SolidWork 2013 - Modifying Tool - How to Fillet, Chamfer And Offset

Filleting Sketched Entities

CommandManager: Sketch > Sketch Fillet

SolidWorks menus: Tools > Sketch Tools > Fillet

Toolbar: Sketch > Sketch Fillet

A fillet creates a tangent arc at the intersection of two sketched entities.You can apply a fillet to two nonparallel lines, two arcs, two splines, an arc and a line, a spline and a line, or a spline and an arc. A fillet between two arcs, or between an arc and a line depends on the compatibility of the geometry to be extended or filleted along the given radius.

You can first choose the Sketch Fillet tool from the Sketch CommandManager, and then select the entities to be filleted or select the vertex formed at the intersection of the two entities to be filleted. Alternatively, you can hold the CTRL key and select the two entities to be filleted and then invoke this tool.

When you invoke the Sketch Fillet tool, the Sketch Fillet PropertyManager will be displayed. Next, select the entities; the preview of the fillet with default radius will be displayed. You can drag the fillet preview to resize it to the required radius or set the radius in the Fillet Radius spinner and press ENTER; a fillet will be created and the Sketch Fillet PropertyManager will be displayed even after applying a fillet. This enables you to create multiple fillets in a sketch. If you create multiple fillets of different radii, then all fillets need to be dimensioned individually. To do so, select the Dimension each fillet check box. But if you need to create multiple fillets of same dimension, then it is recommended that this check box should be cleared. If the Keep constrained corners check box is selected, the dimension and geometric relations applied to the sketch will not be deleted. If you clear the Keep constrained corners check box, you will be prompted to delete the relations applied to the corners of the sketched entities to be filleted. Choose the OK button to exit the Sketch Fillet PropertyManager.

You can also select the non-intersecting entities for creating a fillet. In this case, the selected entities will be extended to form a fillet.

Chamfering Sketched Entities

CommandManager: Sketch > Sketch Fillet flyout > Sketch Chamfer

SolidWorks menus: Tools > Sketch Tools > Chamfer

Toolbar: Sketch > Sketch Fillet flyout > Sketch Chamfer

The Sketch Chamfer tool is used to apply a chamfer to the adjacent sketch entities at the point of intersection.

A chamfer can be specified by two lengths or angle and length from the point of intersection. You can apply a chamfer between two nonparallel lines that may be intersecting or non-intersecting. The creation of a chamfer between two non-intersecting lines depends on the length of the lines and the chamfer distance.

To create a chamfer, choose the Sketch Chamfer button from the Sketch Fillet flyout of the Sketch CommandManager; the Sketch Chamfer PropertyManager will be displayed. Next, select the two entities to be chamfered. You can also select the two entities before invoking the Sketch Chamfer tool. The options in the Sketch Chamfer PropertyManager are discussed below.

Angle-distance

The Angle-distance radio button is selected to create a chamfer by specifying the angle and the distance. When you select this radio button, the Direction 1 Angle spinner will be displayed below the Distance 1 spinner. Specify the distance and angle values in the Distance 1 and Direction 1 Angle spinners, respectively. Next, select the two entities to which the chamfer needs to be applied; a chamfer will be created. Note that the angle will be measured from the first entity you have selected.

Distance-distance

When you invoke the Sketch Chamfer PropertyManager, the Distance-distance radio button and the Equal distance check box are selected by default. Clear this check box to specify two different distances for creating chamfer. When you clear this check box, the Distance 2 spinner will be displayed below the Distance 1 spinner to set the value of the distance in the second direction. Specify the distance value in both the spinners. Next, select the two entities that need to be chamfered; the chamfer will be created.

Equal distance

When you invoke the Sketch Chamfer PropertyManager, the Distance-distance radio button and the Equal distance check box are

selected by default. As a result, you can create an equal distance chamfer between the selected entities. Specify the distance value in the Distance 1 spinner and select the entities; the chamfer will be created.

Choose the OK button from the PropertyManager to exit the tool.

Offsetting Sketched Entities

CommandManager: Sketch > Offset Entities

SolidWorks menus: Tools > Sketch Tools > Offset Entities

Toolbar: Sketch > Offset Entities

Offset is one of the easiest methods to draw parallel lines or concentric arcs and circles. You can select the entire chain of entities as a single entity or select an individual entity to be offset. You can offset the selected sketched entities, edges, loops, and curves. You can also select the parabolic curves, ellipses, and elliptical arcs to be offset.

When you choose the Offset Entities button from the Sketch CommandManager, the Offset Entities PropertyManager will be displayed. The options in the Offset Entities PropertyManager are discussed below.

Offset Distance

The Offset Distance spinner is used to set the distance through which the selected entity needs to be offset. You can set the value of the offset distance in this spinner or set the value by dragging the offset entity in the drawing area.

Add dimensions

The Add dimensions check box is selected by default in the Parameters rollout. Therefore, a dimension showing the offset distance between the parent entity and the resulting offset entity will be displayed on creating offset entities.

Reverse

The Reverse check box is used to change the direction of the offset. Note that while offsetting the entities by dragging, you do not need this check box. This is because you can change the direction of the offset by dragging the entities in the required direction.

Select chain

The Select chain check box is used to select the entire chain of continuous sketched entities that are in contact with the selected entity. When you invoke the Offset tool, the Select chain check box will be selected by default. If you clear this check box, only the selected sketched entity will be offset.

Bi-directional

The Bi-directional radio button is used to create the offset of a selected entity in both the directions of the selected entity.

Make base construction

The Make base construction check box is used to convert the parent entity into a construction entity.

Cap ends

The Cap ends check box is available only when the Bi-directional check box is selected in the Offset Entities PropertyManager. On selecting this check box, the ends of the bidirectionally offset entities will be closed. You can select the Arcs or Lines radio button to specify the type of cap to close the ends.