Contact strategies, algorithms, and options (Simcenter Samcef)

Defining the source and target regions

Optimum source and target regions

Choose the Source Region (slave) and Target Region (master) regions based on the region’s mesh refinement level. For the Source Region (slave), we recommend that you choose the most refined region (1), not the contrary (2). Choosing the most refined region as the Source Region (slave) helps the contact algorithm to find a greater number of candidates and ensures better coverage of the contact zone.

Coupled and Uncoupled algorithms

In Simcenter Samcef, two main algorithms drive the contact iterative solve.

• Coupled method.This algorithm is available only for nonlinear analyses.In this algorithm, the contact degrees of freedom are processed with all the other degrees of freedom of the model.Note: We recommend that you use this algorithm in nonlinear analyses.

• Uncoupled method.You can select this algorithm for nonlinear analyses. For linear analyses, this algorithm is always used. In this algorithm, the contact degrees of freedom are processed separately from the other degrees of freedom of the model. The processing cost equals the cubic power of the number of contact degrees of freedom.This algorithm is the slowest of the two options.Note: We do not recommend that you use this algorithm in nonlinear analyses if you define a Bidirectional contact.

Normals smoothing process

During the contact solve, Simcenter Samcef projects each node of the Source Region (Slave) onto the Target Region (Master) to find the contact zones and the target elements/faces candidates.

This projection follows the normals to the candidates.

Smoothed normals

In the case of rough meshes in the contact area, the contact conditions can be affected if you use linear elements (1) instead of parabolic elements (2).

Dark area for contact automatic algorithm

In the example above, at the junction of two facets, a discontinuity in slope occurs. This discontinuity can cause contact convergence problems.

In region 1, there is no problem with detecting the normal to the target facet and then creating the contact element. But, in region 2, due to this discontinuity, the contact can oscillate between two facets.

We recommended that you refine the mesh in the contact area and use parabolic elements.

However, for a rough linear mesh (and even for a parabolic mesh), the Continuous Segment Normal (KSMO) option of the Simcenter Samcef contact parameters can help to fix this dark zone issue.

This option creates smooth transitions between facets and helps to solve the following issue.

Smooth transition

Number of facets in contact

During the contact solve, for each node of the Source Region (slave) region, Simcenter Samcef tries to find the best candidate among the Target Region (master) region list of elements/faces.

The Topology Search (UN2) list of options drives this search:

• If you select Default, the best candidate is evaluated at the beginning of the contact solve and is never updated.This option has the lowest processing cost when solving contact problems and is well suited for small displacements of the model.However, this option is not recommended for models with large displacements. In this case, the contact conditions must be recomputed at each time step or each iteration to ensure a proper convergence.

• If you select Compute At Each Iteration (UN2 3), the best candidate is reevaluated at each contact solve iteration. Although this option has the higher processing cost, it is well suited for models with large displacements.

• If you select Compute At Each Timestep (UN2 2), the best candidate is reevaluated at each time step.

Unidirectional or Bidirectional contact

When your contact's Source Region (Slave) region and Target Region (Master) region are nearly parallel and have a small clearance between them, the Bidirectional contact ensures a better stress-strain computation than the classical Unidirectional contact can offer.

This difference is significant when you model the contact in bolted areas.

You can use this option in both Linear Static and Nonlinear Static analyses. You select the Bidirectional or Unidirectional contact type when you create the contact simulation object.

Contact offset

To consider shell thickness or model an initial gap, you can use the Default Offset Distance for Contact Regions (DMIN) option to specify this offset.

Contact offset

A positive value of this offset reduces the clearance (1).

Note:

If the Target Region (master) is made of shells or membranes, a positive value for the Default Offset Distance for Contact Regions (DMIN) adds an offset according to the shell/membrane normals (2). If the normals are against the contact moment, the offset reduces the clearance. If not, the offset adds an extra clearance.

Regularization for hyperelastic behavior

The regularization parameter used for the contact condition is a characteristic stiffness of the structure. In some cases, especially when the material stiffness of the slave region is very small with respect to the master region, the contact convergence can be difficult to reach.

For these special cases, you can set a Regularization Type in two different ways:

• To let the software automatically compute a characteristic stiffness linked to the elements involved in the contact area, select Normal Regularization Value (PRCS).

• To manually set a specific value for the regularization, select User Defined.

In most models, however, you can safely use the No Regularization default option.

Note:

You can set this regularization parameter in each contact condition you define.

Creating contact and contact parameters

You can define contact source and target regions, the type of contact, and the Contact Parameters modeling object that determines the contact algorithm, smoothing process, contact offset, and so on, from the dialog box that opens when you create a contact simulation object. You can also create the Contact Parameters modeling object separately and then select the appropriate modeling object when you create the contact.

Where do I find it?

Creating Contact Parameters modeling object

Application	Pre/Post
Prerequisites	A Simulation or FEM file as the work part and displayed partSimcenter Samcef as the specified solverStructural as the specified analysis typeLinear Static Analysis or Nonlinear Analysis as the specified solution type
Command Finder	Modeling Objects
Location in dialog box	Modeling Objects Manager dialog box→Type list→Contact Parameters→Create

Creating contact simulation objects

Application	Pre/Post
Prerequisites	A Simulation file as the work part and displayed partSimcenter Samcef as the specified solverStructural as the specified analysis typeLinear Static Analysis or Nonlinear Analysis as the specified solution type
Command Finder	Surface-to-Surface Contact Edge-To-Surface Contact Nodes-To-Surface Contact Nodes-to-Edge Contact Beam to Beam Contact

How do I

Define a surface for the Rigid-Flexible Simcenter Samcef contact

Learn more

Rigid Analytical Surface Contact (Simcenter Samcef)

Surface-To-Surface Contact (Simcenter Samcef)

Nodes-To-Surface Gluing (Simcenter Samcef)

Solid-To-Edge Gluing (Simcenter Samcef)

Edge-To-Edge Gluing (Simcenter Samcef)

Surface-To-Surface Gluing (Simcenter Samcef)

Edge-To-Surface Contact (Simcenter Samcef)

Edge-To-Surface Gluing (Simcenter Samcef)

Previewing contact and glue element locations (Simcenter Samcef)

Contact and glue specific results (Simcenter Samcef)

Nodes-To-Surface Contact (Simcenter Samcef)

Nodes-to-Edge Contact (Simcenter Samcef)

Nodes-to-Edge Gluing (Simcenter Samcef)

Edge-to-Edge Contact (Simcenter Samcef)

Display of the analytical surface of a Rigid Analytical Simcenter Samcef contact in post-processing

Rigid or flexible surface in classical Simcenter Samcef contacts

Beam to Beam Contact (Simcenter Samcef)

Automatic face pairing

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Contact strategies, algorithms, and options (Simcenter Samcef), Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });