To Define Varied Dimensions for Flexibility
1. Open an assembly.
2. Choose one of the following items:
◦ A flexible component—Select the component, right-click it in the Model Tree or graphics window, and choose
from the shortcut menu. The
Component Placement tab opens. Click
Flexibility >
Varied Items. The
Varied Items dialog box opens.
◦ A component without defined flexibility—Select the component, right-click it in the Model Tree or graphics window, and choose Make Flexible > Make Flexible from the shortcut menu. The Component Placement tab opens with the Varied Items dialog box open.
3. To add a new
Dimension varied item, select a dimension and click
. The new dimension appears in the table.
4. Enter a New Value for the feature dimension or select an option from the Method list:
◦ By Value (default)—Enter a value in the New Value cell.
◦ Curve Length—Opens the Length dialog box. Click Definition and select a curve or edge to define its value. Click Details to open the Chain dialog box. Set Standard or Rule-basedReferences for the curve chain. Rule-based references allow you to choose an anchor and chain type: Tangent, Partial loop, or Complete loop. Configure an Extent Reference for a partial loop chain and use Options if required.
| For more information on chains, search the Help Center. |
◦ Distance—Opens the Distance dialog box. Click Definition and select two entities to drive the new value.
◦ Angle—Opens the Angle dialog box. Click Definition and select two entities to drive the new angle value.
◦ Area—Opens the Area dialog box. Click Definition and select the surface to drive the new value.
◦ Diameter—Opens the Diameter dialog box. Click Definition and select a round surface or edge to drive the new value. Click the Point box and select a point from which to begin the new diameter calculation.
5. Click
.
| You can define a Geometric Tolerance for the varied dimension. Only the By Value option is applicable for setting a geometric tolerance. |