SolidWork 2013 - Adding Geometric Relation To Sketch

ADDING GEOMETRIC RELATIONS TO THE SKETCH

The geometric relations are the logical operations that are performed to add a relationship (such as tangent or perpendicular) between the sketched entities, planes, axes, edges, or vertices. The relations applied to the sketched entities are used to capture the design intent. The geometric relations constrain the degree of freedom of the sketched entities. There are two methods to apply the relations to the sketch. These two methods are

1. Add Relations PropertyManager

2. Automatic Relations

Adding Relations Using the Add Relations PropertyManager

Toolbar: Sketch Relations > Add Relation

Menu: Tools > Relations > Add

The Add Relations PropertyManager is widely used to apply relation to the sketch in the sketcher environment of SolidWorks.

The Add Relations PropertyManager is invoked using the Add Relation button from the Sketch Relations toolbar. The Add Relations PropertyManager is displayed on the left of the drawing area as soon as you choose the Add Relation button. You can also invoke the Add Relations PropertyManager by right-clicking in the drawing area and choosing the Add Relation option from the shortcut menu.

Selected Entities

The Selected Entities rollout displays the name of the entities that are selected to apply the relations.

Existing Relations

The Existing Relations rollout displays the relations that are already applied to the selected sketch entities.

Add Relations

The Add Relations rollout is used to apply the relations to the selected entity.

The relations that can be applied to the sketches using the Add Relations rollout are discussed next.

Horizontal

The Horizontal relation forces the selected line or lines to become horizontal.

Vertical

The Vertical relation forces the selected line or lines to become vertical. Using the Vertical relation you can also force two or more points to become vertical.

Collinear

The Collinear relation forces the selected lines to lie on the same infinite line.

Coradial

The Coradial relation forces the selected arcs to share the same radius and the same centerpoint.

Perpendicular

The Perpendicular relation forces the selected lines to become perpendicular to each other. Select two lines to apply the Perpendicular relation.

Parallel

The Parallel relation forces the selected lines to become parallel to each other. Select two lines to apply the Parallel relation.

ParallelYZ

The ParallelYZ relation forces a line in the 3D sketch to become parallel to the YZ plane with respect to the selected plane.  Select the line in the 3D sketch and a plane and choose the ParallelYZ button from the Add Relations rollout.

ParallelZX

The ParallelZX relation forces a line in the 3D sketch to become parallel to the ZX plane with respect to the selected plane.  Select the line in the 3D sketch and a plane and choose the ParallelZX button from the Add Relations rollout.

AlongZ

The AlongZ relation forces a line in the 3D sketch to become normal to the selected plane. Select the line in the 3D sketch and a plane and choose the AlongZ button from the Add Relations rollout.

Tangent

The Tangent relation forces the selected arc, circle, spline, or ellipse to become tangent to other arc, circle, spline, ellipse, line, or edge.

 Select two entities to apply the Tangent relation.

Concentric

The Concentric relation forces the selected arc or circle to share the same centerpoint with other arc, circle, point, vertex, or a circular edge.

Midpoint

The Midpoint relation forces the selected point to move at the midpoint of the selected line.

Intersection

The Intersection relation forces the selected point to move at the intersection of the two selected lines.

Coincident

The Coincident relation forces the selected point to be coincident with the selected line, arc, circle, or ellipse.

Equal

The Equal relation forces the selected lines to have equal length and selected arcs, circles, or an arc and a circle to have equal radii.

Symmetric

The Symmetric relation forces two selected lines, arcs, points, and ellipses to remain equidistant from a center line. This relation also force the arcs to have the same radii. Select the required entity to apply the Symmetric relation and select a centerline. Choose the Symmetric button from the Add Relations rollout.

Fix

The Fix relation forces the selected entity to fix at the specified position.

Pierce

The Pierce relation forces a sketch point to be coincident where an axis, line, arc, edge, or spline pierce the sketch plane.

Merge Points

The Merge Points relation forces two sketch points or endpoints to merge in a single point.

Automatic Relations

The automatic relations are applied automatically to the sketch while drawing.

You can activate the automatic relations option if it is not available. Invoke the System Options - Sketch dialog box by choosing Tools > Options > System Options > Sketch. The System Options – Sketch dialog box is displayed. Select the Automatic Relations check box from the System Options - Sketch dialog box and choose the OK button.