> > About Translating Sketch Geometry

You can translate the sketch geometry within an active sketch. Drag the translation handle until you achieve the required translation, or specify the translation value in the Rotate Resize tab.
Consider the following points when you translate sketch geometry:
You can select a reference to define a translation reference. The translation reference can be:
Any line or centerline within the geometry that you select for translation.
Any line or centerline that belongs to the active sketch group or any of the subgroups within the active sketch group, if the geometry that you select for translation is within a sketch group that is not a top-level sketch.
Any line or centerline that belongs to the top-level sketch or any other sketch group within the sketch, as well as any linear external reference such as a plane, axis, linear edge, or curve, if the geometry that you select for translation is within the top-level sketch.
You can translate the geometry freely in the sketch plane or constrain the geometry to the parallel or perpendicular direction with respect to the translation reference.
When you translate the geometry in a direction that is nearly parallel or perpendicular to the translation reference, the dragging is constrained in the parallel and perpendicular directions.
If you do not select a translation reference, you can translate the geometry freely or constrain it to the horizontal or vertical direction.
You can drag the translation handle independent of the geometry, and constrain it to:
The geometry itself
Other sketch geometry within the same sketch group
Geometry that belongs to the subgroups within the active sketch group
An external reference geometry, if the selected geometry is the top-level sketch
When you translate a geometry within a sketch group, the horizontal and vertical directions are defined by the group reference coordinate system.
When you translate the geometry in a direction that is nearly horizontal or vertical, the dragging is constrained in the horizontal or vertical direction.
Two direction and two distance dimensions are added to the translation handle when you translate sketch geometry. The direction dimensions correspond to the parallel and perpendicular directions or the vertical and horizontal directions. The distance is measured with respect to the original location of the original geometry and along the corresponding direction.
The direction dimensions are temporary dimensions and are removed when you complete the translation operation.
You can select a temporary dimension in the graphics window and specify a value for the translation.
You can specify the translation reference and the translation value in the Rotate Resize tab.