Setting up contact (SOL 402)

When you set up contact simulation objects for your SOL 402 solution, important considerations include:

• Selecting the source and target regions when you create a contact.

• Modifying contact parameters when your solution won't converge.

Selecting regions

When you select the regions for your contact pairs, a best practice is to select the source and target regions as follows:

• For the source region, select the more flexible region, which is typically the region with the most refined mesh. Selecting the most refined mesh yields the maximum number of contact conditions.

• For the target region, select the most rigid region. Selecting the most rigid surface for the target region is important because the more rigid region undergoes less deformation.

Setting contact parameters to aid convergence

Each contact simulation object can be defined with its own unique set of parameters in the Contact Parameters - Multi-Step Nonlinear Kinematics Pair modeling object. When you create your contact, we recommend that you use the default values for the Contact Parameters - Multi-Step Nonlinear Kinematics Pair modeling object. The default settings are suitable for most cases.

If your solution is not converging, however, modifying the following options may help, depending on your model:

• Normal Regularization Type

• Continuous Segment Normal (SEGNORM)

• Normal Stiffness Model Type

• Regularization Model Type

Normal Regularization Type (for the normal direction)

This option can help the solution converge, and it does not impact the results. The regularization types define the status of the contact (in contact or open) based on a normal distance and a regularization stiffness. By default, the stiffness comes from the mean value of the stiffnesses in the model. But for certain applications that include soft components, you may want to use a value computed per contact (smallest in the contact pairs), or you may want to define it manually.

Normal regularization is very helpful, and is likely required for the solution to converge, when the stiffness of the components that are in contact are very different, such as steel in contact with rubber.

• The Default option for Normal Regularization Type computes the stiffness from the mean value of the stiffnesses in the mode. We recommend that you use the Default value unless you have contact between parts with very different stiffnesses.

• If your model has contact between parts with very different stiffness, try setting Normal Regularization Type to one of the following depending on the relative stiffness of the two parts:Automatic Choice****Automatic Choice chooses between Characteristic Stiffness of the Whole Structure and Computed from Contact Supports depending on the relative stiffnesses of the two parts.Computed from Contact Supports****Computed from Contact Supports computes a value dedicated to the two supports used for the contact condition. If all of the materials are the same, or if the order of magnitude of the stiffness is the same, selecting this option has no visible effect on how the contact is solved.

For information on the other regularization types, see Contact Parameters- Multi-Step Nonlinear Kinematics Pair dialog box.

Continuous Segment Normal (SEGNORM)

If your model has a curved target that is meshed with linear elements, the normal directions are discontinuous between elements. This leads to convergence problems. Use this option to obtain unity in the normal directions at nodes and to define smooth transition between facets of the target.

Normal Stiffness Model Type

Setting the Normal Stiffness Model Type to use contact stiffness can help the solver to converge because it allows the contact to penetrate and then releases the contact constraints. However, do not use contact stiffness if the solution converges without it. Changing Normal Stiffness Model Type has an impact on both convergence and the results.

To use the Normal Stiffness Model Type, try the options in this order:

1. Automatic ChoiceIf Automatic Choice results in penetrations that are too large, look in the .f06 file for the computed contact penetration results.

2. Constant StiffnessWhen you select Constant Stiffness, you can manually enter a stiffness value in the Normal Contact Modulus (NCMOD) box. Enter a value that is higher than the computed penetration value you identified in the .f06 file.

When you use Normal Stiffness Model Type to add stiffness to the contact condition, consider the effects of the following levels of stiffness:

• Low contact stiffness helps with contact convergence, but it can lead to high penetrations between the contact source and target.

• Moderate contact stiffness can help with convergence when convergence issues are related to contact condition.

• High contact stiffness creates a hard contact (no numerical penetration between the source and the target). Typically, a high normal contact stiffness is the same as using Default (no normal stiffness) and thus is not necessary.

Note:

If you use a normal contact stiffness, you must check the contact penetration results and final separation distance. If the penetration is too high, you must increase the normal contact stiffness.

To request the contact penetration results, in the Structural Output Requests dialog box, click the Contact Result page, select the Enable BCRESULTS Request check box, and from the Separation and Slide Distance list, select SEPDIS.

Regularization Model Type (for the tangential direction)

The regularization models ensure a smooth transition of friction stress between sliding and non-sliding regions, which aids in convergence. You can specify whether you want the regularization to be based on sliding velocity or displacement.

For more information on these options, see Contact Parameters- Multi-Step Nonlinear Kinematics Pair dialog box.

Setting up contact (SOL 402), 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 } });