Defining Small Assemblies

Main steps are:

• Defining input geometry
• Sketching the contour in a positioned sketch 
• Creating the small assembly
• Creating an assembly template.

Small assemblies are document templates. Templates created reference the shapes and plates making up the assembly.

(Tools - Options - Infrastructure - Part Infrastructure - General).

Defining Input Geometry

This part will contain input geometry, i.e. imported plate and shape surfaces or edges.

• Switch to the Wireframe and Surface workbench (Start -> Mechanical Design -> Wireframe and Surface Design).
• Using the Intersection command , create the intersection geometry between planes of the new part and surfaces/edges of the plates and shapes and/or reference planes.
  Surfaces/edges are imported under an External References entry in the specification tree.

• When done, delete the geometrical set containing the intersect entries.

• Rename imported surfaces/edges as follows:

Plate surfaces/edges: Platen_(name of the published plate surface or edge)
Shape surfaces/edges: Shapen_(name of the published shape surface or edge)
where n is a number identifying the number of parts to be selected by the user when instantiating the assembly template.

For example, Plate1_Face_Standard, Shape1_Face_MoldedFlange1

• Isolate imported surfaces/edges and rename the Isolated External References entry, for example, Isolated Inputs.
  This breaks the link between imported surfaces/edges and referenced shapes.

Note: The user feature creating stable geometry uses rules and formula.

You must not use these planes when creating construction geometry.

Sketching the Contour in a Positioned Sketch

Using a positioned sketch lets you explicitly define the position of the absolute axis of the sketch. To create a positioned sketch, you must specify a reference plane, an origin and the orientation of the absolute axis.

The new body inserted below will contain the geometry needed to define a positioned sketch as well as the small assembly contour.

Stable lines are lines whose orientation is known and whose orientation will be kept when the small assembly template is instantiated.

• Select Insert -> Instantiate from Document... from the menubar to instantiate the user feature OrientedCurve.CATPart located in folder ..\OS\startup\EquipmentAndSystems\Structure\DetailingFeatures\UtilityUDFs

OrientedCurve.CATPart has two inputs and one parameter:

1. a curve or line (can be an intersect)
2. a reference surface
3. a parameter determining whether or not the starting point of the line is the nearest element to the reference surface.

• Select one of the wireframe lines just created then select a reference surface. The reference surface must be an offset or an extract of the imported external reference.
• If necessary, click Parameters in the Insert Object dialog box to define the starting point of the stable line.
  By default, the starting point is the point nearest the reference surface.
• Click Preview to visualize the stable line.
  The user feature generates a line (in bold blue) oriented as defined by the parameter and two points, one at each end of the line. The start point is represented by a green circle and the end point by a white cross.
• Check Repeat in the dialog box then click OK when done.
  The user feature is automatically re-instantiated when the Repeat option is checked.
• Repeat to create other stable line.
  Do not forget to uncheck the Repeat option before clicking OK.

• Create a plane from the two stable lines.
  
  Note: Any of the points created by the user feature can be used to specify the origin of the sketch.

The Sketch Positioning dialog box opens.

• Keep Type set to Positioned.
• Select the plane created above as the reference plane for the sketch support.
• Define the sketch origin as follows: Set Type to Projection point then select one of the points created above.
• Define sketch orientation as follows: Set Type to Parallel to line then select one of the two lines defined above.
• Use dialog box options to orient the H,V axis system correctly.
• Click OK.

The Sketcher workbench opens.

• Do not apply vertical or horizontal constraints.
• Constrain the sketch to stable construction geometry.
• A green sketch means your contour has been properly constrained.
• You are advised to change values of parameters that the user will be required to enter to ensure that the small assembly behaves correctly.

• Switch to the Part Design workbench (Start -> Mechanical Design -> Part Design)
• Select Tools -> Publication.

This will ensure that you select only published geometry when creating plates and shapes.

Creating the Small Assembly

For a plate, use the Support and contour mode, selecting the plane created as support.

Creating an Assembly Template

The Document Template Definition dialog box opens, listing CATParts in the document.

• Any documents referenced must have New document Action status.
• Click the Inputs tab and then select isolated surfaces/edges.
• Enter roles for these surfaces/edges using the following naming conventions:

SHAPEn _(name of published shape surface or edge)
where n is a number identifying the number of parts to be selected by the user when instantiating

PLATEn_(name of published plate surface or edge)
where n is a number identifying the number of parts to be selected by the user when instantiating

For example,
SHAPE1_Edge_MoldedFlange2
PLATE1_Face_Standard

• Click OK when done.

The assembly template is created under a Knowledge Templates entry in the specification tree.