Home
Aerospace
Essential utility tools developed using HyperMesh-Tcl.
Connection Tools
Create Linear Gaps
Use the Linear Gap tool to create linear gap analysis cards for Nastran and OptiStruct.
Linear Gap
Linear gap is the simplest contact form used in Nastran simulations.

Welcome
What's New
View new features for Altair HyperWorks 2024.
Get Started
Learn the basics and discover the workspace.
Tutorials
Learn more about the Altair HyperWorks suite of products with interactive tutorials.
Startup Procedures and Customizations
Start and configure the applications.
Tool Finder
View a list of deprecated panels and their newer, equivalent workflows.
Manage Files and Data
Create, open, import, and save models.
Sessions and Report Templates
Set up sessions and create report templates.
Interface with External Products
Solver interfaces supported in HyperMesh.
Entities and Solver Interfaces
A solver interface is made up of a template and a FE-input reader.
Browsers
Browsers provide a structured view of model data, which you can use to review, modify, create, and manage the contents of a model. In addition to visualization, browsers offer features like search, filtering, and sorting, which enhance your ability to navigate and interact with the model data.
Sketching
Create and edit 2D parametric sketch geometry.
Topology
Create, edit, and cleanup geometry.
FE Geometry
FE geometry is topology on top of mesh, meaning CAD and mesh exist as a single entity. The purpose of FE geometry is to add vertices, edges, surfaces, and solids on FE models which have no CAD geometry.
Meshing and Elements
Explore the different types of mesh you can create in HyperMesh and create and edit 0D, 1D, 2D, and 3D elements.
Model Build and Assembly
Create, organize and manage parts and subsystems.
Composites
HyperMesh composites modeling.
Connectors
Create connections between parts of your model.
Morph
Rapidly change the shape of the FE mesh without severely sacrificing the mesh quality.
Skeleton Modeling
Create a reduced ordered model to facilitate optimization at the concept phase.
Design Space
Workflow to support topology optimization model build and setup.
Optimization
Setup an Optimization in HyperMesh.
Design Explorer
Multi-disciplinary design exploration and optimization tools.
Validate
Validate the model built before running solver analysis.
Analyze
Models require loads and boundary conditions in order to represent the various physics and/or physical equivalents to bench and in-use testing.
Axisymmetry
Reduce a full 3D model with axisymmetric surfaces while accounting for imperfections.
Concept Modeling
Tools and workflows that are dedicated to rapidly creating new parts for specific use cases, or amending existing parts. The current capabilities are focused on stiffening parts.
Crash and Safety
Tools used for crash and safety analysis.
Airbag
Use airbag folder utilities and export a resulting airbag in a Radioss deck.
Aerospace
Essential utility tools developed using HyperMesh-Tcl.
- Assembly Tools
  Create an assembly structure from a .csv file definition.
- Load/BCs Tools
- Connection Tools
  - Fastener Setup
    Create node-to-node CBUSH elements at the connector locations point/node or line.
  - Convert CFAST Elements
    Use the cfast converter tool to convert CFAST elements into CBAR/RBE3 (spiders). For thermoelastic analysis, the CFAST has no thermal expansion coefficient. CBAR is thermoelastic compatible.
  - Stuck Node Creation
    Use the Stuck Node Creation tool to create (double) RBE3 connection to "stick" nodes on QUAD or TRIA elements to make the node displacements following the element ones.
  - Create Linear Gaps
    Use the Linear Gap tool to create linear gap analysis cards for Nastran and OptiStruct.
    - Linear Gap
      Linear gap is the simplest contact form used in Nastran simulations.
  - Sewing Tools
    Connect two dissimilar 2D shell meshes using RBE3 connection.
  - Create 0D Elements Between Disconnected Nodes
    In the steps below, you will create zero length elements and review.
  - Create 0D Elements Between Connected Nodes
- Spatial ID Manager Tools
- Display Tools
- Export Tools
- Set Tools
- System Tools
- Node Tools
Aeroelasticity
Import an aeroelastic finite element model with Nastran Bulk Data format.
Certification
Framework to plug certification methods to assess margin of safety from the model and result information.
PhysicsAI
Use PhysicsAI to build fast predictive models from CAE data. PhysicsAI can be trained on data with any physics or remeshing and without design variables.
Results Data
Results data can be post-processed using both HyperMesh and HyperView.
Developer
The Developer ribbon contains tools for automation and customization.
Plot Data
HyperGraph is a data analysis and plotting tool with interfaces to many file formats.
Multibody Modeling
MotionView is a general pre-processor for Multibody Dynamics.
Media Files
MediaView plays video files, displays static images, tracks objects, and measures distances.
Tabulate Results
Use TableView to create an Excel-like spreadsheet.
Text Files
TextView math scripts reference vector data from HyperGraph windows to automate data processing and data summary.
Publishing and Reporting
Create, define, and export reports.
Collaboration Tools
Explore, organize and manage your personal data, collaborate in teams, and connect to other data sources, such as corporate PLM systems to access CAD data or publish simulation data.

View All Altair HyperWorks Help

Linear Gap

Linear gap is the simplest contact form used in Nastran simulations.

Linear gap can solve a large class of problems, such as hole bearing, heel-toe interaction and fitting contacts. Linear does not include friction, large displacements and material non-linearity. CGAP contact elements (node-to-node defined in the FEM environment) run in both linear static (SOL101) and non-linear analysis (SOL106).

The linear gaps provide for simple contact (compressive) forces only. MPC’s are used to define the gaps. The displacements and MPC-forces are used to determine if each gap is "welded" or "free".

Displacement criteria: no penetration (MPC displacement > =0)
MPCFORCE criteria: compressive force only (MPC force < =0)

The solution converges when there is no penetration of MPC's (gap deflection > = 0.0) and there are no tensile forces. An iterative procedure (CDITER-constrained displacement iterative technique) is used to solve the model based on displacements/MPC forces. The image below is an example where the CGAP is modeled.

Figure 1.

The equation for the gap displacement can be written as:

Uygap = Uyopening – Uyclosing + Uyinitial

Rearranging in MPC format and setting Uyclosing as the dependent (first) term:

Uyclosing – Uyopening + Uygap – Uyinitial = 0

The Nastran commands to use for linear gaps are the following:

SPOINT (scalar point definition) is used to define the U_gap and U_init :

SPOINT 55 155

The SUPORT entry specifies reference degrees-of-freedom for rigid body motion, and it puts SPOINT 55 (U_gap) in the R-set for iteration:

SUPORT 55 0

SPC selects a single-point constraint set to be applied and defines the initial gap opening = .05 (U_init):

SPC 101106 155 0 .05

MPC entry: (equations of motion: Uy3 – Uy2 + U_gap – U_init = 0)

$ SID G1 C1 A1 G2 C2 A2

MPC 101106 3 2 1.0 2 2 -1.0

$ G3 C3 A3 G4 C4 A4

55 0 1.0 155 0 -1.0

Related MSC/Nastran Bulk Data Entries are:

PARAM, CDITER (integer) maximum number of iterations to determine open/closed
PARAM, CDPRT (yes/no) print iteration history of constraint violations
PARAM, CDPCH (yes/no) punches DMIG, CDSHUT entries for final solutions
DMIG, CDSHUT: input vector of initial open/closed state of gaps (default = all closed)

Figure 2.