How to deal with contacts in linear analysis in OptiStruct


Table of Contents

 

Contacts are one of the main non-linearity sources that we have in CAE and play a crucial role in simulating interactions between components, influencing stress distribution, changing loads paths and overall model behaviour. Nevertheless, it can be widely used in linear analysis as well, given that this analysis type consumes less memory and runtime, and it could be enough for most cases. This article will explore defining and managing contacts within linear analysis in Altair OptiStruct.

 

Key Points

Introduction

 

First, it is important to clarify that in Linear analysis (static and dynamic) the contact status and stiffness is constant throughout the solution. In other words, if the contact is initially open, it remains open for the complete duration of the run. The same goes for closed contacts, meaning that no matter if you have tension or compression, there will be load transfer, just as a linear spring connecting your parts.

The contact stiffness (STIFF) depends on the initial state of the contact, and it is calculated based on the gap opening distance (U0), which is calculated based on the positions of the Secondary and Main surfaces. For open contact elements, a very small stiffness value of KB=10E-14 * STIFF is used to avoid numerical singularities.

A diagram of a slope and a lineDescription automatically generated with medium confidence

Types of Contacts in Linear Analysis

 

In Linear analysis, the contact types can assume two main behaviours:

Ensuring Contact Activation

 

For linear analysis, successful contact activation relies on the initial distance between parts. If the parts aren't touching initially, contact won't be established. Here's how to guarantee contact:

A diagram of a diagram of a shell mix planeDescription automatically generated with medium confidence

In the example above, if SRCHDIS is set to 3.0, contact will be generated as expected.

To validate that the contacts are actually closed, you can add CONTPRM,PREPRT,YES entry to your model and this command prints initial contact conditions (except for MPC-based TIE) into an ASCII data file (.cpr file).

A screenshot of a computerDescription automatically generated

For a detailed description of this file content, refer to https://help.altair.com/hwsolvers/os/topics/solvers/os/cpr_file.htm

 

Contact Results Output

 

The CONTF entry can be used to request contact results output for linear static subcases in H3D and OPTI formats. For a detailed description of OPTI file content, refer to https://help.altair.com/hwsolvers/os/topics/solvers/os/cntf_file.htm

Multiple results will be output through CONTF entry, the main ones that will be highlighted in this article are contact forces (total, normal and tangential) and contact status. Contact Status is divided in Open/ClosedSlip/ClosedStick/Frozen status and represented by 0.0 for Open, 1.0 for ClosedSlip (closed SLIDE contact), 2.0 for ClosedStick (closed STICK contact), and 3.0 for Frozen. Below, we can see an example of its representation in HyperView using two different models:

A screenshot of a computer generated imageDescription automatically generated

 

A detailed description of all the outputs provided by CONTF can be found in our documentation: https://help.altair.com/hwsolvers/os/topics/solvers/os/contf_io_r.htm

Evaluating contact forces in dynamic subcases

 

For now, CONTF output is only available for linear static analysis. To evaluate contact forces in linear dynamic subcases, the user can create a cross section through SECTION entry at contact interface and plot the forces at the section. A grid set (GSID) and an Element set (ESID) need to be specified and RESULT option under STYPE selected:

A screenshot of a computerDescription automatically generated

In the example below, if we want to determine the contact force of the green plate on the blue one, GSID should represent the grids of the blue plate on the interface and ESID all elements of the blue plate too:

A screenshot of a computer generated cubeDescription automatically generated

 A blue and yellow gridDescription automatically generatedA screenshot of a computer generated graphDescription automatically generated

 

The cross sections forces and moments results will be output in a .secres file and in the .out file.
A black screen with white textDescription automatically generated with medium confidence

For a detailed description of this file content, refer to https://help.altair.com/hwsolvers/os/topics/solvers/os/secres_file.htm

 

Example Models and Validation

 

In the following link you can find 4 different models to use as a reference: Models

Three of them represent two plates connected by different contact types (FREEZE, SLIDE and PCONT with MU1=0.2) in a free-free modal analysis load case:

modes.gif

Looking at the results for the same mode shape in the modal analysis, we can validate the information under “Types of Contacts in Linear Analysis” topic. For SLIDE contact, both plates are moving freely in the contact plate, making it the less rigid model, while FREEZE and PCONT with MU1=0.2 are completely bonded. We can also observe that the FREEZE contact natural frequency is slightly bigger than PCONT with MU1=0.2, since the tangential stiffness in PCONT with MU1=0.2 is slightly lower.

The fourth model is the model with PCONT with MU1=0.2 and now it covers two linear static load cases, first with a force applied normal to the surface and the second with a force applied in the plane direction.

A computer generated image of a square objectDescription automatically generated

 

In the setup we can see how to define contact force with CONTF output, print initial contact conditions with CONTPRM,PREPRT and define a cross section through SECTION entry.

 

Useful Links

OptiStruct Contacts User Guide

OptiStruct Contact Types

Search Distance (SRCHDIS)

Contact Clearence (CLEARENCE)

How to Choose Main-and-Secondary-Surface in OptiStruct