Creating Shapes  

This task shows how to create shapes.

The Shape command allows you to create shapes of different sections, including curved or twisted shapes. 
There are two methods for placing a shape: 
  • selecting an existing support element (e.g., line, spline, arc, etc.) 
  • point-to-point 
1. With your product open, click the Shape button .

The Shape dialog box opens. (If the Type is set to Point to Point then the Point Definition dialog box will also open.)
   
2. To place a shape on an existing support element, choose Select Support in the Type field. 
3. Click the Material & Orientation tab and select material, grade and section. See Material Management for more information about selecting material.

Material, grade and section are defined in the specifications catalog.
4. Select the support line on which you want to create the shape. 

The shape is created in preview.

  Note: Multi-selection of supports is available.

To visualize selected supports, click the List icon or right-click in the Support field and select Elements list from the contextual menu. The Elements list dialog box opens showing selected supports.
   

Shape Orientation

If the support line is vertical, the web of the shape (local V-axis of section) is oriented toward the Y-axis of the document coordinate system.

If the support line is non-vertical, the web is oriented toward the Z-axis of the document coordinate system.

In the Shape dialog box, the selected support line will display in the Support field under Placement.
    In the Material & Orientation tab click the drop-down arrow opposite the Anchor point field to select the desired anchor point for the shape you are creating.
    Use the arrows in the Angle field to rotate the section. The default is in 90 degree increments, but you can change the step. To change it, right click on the Angle field and select Change Step in the drop down menu.
    Use the Flip button to flip the section about its vertical axis.
    Click the Custom Attributes tab to change the values of attributes added by the user. See Adding/Modifying Custom Attributes.

These attributes can also be browsed and edited via the Properties dialog box.
9. Click OK when done. The shape is created.
Similarly, you can create a shape on a curved support line. Using the Select Support method, simply select a curved line.

Creating Curved or Twisted Shapes

In the case of a swept or lofted surface in a design where a shape may curve or twist, you can create the shape normal to the surface. This is done using the Reference option in the Shape dialog box.
  • In a product utilizing a sweep or loft in the design, create a shape on a support line as described in the previous steps.
  • In the Shape dialog box, click in the Reference field.
  • Select the surface of the sweep as the reference. The name of the object appears in the Reference field and the shape becomes normal to the surface.

Using Point-to-Point to Create a Shape

This method requires no support.

  It lets you place shapes using points, a plane or an axis, and lets you define shape limits in different ways, for example by specifying a length.
1. With your product open, click the Shape icon .

The Shape dialog box opens. 
  2. To create a shape using the point-to-point selection method, select Point-to-point in the Type field. 

The Point Definition dialog box will open. 
  3. Make the necessary changes to the Section, Material, Anchor Point and Orientation settings, and (optional) valuate any attributes.
  4. In the Direction list, select how you want to place the shape.

You can place shapes using points, a plane or an axis.
 
   

Unspecified Planes and Lines

  • When placing parallel to or on an unspecified plane, you must select a plane before defining shape limits.
    The plane is identified in the Direction support field and the shape is placed parallel to or projected onto the selected plane.
  • Similarly, when placing parallel to an unspecified line, you must select a line before defining shape limits.
    The line is identified in the Direction support field and shape is placed parallel to the selected line.
 

Specifying an Offset to the XY, YZ or XZ Plane

Specifying an offset is particularly useful when creating shapes between existing structures. The offset is computed along the normal to the defined plane.

  • Select the Offset checkbox and enter a value or use the arrows to change the value in the Offset field that appears. You can enter a positive or a negative value.
  • Select wireframe elements or two existing structures.

This option is only available when the selected direction is parallel to the XY, YZ or XZ plane.

  5. Define the limits of the shape you want to create.

You can define the start and end points of a shape in different ways, by:
 

Entering Coordinates

  • Enter the XYZ coordinates in the Point Definition dialog box or in the power input field in the status bar.
    You can combine coordinates and selection of 3D points when defining start and end points for shapes.
   
   

Retrieving Coordinates using 3D Compass

You can use the 3D compass in the Point Definition dialog box to retrieve point coordinates:

  • Drag the 3D compass to the location of interest.
  • Select the 3D compass icon in the Point Definition dialog box.
    The compass coordinates are retrieved and taken as the start point.
  • Repeat again if desired to define the end point.
 

Creating a Point on a Existing Shape

You can also use the Point on member option in the Point Definition dialog box to define a point on an existing shape:
  • Click the Point on member option and select the existing section, or shape, of interest.

    The Start and End points of the section are identified and Offset will display a zero value. 
  • Enter the value for the Offset. Or you can move your pointer over Offset. When it highlights red, click and drag the dot (Start or End point) to set the desired offset. 

 
  • Click OK in the Point Definition dialog box. 
  • Now, select the terminating point for the shape you are creating and click. The shape is created.

 

 

Specifying a Length

  • Enter XYZ coordinates or select a 3D point to define the start point.
  • Select the Length checkbox and enter a value or use the arrows to change the value in the Length field that appears.
  • Indicate in the geometry area to identify the direction.
  6. Click OK when done.