finite-sliding option allows for arbitrary separation, sliding, and rotation of the contact interfaces. It is computationally expensive, but guarantees solution accuracy. • Small-sliding option assumes relatively small sliding motion (<20% contact length) occurs on contact interface, but arbitrary rotations of contacting bodies is permitted. It improves solution robustness for models having a bad quality geometry or mesh and non-smooth contact interfaces. • The small-sliding logic can cause nonphysical results if the relative sliding motion does not remain small. Use the finitesliding option if you are not absolutely sure that the smallsliding logic is appropriate. • Use the small-sliding option with greatcaution:– EKILL command applied to contact/target elements – Debonding (TB,CZM) – A general contact definition – Rezoning (REZONE) or mesh nonlinear adaptivity (NLADAPTIVE) 20 © 2016 ANSYS, Inc. July 19, 2017
21.21 © 2016 ANSYS, Inc. True Linear ContactConcept:• For bonded and no separation contact, if no other nonlinearities exist in the model (plasticity, large deformation, or unilateral contact), a linear solution (no equilibrium iteration) is good enough to obtain an accurate solution.Advantages:• Reaction forces are always balanced comparing with the existing “one iteration NL solution” (NEQIT,1,forcer). Applied force = 4N Reaction forces Linear contact From contact elements 4.002N (Reaction balance) From underlying elements of contact 4.N From underlying elements of target 4.N 1 iteration with NL 6.4634e7 (Reactions don’t 4.N contact balance) 4.N July 19, 2017
22.Contact Pinball  ANSYS solver internally categorizes the state of contactas:Far field, Near field, Touching  Category is based on if the distance between contact and target surface is lesser (or) greater than pinball radius  For interference problems, ensure that the pinball radius is greater than the maximum interference  In bonded contact and noseparation contacts, any region between the surfaces which touches or lies within pinball radius will be assumed to be in contact 22 © 2016 ANSYS, Inc. July 19, 2017
23.Contact Pinball - Notes Pinball radius • This is one of the most important parameters to get the desired contact result – Effective PINB : measure the largest gap in your model via Initial Contact Tool, then specify PINB a little bit larger than the gap, e.g if the largest gap is X, use PINB=X+X/10. • If you introduce a large pinball, you will have risks to introduce the spurious region. • Use large pinball for load step which resolves interference fit. Use small pinball for other steps. 23 © 2016 ANSYS, Inc. FE model Contact status Deformation July 19, 2017
24.Contact Pinball - Notes 24 © 2016 ANSYS, Inc. Usually, you should not use large PINB to run the analysis. The contact search time will increase. Case 1: User defined pinball region PINB 0.10000E-02 *** NOTE ***One of the contact searching regions contains least 348 target elements. You may reduce the pinball radius. Case 2: Default pinball region factor PINB 1.0000 The resulting pinball region 0.17553E-03 CASE 1 CPU CONTACT SEARCH 2199.251 CONTACT ELEMENTS 399.591 OTHER ELEMENTS 328.731 EQUATION SOLVER 456.250 TOTAL SYSTEM 3383.140 July 19, 2017 CASE 2 57.313 236.996 227.731 416.250 938.290 CONFIDENTIAL
25.InterfaceTreatment:Adjust to touch Initial mesh with undesired gaps and or penetration between contact surfaces results in difficulty in converge gap Mesh discretization can create artificial gaps between surfaces even though the CAD surfaces touch each other Adjust to touch option will remove the gap numerically and assume the surfaces touch each other Physically moving contact nodes towards target surface is not directly exposed in Mechanical, but can be manually defined via CNCH,ADJU/MORPH in a command object. 25 © 2016 ANSYS, Inc. July 19, 2017
26.Mesh Morphing for Contact Adjustment • Mesh morphing (Command:Cnch,morph) adjusts contact surfaces by stress-free movement of mesh • Moves the contact nodes to close gaps and remove penetration (similar to cncheck,adjust) • Morphs the resulting mesh to improve mesh quality 26 © 2016 ANSYS, Inc. July 19, 2017 Cnch, morph creating initial interference
27.Modeling Interference Fit – Three Options Contact surface offset (CNOF) as a function of time via tabular input • Use tabular input to specify a table in which the magnitude of CNOF is ramped down from the possible maximum values of interference to zero over time. • For Arbitrary interface with varying contact normal Automatic interference fit method • The program automatically ramps the initial penetration down to zero over time along the true contact normal direction. • For near flat interface User-defined contact surface normal • The automatically ramps the initial penetration down to zero over time along the user-defined shift direction. • For curve interfaceTip:In some interference fit applications, the reactions calculated via contact element option may differ from those calculated via underlying elements. In such scenarios, the underlying element approach is more accurate. Try tightening the force tolerance (CNVTOL,F command) to improve the contact element reaction calculations. 27 © 2016 ANSYS, Inc. July 19, 2017
28.Contact Pair vs. General Contact • The specific contact pair definition is usually more efficient and robust. It supports more options and special features. Take advantages of WB auto contact detection. • The general contact automatically identifies all possible contacts. However, it is computationally expensive. It is recommended only for cases the pair definition can not identify all possible interactions. – Complex assemblies, Large deformation/motion, Self Contact, Thin geometries CONFIDENTIAL 28 © 2016 ANSYS, Inc. July 19, 2017
33.Contact Stabilization Damping • Stabilization Damping Factor is applied in the contact normal direction and it is valid only for nonlinear contact (frictionless, rough, frictional contacts, and no-separate contact). – If this factor is 0 (default), the damping is activated under certain conditions mentioned and only in the first load step. – If its value is greater than 0, the damping is activated for all load steps. – Additional controls are available via KEYOPT(15) in a command object. – Tangential damping factor is not directly exposed in Mechanical, but can be manually defined via RMODIF in a command object. 33 © 2016 ANSYS, Inc. July 19, 2017
34.…Contact Stabilization DampingExample:Consider a fixed pin interfacing with a hole in plate with initial radial clearance and under a force based load – Stabilization captures localized stress distribution more accurately then ‘Adjust to Touch’ Conventional ‘Adjust to Touch’ Contact Stabilization Damping 34 © 2016 ANSYS, Inc. July 19, 2017
35.Debugstrategies:Overconstraints Overconstrained model • Overconstraints are indicated by the presence of zero pivot warnings. It often results in very large residual force (orders of magnitude larger than a typically applied force) followed by very easy convergence. • First check potential overconstraints via Contact Tool Tips for manually removing overconstraints • Remove overlapped pairs • Merge pairs • Flip contact and target surfaces • Add multiple layers 35 © 2016 ANSYS, Inc. July 19, 2017
36.Debugstrategies:Overconstraints The assembly is connected with MPC contacts 2 elements in sweep direction Contact status In these regions Parts are not correctly connected 36 © 2016 ANSYS, Inc. 36 July 19, 2017 Contact status
37.Solver Settings Decoded F 37 © 2016 ANSYS, Inc. July 19, 2017 1) Weak Springs • Always turn it off, unless it is really needed for prevent rigid body motion. Adding displacement constraints is the right way. • When weak springs are used, carefully verify the reaction forces 2) Large Deflection • Always turn it on, unless the model is truly for small strains, small deformations, small rotations, small sliding. 3) Stabilization • Required for unstable problems • Perform stringent checks on the results when stabilization is used
38.DiagnosticTool:Contact Result Tracker • Provides contact information during solution. • The trends observed can help diagnose problems. • For instance, a decreasing number of contact points indicate a loss of contact 38 © 2016 ANSYS, Inc. July 19, 2017
42.Procedure for Overcoming Convergence Difficulties • Identify the problematic contact region(s)using:–Contact tracking –Contact results (e.g. status, penetration) –Force convergence plots –NR residuals –Outputs • Once identified, possibleremedies:– Check Mesh Quality. – Make sure model units are on an appropriate scale – Adjust the Contact Stiffness – Check for proper initial conditions/pinball. – Change to nodal detection if the problem is at a corner. – Reduce the time step size before and during the onset of the divergence. – If large friction coefficient is defined(>.20) consider using unsymmetric solver – Use small sliding in conjunction with Lagrange multiplier method. – Lastresort:Add stabilization(contact or global) 42 © 2016 ANSYS, Inc. July 19, 2017
43.Debugstrategies:Check non contact-related issues • Unrealistic physical model • Unreasonable loading and boundary conditions. – Insufficient constraints, missing rotation constraints – Overconstraints – Loadingcondition:Step vs. ramped (KBC) • Elementformulation:Hourglass and locking, U/P, joints • Material constitutive Large plastic deformation, creep, incompressible or near incompressible • Unreasonable or incorrect material properties and inconsistent units • Local & global instabilities • Follower loads, Link Elements 43 © 2016 ANSYS, Inc. July 19, 2017
44.Debugstrategies:Other Attempts If above steps still don’t provide enough information on what the problem is, there are other things that can bedone:• Turn on large deflection. • Turn off weak springs. • Use SPARE direct solver instead of PCG iterative solver. • Turn off prediction. • Solve problem using transient option with quasi static option. • Use single process instead of multiple processes. If none of above tricks works, call ANSYS experts for technical supports. 44 © 2016 ANSYS, Inc. July 19, 2017