Engineering Connection Definition Dialog Box

The Engineering Connection Definition dialog box appears when you select Engineering Connection.

This dialog box contains controls for:



Constraints

Type
The options in the engineering connection Type are as follows:
  • User Defined
  • Rigid
  • Spherical
  • Cylindrical
  • Planar
  • Prismatic
  • Revolute
  • Screw
  • Point Curve
  • Point Surface
  • Gear
  • Rack
  • Cable
  • Universal
  • Roll Curve
  • Slide Curve
  • Fix
  • Free
  • Symmetry
  • Projection.

    This engineering connection is used typically for positioning of a Spot Fastener Instance (see CATIA : Mechanical : Fastener Design for further information on Spot Fasteners).

  • Pattern
Important:
  • The engineering connection type is defined by a combination of Driving constraint and Controlled constraint.

    The engineering connection type is automatically detected when its Driving constraints respect its definition.

  • A constraint can be deactivated. In this case it is not taken into account during the PLM update.

    A deactivated mask (red parentheses) appears on the upper left corner .

  • Examples of the Driving constraint relation in Engineering Connection Type above are not necessarily exhaustive.
Lock or Unlock an Engineering Connection Type
When you are creating an engineering connection, the Type field is updated according to the created constraints.
  • Lock: The engineering connection type is locked. Modification of constraint definitions outside the engineering connection type definition is possible, but the engineering connection type will be detected in error during the PLM update.
  • Unlock: The engineering connection type is unlocked. The Type field is updated according to constraint definition modifications.

Note:

If you are a DS Passport Customer, you can read the Knowledge Base for more about Revolute behavior in Lock and Unlock modes.

Engineering Connection Templates
According to the selected engineering connection type, Engineering Connection Templates displays the constraints, constraint modes and constraint elements needed to define the engineering connection type.
Important:
  • Using this option you can create an engineering connection from scratch, then select the geometry.
  • This option can be enabled after you lock the engineering connection type; in this case missing constraint is proposed.
Constraint Definition
Constraint Type
The following constraints can be created according to the context type, from a contextual menu:
  • Insert a constraint:
    • Contact
    • Fix together relatively
    • Fix together
    • Coincidence
    • Offset
    • Angle
      • Angle
      • Parallelism
      • Perpendicularity
      • Hinge
    • Curve
      • Curvilinear distance
      • Roll
      • Slide
    • Symmetry
    • Coupling

      See also Coupling Dialog Box.

    • Fix
    • Fix in space
  • Delete the constraint.
  • Replace the constraint by another one.
    Important:

    When elements defining the constraint are not compliant with the new one, a warning message appears, the previous constraint is deleted and you have to select new geometries.

  • Deactivate the constraint. In this case the constraint is not taken into account during the PLM update.
Constraint Mode
This column displays the constraint icon. Three modes are available:
  • Driving: the constraint definition is applied during the PLM update.
  • Measured: the constraint value is deducted from its definition and other constraints of the engineering connection during the PLM update.
  • Controlled: defines the constraint controlled by the user in the kinematics relation. The constraint value is defined between bounds.
    Important:

    When a constraint leads to an unpredictable state, a warning mask will appear on all controlled constraints.

Constraint Options
This column displays the constraint geometry option and is filled only when the orientations of the selected elements are taken into account in the constraint definition:
  • For a plane:
    • Undefined: the plane orientations are undefined and can be modified during the PLM update.
      Important:

      Leaving the plane orientations undefined may allow an inversion of the components repositioning during:

      • PLM update process,
      • or move under constraint,
      • or using Assembly Design Manipulation command.

    • Same Orientation: the plane orientations are the same.
    • Opposite Orientation: the plane orientations are opposite.
  • For a line:
    • Undefined: the line orientations are undefined and can be modified during the PLM update.
    • Parallelism: the lines are parallel but not oriented.
    • Same Orientation: the line orientations are the same.
    • Opposite Orientation: the line orientations are opposite.
  • For a hinge:
    • Direct Angle
    • Angle + 180deg
    • 180deg - Angle
    • 360deg - Angle
  • For an axis system:
    • x axis
    • y axis
    • z axis
Lower
This column displays the lower constraint value for an angle or an offset.

This value is used for a constraint in Controlled mode.

Value
This column displays the constraint value for an angle or an offset, or the ratio%offset value for a coupling.
Important:

A value may be unset to leave the value unspecified.

Upper
This column displays the upper constraint value for an angle or an offset.

This value is used for a constraint in Controlled mode.

Constraint Support
This table displays the constraint support:
Element/Geometry Icon
Axis system
Circle
Cone
Continuous curves
Curve
Cylinder
Edge
Face
Line (from Generative Shape Design)
Plane (from Generative Shape Design)
Point (from Generative Shape Design)
Product
Sketch containing continuous curves
Sphere
Surface
Vertex
Important:
  • Some masks can be displayed on the support icon:
    Status OK Warning Error
    Free
    Locked
    Published
    Locked & Published
  • A support is automatically locked when the engineering connection is created or when you click Engineering connection templates .

Interferences



Important:

You can only access the Interferences tab for the configurations or products you installed and for which you have a license.

Check specification
The options in the Check specification are as follows:
  • Default: no interference specification has been defined in the engineering connection.
  • Check:
    • No clash: checks clash between components involved in the engineering connection.
    • Contact: checks contact between components involved in the engineering connection.
    • Clearance: checks the minimal clearance between components involved in the engineering connection with the defined value.
  • No check: do not check interference.

Simulation



Important:

You can only access the Simulation tab for the configurations or products you installed and for which you have a license.

Connection property
The options in the Connection property are as follows:
Distant

Creates a distant connection property.

User-defined

Creates a user-defined connection property.

Face face

Creates a face face connection property.

Fastened

Creates a fastened connection property.

Bolt tightening

Creates a bolt tightening connection property.

Spot weld

Creates a spot weld connection property.

Seam weld

Creates a seam weld connection property.

Curve curve weld

Creates a curve curve connection property.

Surface weld

Creates a surface weld connection property.

Add
Opens the User-defined Connection Property dialog box in order to create a user-defined connection property.
Connection Properties
Display the list of connection properties in the Engineering Connection.