ANSYS LS-DYNA in Mechanical APDL

Transcription

1 Lecture 6 Contact Surfaces 14.5 Release ANSYS LS-DYNA in Mechanical APDL 2012 ANSYS, Inc. February 5, Release 14.5

2 Objectives This lecture covers contact surfaces. The different algorithms are presented, along with recommendations on their use. Topics: A. Overview of Contact Surfaces B. Single Surface Contact Algorithm C. Nodes-to-Surface Contact Algorithm D. Surface-to-Surface Contact Algorithm E. General (Basic) Contact Family F. Automatic Contact Family G. Rigid Contact Family H. Tied Contact Family I. Tiebreak Contact Family 2012 ANSYS, Inc. February 5, Release 14.5

3 Objectives Topics (continued): J. Eroding Contact Family K. Edge Contact Family L. Drawbead Contact Family M. Forming Contact Family N. 2-D Contact Family O. Defining Basic Contact P. Listing and Plotting Contact Q. Deleting/Deactivating/Reactivating Contact R. Advanced Contact Controls S. General Contact Guidelines T. Contact Surfaces Workshop 2012 ANSYS, Inc. February 5, Release 14.5

4 A. Overview of Contact Surfaces There are many ways to define contact in ANSYS LS-DYNA. The differences include how the contact surfaces are represented, how the contact penetration is interpreted, and what advance features and limitations exist in the different algorithms. For some contact models, segments are used to define the surfaces of the contacting bodies. This is analogous to the new surface-to-surface algorithms in implicit ANSYS, but the user does not need to define these segments himself. ANSYS LS-DYNA will create the segments automatically from specified nodal components, etc. Other contact models allow for any surface of the model to come into contact with any other surface, including the same surface. This completely arbitrary contact is actually the easiest to define, and is very useful when the contacting surfaces are not known ahead of time, such as in entire car crash simulations ANSYS, Inc. February 5, Release 14.5

5 ... Overview of Contact Surfaces Generally, when a contact (slave) node or segment penetrates a target (master) segment, a restoring (penalty) force pushes it back across the boundary. The contact penalty stiffness is automatically calculated by LS-DYNA based on the moduli of the contacting bodies. This is why it is very important to use a realistic Young s modulus when defining rigid bodies (materials). ANSYS LS-DYNA allows for the simulation of a wide range of contact conditions: Surface finish can be accounted for by specifying velocity dependent friction along with a shear stress at failure. Eroding contact allows for the contact surface to be established on interior elements, as those on the exterior surface fail. Edge contact permits the edge of one shell element to detect the edge of another shell - a feature not associated with surface-to-surface contact ANSYS, Inc. February 5, Release 14.5

6 ... Overview of Contact Surfaces To define contact in ANSYS LS-DYNA, simply indicate the contact surfaces (not always required), the type of contact between them, and any specific parameters related to a given contact type. With so many different contact types available, it is often difficult to determine which contact type best defines the physical system being modeled. To properly select a contact surface for a given model, it is important to understand the different contact algorithms and contact families available within ANSYS LS-DYNA. A contact algorithm is a method by which the code processes contact surfaces. There are three different contact algorithms available: Single Surface Contact Nodes-to-Surface Contact Surface-to-Surface Contact 2012 ANSYS, Inc. February 5, Release 14.5

7 Overview of Contact Surfaces A contact family is a set of contact types that have similar specialized properties. There are ten different contact families available: General (Basic) Contact Automatic Contact Rigid Contact Tied Contact Tied with Failure Contact Eroding Contact Edge Contact Drawbead Contact Forming Contact Two-Dimensional Contact ANSYS LS-DYNA supports 24 combinations of these contact algorithms and contact families, but there is some overlap ANSYS, Inc. February 5, Release 14.5

8 Overview of Contact Surfaces Single Surface Nodes to Surface Surface to Surface General (Basic) SS NTS STS, OSTS Automatic ASSC, AG ANTS ASTS Rigid RNTR ROTR Tied TDNS TDSS, TSES Tied with Failure TNTS TSTS Eroding ESS ENTS ESTS Edge SE Drawbead DRAWBEAD Forming FNTS FSTS, FOSS Two-Dimenional ASS2D Each of the contact algorithms and contact families will be described in detail so that the most appropriate contact model may be chosen to accurately represent the physical phenomenon being simulated ANSYS, Inc. February 5, Release 14.5

9 B. Single Surface Contact Algorithm The single surface contact algorithm establishes contact when an external surface of one body contacts itself or the external surface of another body. Single surface contact is the most general type of contact because the ANSYS LS-DYNA program automatically searches all of the external surfaces within a model to determine if penetration has occurred. Since all of the external surfaces are included, no contact or target surface definitions are required. Single surface contact can be very powerful for self-contact or large deformation problems where areas of contact are not known beforehand ANSYS, Inc. February 5, Release 14.5

10 ... Single Surface Contact Algorithm Single surface contact in ANSYS LS-DYNA will cause only minor CPU time increases over limiting the contact surfaces. Most impact and crash applications require single surface contact to be defined, since all of the contact surfaces are not known beforehand. In most cases, the single surface contact algorithm automatically releases the contact if a node penetrates more than 40 % of the thickness of the contacted element. This can cause potential problems for the following conditions: Excessively thin parts Soft materials that have low stiffness values Contact between bodies with extremely high velocities 2012 ANSYS, Inc. February 5, Release 14.5

11 ... Single Surface Contact Algorithm These conditions can result in contact nodes exceeding the 40% depth condition. The contact algorithm will then assume that the surfaces are not in contact, and material pass-through will occur. Contact nodes can then get trapped behind a target surface. The single surface contact algorithm does not record the overall resultant contact forces in the ASCII rcforc file. If contact forces are desired, node-to-surface or surface-to-surface algorithms should be used. Alternatively, *CONTACT_FORCE_TRANSDUCER_PENALTY commands may be added to the.k file to be able to get this rcforc output. However, this latter practice is not supported by ANSYS. The single surface contact algorithm includes the following contact models: Single Surface (SS), Automatic Single Surface (ASSC), Automatic General (AG), Eroding Single Surface (ESS), Single Edge (SE), and 2-D Automatic Single Surface (ASS2D) 2012 ANSYS, Inc. February 5, Release 14.5

12 C. Nodes-to-Surface Contact Algorithm The nodes-to-surface contact algorithm establishes contact when a contacting node penetrates a target surface. It is the fastest algorithm because it is asymmetric. Only the treatment of contact nodes impacting the target surface is considered. For node-to-surface contact, nodal components or Part numbers (or Part assemblies) for the contact and target surfaces must be specified, similar to the ANSYS implicit method. Node-to-surface contact is very robust for problems where the contact area is relatively small and the contact area is known beforehand. It is also efficient for modeling nodes contacting rigid bodies ANSYS, Inc. February 5, Release 14.5

13 ... Nodes-to-Surface Contact Algorithm The following guidelines should be used with nodes-to-surface contact: 1. Flat or convex surfaces should be targets and concave surfaces should be contacts. CONTACT NODES 2. Coarser meshes should be targets and finer meshes should be contact surfaces. TARGET SURFACE 3. For Drawbead contact, the bead is always the nodal contact surface and the blank is the target. The nodes-to-surface contact algorithm records the overall resultant contact forces in the ASCII rcforc file. The nodes-to-surface contact algorithm includes the following contact models: NTS, ANTS, RNTR, TDNS, TNTS, ENTS, DRAWBEAD, FNTS 2012 ANSYS, Inc. February 5, Release 14.5

14 D. Surface-to-Surface Contact Algorithm The surface-to-surface contact algorithm establishes contact when the surface of one body penetrates the surface of another. Surface-to-surface contact is fully symmetric so that the choice of contact and target surfaces is arbitrary. For surface-to-surface contact, nodal components or Part numbers (or Part assemblies) are required for the contact & target surfaces. Nodes may belong to multiple contact surfaces. Surface-to-surface contact is a general algorithm and is commonly used for bodies that have large contact areas and the contact surfaces are known beforehand ANSYS, Inc. February 5, Release 14.5

15 ... Surface-to-Surface Contact Algorithm CONTACT AND TARGET DEFINITIONS ARBITRARY V Surface-to-surface contact is most efficient for bodies that experience large amounts of relative sliding, such as a block sliding on a plane. The surface-to-surface contact algorithm records the overall resultant contact forces in the ASCII rcforc file. The surface-to-surface contact algorithm includes the following contact models: STS, OSTS, ASTS, ROTR, TDSS, TSES, TSTS, ESTS, FSTS, FOSS 2012 ANSYS, Inc. February 5, Release 14.5

16 E. General (Basic) Contact Family General (basic, original, old, etc.) contact considers contact on only one side of shell elements (except for SS). For solid (brick) elements, ANSYS LS-DYNA always creates the target segments with outward normals, so the desired contact will always be recognized. The restoring force (i.e., the penalty force resisting nodal penetration) will continue to increase as the contact node penetrates the target surface. By default (except for SS), this force will not be eliminated after the node passes a set percentage of the element thickness: TOP surface Restoring forces are perpendicular to surface BOTTOM surface penetrating node Contact Restoring Force General Contact models include: SS NTS STS OSTS General Contact 2012 ANSYS, Inc. February 5, Release 14.5

17 F. Automatic Contact Family Automatic contact considers contact on both sides of shell elements. The contact surface orientation for shells is automatically determined. The restoring force will continue to increase as the contact node penetrates the target surface, but only up until a point 1, because the contact needs to be detected on either side of the shell element: penetrating node Shell TOP surface Contact Restoring Force Shell BOTTOM surface Automatic Contact models include: ASSC AG (includes SE) ASS2D ANTS ASTS Automatic Contact Restoring forces perpendicular to surface 1 This point is much greater for AG contact than for the others 2012 ANSYS, Inc. February 5, Release 14.5

18 G. Rigid Contact Family Rigid contacts RNTR and ROTR are similar to NTS and OSTS except that instead of a linear stiffness to resist penetration, the user defines a force-deflection curve. These contacts are normally used for multi-body dynamics. They are intended to allow inclusion of energy absorbing compliance without the modeling deformable elements. A contact of a rigid body to a deformable body must be defined with the normal, automatic or eroding contacts. Contact of the knees against the dashboard Rigid contact types are not that common, since the penalty-based contacts used for deformable bodies can also be used for rigid bodies and are generally better ANSYS, Inc. February 5, Release 14.5

19 H. Tied Contact Family Tied contact is used to connect dissimilar meshes together in much the same way as bonded contact is used in implicit ANSYS. The contact nodes are glued to the target surfaces. Both surfaces must be initially coplanar. Nodes close to being coplanar will be moved to become coplanar. The target surfaces can deform, forcing the contact nodes to follow that deformation. Tied contact models include TDNS, TDSS, and TSES contact. Since a constraint-based formulation is used, tied contact cannot include rigid bodies. (However, an unsupported penalty-based tied contact formulation using offsets does allow the inclusion of rigid bodies). Only translational DOF s (UX, UY, UZ) are affected by tied contact types TDNS and TDSS, so generally only solid (brick) elements are used for them. Incidentally, tied contact is best defined with nodal components instead of Part ID s ANSYS, Inc. February 5, Release 14.5

20 I. Tiebreak Contact Family Tiebreak contact is essentially tied contact with failure. It is often used to simulate spot-welded or bolted connections. Once the failure equation is met, the contact nodes can slide or separate from the target surface. The formulation is penalty-based. The TNTS failure equation is based on normal and shear force, whereas the TSTS failure equation is based on normal and shear stress. fn f m 1 f m 2 n + s f f n, fail s, fail 1 tied Failed (connection released) fs 2012 ANSYS, Inc. February 5, Release 14.5

21 J. Eroding Contact Family These contact models (ESS, ENTS, ESTS) are used when solid elements on the outer surface fail (e.g., due to exceeding an allowable strain), thereby requiring that the interior solid elements assume the duties of resisting the penetration. This algorithm usually requires part numbers as opposed to nodal components. Eroding contact is used with material models that support failure. The unsupported *MAT_ADD_EROSION capability can be used with materials that do not normally support failure ANSYS, Inc. February 5, Release 14.5

22 K. Edge Contact Family Edge contact is needed when the shell surface normals are orthogonal to the impact direction. Shell edge (SE) contact selects all shell edges automatically. A subset may be used by specifying a contact (slave) component. SE contact is also included in automatic general (AG) contact ANSYS, Inc. February 5, Release 14.5

23 L. Drawbead Contact Family Drawbead contact is typically used in metal forming operations when special care is need to restrain the blank. For example, in stamping processes, it is common for the blank to lose contact with the forming dies, causing wrinkling in the blank. Drawbead contact simulates the presence of these actual drawbeads by including bending and frictional restraining forces, which ensure that the blank will remain in contact through the entire length of the drawbead depth. Depth of drawbead F = Ffriction+ Fbending 2012 ANSYS, Inc. February 5, Release 14.5

24 M. Forming Contact Family The forming contact options forming node-to-surface (FNTS), forming surface-tosurface (FSTS) and forming one-way surface-to-surface (FOSS) are primarily used in metal forming applications. FOSS contact is generally recommended, since penetration of the target (master) nodes through the contact (slave) surface is considered in adaptive meshing, minimizing tooling penetration. For these contact types, the tools and dies are typically defined as the target surface while the workpiece is the contact surface. Mesh connectivity is not required, but the orientation of the tooling meshes must be in the same direction. Reorientation of these disconnected target surfaces is done automatically, as needed. Since the forming contact options are based on automatic contact types, they are very robust ANSYS, Inc. February 5, Release 14.5

25 N. 2-D Contact Family For models made up of PLANE162 elements, only two-dimensional contact can be defined. The 2D contact option that is supported in ANSYS LS-DYNA is ASS2D. The default contact surface is the entire model (i.e., the target surface is not used). The contact surface can be limited to a part assembly (EDASMP). Static and dynamic friction coefficients, an exponential decay coefficient, and birth and death times are all supported with 2D contact ANSYS, Inc. February 5, Release 14.5

26 O. Defining Basic Contact The three basic steps in defining contact within ANSYS LS-DYNA are: 1. Select the contact model that best simulates your physical system 2. Identify the contact entities (Not required for single surface contact) 3. Define the contact and any additional input parameters required Select the Contact Model : To select the contact model that is best suited for a given application, consult the ANSYS LS-DYNA User s Guide and review the descriptions found in this lecture. For most analyses, the automatic single surface (ASSC), automatic general (AG), nodes-to-surface (NTS), and surface-to-surface (STS) contact models are recommended. They are very robust and cover most applications ANSYS, Inc. February 5, Release 14.5

27 ... Defining Basic Contact Identify the Contact Entities : With the exception of the single surface contact models (SS, ASSC, AG, ESS, SE, and ASS2D), all of the ANSYS LS-DYNA contact models require the definition of a contact surface and a target surface. Although not required, the single surface contact models can restrict the contact to a portion of the model by specifying a contact surface. By default, this algorithm considers the entire model for possible contact. Contact and target surfaces can be represented by either nodal components (CM command) or Part numbers/part assemblies (EDPART and EDASMP commands). As discussed in Lecture 3, the Part list can change if it is recreated after additional modeling is done, so it is normally best to just update the Part list after making any changes. Otherwise, a contact definition defined to an old Part number will give undesired results. The best practice is to do all of your ANSYS geometry modeling before issuing any ANSYS LS-DYNA specific commands ANSYS, Inc. February 5, Release 14.5

28 ... Defining Basic Contact If Part numbers (or Part assemblies) are used to identify the contact and target surfaces, the area of contact can be further restricted by using box ID s. Box ID s are defined with the EDBOX command: Preprocessor > LS-DYNA Options > Contact > Define Box These box-shaped volumes cannot be used with nodal components. Restricting the amount of contact processing is more important in very large models, but it may even be of use in small models where including the entire model causes the contact to misbehave ANSYS, Inc. February 5, Release 14.5

29 ... Defining Basic Contact Define the Contact : The EDCGEN command automatically creates contact between the specified contact and target surfaces: Preprocessor > LS-DYNA Options > Contact > Define Contact First pick the desired contact algorithm and corresponding model: Contact algorithms Contact models 2012 ANSYS, Inc. February 5, Release 14.5

30 ... Defining Basic Contact Next, specify the static and dynamic coefficients of friction along with the coefficients for exponential decay, viscous friction, and viscous damping. In ANSYS LS-DYNA, the friction coefficient can be dependent on the velocity and a limiting value can be used for the overall frictional force. Model frictionless contact by leaving all of these fields blank ANSYS, Inc. February 5, Release 14.5

31 ... Defining Basic Contact The friction coefficient, m c, is defined by: m c = m d + (m s - m d )e -(DC) (v) where m s = Static friction coefficient m d = Dynamic friction coefficient DC = Exponential decay coefficient v = Relative velocity between contacting surfaces With DC or v = 0, m c is equal to the m s The maximum friction force, F lim, can also be limited by the product of the coefficient for viscous friction, VC, and the area of the contact segment, A segment : F lim = VC A segment The limiting friction coefficient is often used in applications where the contact causes plastic flow. The recommended value of VC = s o, where s o is the yield stress of the contacted material ANSYS, Inc. February 5, Release 14.5

32 ... Defining Basic Contact In order to avoid undesirable oscillations during contact, a contact damping perpendicular to the contact surface can be applied using the viscous damping coefficient, VDC. The input, VDC, requires a damping value as a percentage of critical: x = (VDC/100.0) x crit = (VDC/100.0) (2m w) where m = mass w = natural frequency of the contact segment Viscous damping is commonly used to damp out high frequency oscillation in metal forming analyses ANSYS, Inc. February 5, Release 14.5

33 ... Defining Basic Contact After the friction data, specify birth and death times for the contact: Facilitates multi-stage forming by allowing tooling used in latter stages of the forming to already be in position without interfering with the blank. The default is to have the contact active for the entire duration of the run. Next specify Box ID s used to further restrict contact or target surface definitions, assuming Part numbers or Part assemblies are used. Due to limitations in the current UIDL, the GUI cannot filter out whether Box ID s are valid until after the entire EDCGEN command is issued. Therefore, only specify Box ID s if they have already been defined (EDBOX) and Part ID s or assemblies are being used ANSYS, Inc. February 5, Release 14.5

34 ... Defining Basic Contact After clicking OK on the first EDCGEN dialogue box, a second box appears so that the contact and target surfaces can be identified. For the single surface contact models, this second box does not typically appear, since contact and target surfaces are not required. The EDCGEN command must be typed in directly (i.e., batch mode) to access this feature of further restricting the contact surface for single surface contact models. Some contact models require additional input parameters. For these models, a model-specific dialogue box will appear instead 2012 ANSYS, Inc. February 5, Release 14.5

35 ... Defining Basic Contact Four contact families require additional input (EDCGEN fields V1-V4): Family V1 V2 V3 V4 Eroding Symmetry option key Internal erosion key Adjacent material key N/A Rigid LCID Force calc. Method Unloading stiffness N/A Tiebreak Tensile failure force Shear failure force Normal force exp. Shear force exponent Drawbead LCID1 LCID2 Drawbead depth # of Integration Points The contact model-specific input further defines the contact. In the Tiebreak Nodes-to-Surface contact (TNTS) shown to the left, the user is prompted for the failure information that defines when the two surfaces unglue ANSYS, Inc. February 5, Release 14.5

36 P. Listing and Plotting Contact Because contact elements are not created, it is very important to list the defined contact surfaces before solution to ensure that the contact has been properly defined. This is done with the EDCLIST command: Preprocessor > LS-DYNA Options > Contact > List Entities All defined contact entities are automatically listed along with the specified friction parameters. Note that each contact definition has a specific reference number ANSYS, Inc. February 5, Release 14.5

37 ... Listing and Plotting Contact Using the contact definition (reference) number from the EDCLIST output, you can plot the contact pairs with the EDPC command: Preprocessor > LS-DYNA Options > Contact > Select and Plot... Contact #1 Contact #2 Contact #3 EDPC both selects and plots the contact pair. Do not forget to reselect the nodes and elements desired before solution 2012 ANSYS, Inc. February 5, Release 14.5

38 Q. Deleting/Deactivating/Reactivating Contact Delete incorrectly defined contact entities with the EDDC command: Preprocessor > LS-DYNA Options > Contact > Delete Entity Contact entities may only be deleted in a new analysis. EDDC, DELE needs: Contact model Contact Part or component Target Part or component The GUI automatically specifies the DELE option for the EDDC command, but you still must specify the contact and target components and/or Part ID s/assemblies. The single surface contact routines will generally not require these surfaces. To delete all of the contact in the model, issue EDDC, DELE, ALL 2012 ANSYS, Inc. February 5, Release 14.5

39 ... Deleting/Deactivating/Reactivating Contact During a small restart analysis, it is also possible to deactivate (EDDC, DACT) and reactivate (EDDC, RACT) a defined contact entity: Preprocessor > LS-DYNA Options > Contact > Deactivate Entity Preprocessor > LS-DYNA Options > Contact > Activate Entity Deactivation and reactivation of contact may be useful in a multi-stage forming simulation. The EDDC command is not supported in a full restart analysis ANSYS, Inc. February 5, Release 14.5

40 R. Advanced Contact Controls ANSYS LS-DYNA has several advanced options for controlling contact. Most of these controls are available on the EDCONTACT command and are global in nature (i.e., pertaining to all defined contact entities): Preprocessor > LS-DYNA Options > Contact > Advanced Control The advanced controls that are local in nature (i.e., for a specific contact entity) are defined with either the EDSP command or the EDCMORE command: Preprocessor > LS-DYNA Options > Contact > Advanced Control Preprocessor > LS-DYNA Options > Contact > Additional Parms The following global options are commonly used to control contact: Controlling the contact search method Controlling the contact depth Controlling the contact stiffness 2012 ANSYS, Inc. February 5, Release 14.5

41 ... Advanced Contact Controls Controlling the Contact Search Method : In ANSYS LS-DYNA, there are two different contact search methods: Mesh Connectivity Tracking Bucket Sort Method (both nodal-based and the newer segment-based) In mesh connectivity tracking, the contact search algorithm uses shared nodes of neighboring element segments to search for contact. When a target segment loses contact with a contact node, the neighboring segment is checked. The mesh connectivity method is extremely fast, but can be disadvantageous since it requires that the contact surfaces have a continuous mesh. Historically, the mesh connectivity method was used as the default for contact models STS, NTS, OSTS, TSTS, TNTS, and TDNS, but advances in the newer bucket sort algorithm permit its use in these models as well. The bucket sort approach is activated whenever thickness offsets are considered ANSYS, Inc. February 5, Release 14.5

42 ... Advanced Contact Controls In the bucket sort method, the 3-D space occupied by the contact surface is divided into cubes ( buckets ). Nodes can contact any segment in the same bucket or in a next-door bucket. The bucket sort algorithm is extremely robust, but can be somewhat slower than mesh connectivity tracking, especially for large models. The bucket sort method is the default for contact models ASTS, ANTS, ESTS, ENTS, and all of the single surface contact models Since many models contain discontinuous meshes, it is often beneficial to switch the search algorithm to the bucket sort method via the multi-surface shell thickness (SHTK) field of the EDCONTACT command: Setting the EDCONTACT SHTK field to Thk Incl-Exc Rgd (use shell thickness except for rigid bodies) or Thk Incl (use shell thickness, including rigid bodies) will cause contact models like NTS to use the bucket sort algorithm ANSYS, Inc. February 5, Release 14.5

43 ... Advanced Contact Controls Controlling the Contact Depth : For the general contact options STS, NTS, TNTS, TSTS, and OSTS, a contact search depth of 1e10 is assumed by ANSYS LS-DYNA (if thickness is not considered). When a contacting node passes behind a target surface, a contact (restoring) force proportional to the contact depth will be generated. This can cause instabilities in dynamic models where components are in continuous relative motion and non-genuine contact is generated. If the contact depth is large, the spurious contact forces could become nearly infinite. If a node appears (slips) behind a target surface, it can shoot off into space. To control the depth for which contact is considered, set the PENCHK field of the EDCONTACT command to one of the ON settings. Please refer to the Commands Reference for a complete description ANSYS, Inc. February 5, Release 14.5

44 ... Advanced Contact Controls By setting PENCHK to ON, the program will only search for contact up to a depth proportional to the target segment thickness. Another ON option, which considers the smallest diagonal, is also available. This small penetration check is applied to all applicable contact entities in the model, since the EDCONTACT command is used to set global contact controls. If you desire to use this feature on a local basis (i.e., on a particular contact entity), you will need to use the EDSP command instead. The EDSP command is discussed later 2012 ANSYS, Inc. February 5, Release 14.5

45 ... Advanced Contact Controls Controlling the Contact Stiffness : In the ANSYS LS-DYNA program, the penalty method is used for the calculation of the contact forces. In the penalty method, an elastic spring is placed between the two bodies such that the contact interface force, F, is given by: F where F = k d k = contact interface stiffness d = penetration between bodies d k 2012 ANSYS, Inc. February 5, Release 14.5

46 ... Advanced Contact Controls Ideally, there should be no penetration between surfaces during contact. This implies that the contact interface stiffness is equal to infinity (k = ), which will lead to numerical instabilities. The ANSYS LS-DYNA program automatically calculates the contact stiffness based on the material properties and size of the contacting segments. This value will generally provide excellent results. However, always check the d3hsp file to make sure that the solution time step is smaller than the time step required for contact stability: The minimum time step of e-6 seconds based on the material properties and element sizes is less than that needed for stable contact (0.185e-5), so this model should be OK, as is 2012 ANSYS, Inc. February 5, Release 14.5

47 ... Advanced Contact Controls The contact stiffness can be changed by using a global contact stiffness scale factor, SFSI, that adjusts the ANSYS LS-DYNA calculated stiffness (kcalc) by the following relationship: k = SFSI kcalc The default SFSI in ANSYS LS-DYNA is To increase the contact stiffness, increase the SFSI field on the EDCONTACT command. SFSI is often increased in eroding contact analyses. However, increasing the contact stiffness increases the risk of convergence instabilities. Try to never increase the SFSI parameter over ANSYS, Inc. February 5, Release 14.5

48 ... Advanced Contact Controls When determining a default contact stiffness, the ANSYS LS-DYNA program uses the material properties and the element sizes of the contact and target surfaces. If the contacting surfaces of a model have large differences in material properties (e.g., steel impacting foam) or element sizes, instabilities or unrealistic behavior may arise. When problems occur due to an incompatible contact stiffness, the contact stiffness of the contact and target surfaces can be scaled to closer values by ANSYS LS-DYNA. The message shown in the d3hsp file a few slides back roughly stated: If the actual solution time step value to be used is greater than that calculated for contact stability, then scale the penalty stiffness of the offending surface ANSYS, Inc. February 5, Release 14.5

49 ... Advanced Contact Controls The PENO field of the EDCONTACT command is used to scale the contact stiffness: There are five main options available for controlling the contact stiffness due to incompatibility: Use the minimum of the contact and target stiffness Use target (master) surface value Use contact (slave) surface value Use area or mass weighted contact value Use contact value inversely proportional to shell thickness (generally not recommended) 2012 ANSYS, Inc. February 5, Release 14.5

50 ... Advanced Contact Controls As mentioned at the beginning of this section, the EDCONTACT command is used to set advanced global contact controls. If local contact controls are needed, then the commands EDSP and EDCMORE should be used: Preprocessor > LS-DYNA Options > Contact > Advanced Control Preprocessor > LS-DYNA Options > Contact > Additional Parms The EDSP command is applicable to STS, NTS, OSTS, TNTS, and TSTS contact. It turns the small penetration check on and off, just like the EDCONTACT command does, but only for a specific contact entity ANSYS, Inc. February 5, Release 14.5

51 ... Advanced Contact Controls Likewise, the EDCMORE command specifies the penalty scale factors, SFS and SFM, for the contact (slave) and target (master) surfaces, respectively, of a specific contact entity. These parameters are needed when the contact stiffness is very different between the two surfaces. The EDCMORE parameters are also controlled by the EDDC command. Additional local contact controls will be added to the EDCMORE command in the future ANSYS, Inc. February 5, Release 14.5

52 S. General Contact Guidelines Although LSTC has initial interference capability in LS-DYNA, it is not supported in ANSYS LS-DYNA. This is because press fit problems are normally static analyses something that is not handled well by an explicit code. Therefore, if there are any initial nodal penetrations in your model, LS-DYNA will move the overlapping surfaces out of contact before proceeding. Always use realistic material property and shell thickness values. The material properties and geometry of contacting surfaces are used to determine the contact penalty stiffness. Do not make multiple contact definitions between the same parts. Use single surface contact if the exact contact behavior is not known beforehand (e.g., use ASSC or AG contact in a car crash analysis). AG includes ASSC, SE, and beam-to-beam contact ANSYS, Inc. February 5, Release 14.5

53 ... General Contact Guidelines List and plot the defined contact surfaces prior to solution to ensure that contact has been properly defined. If an analysis begins to diverge soon after starting, the following ASCII output files should be examined. Extremely large energies in these files will isolate the material in the contact definition that is causing problems: GLSTAT: overall energy distribution MATSUM: energies by Part ID SLEOUT: sliding interface energy on a contact entity basis RCFORC: resultant contact forces for the contacts and targets Always first use a small test model to verify your contact definitions instead of trying to debug a large model. What often appears to be a contact problem may actually be a units problem, an incorrect load, or a material definition error ANSYS, Inc. February 5, Release 14.5

54 T. Contact Surfaces Workshop This workshop consists of the following problem: WS06. Aluminum Rod Impact Analysis Please refer to your Workshop Supplement for instructions ANSYS, Inc. February 5, Release 14.5