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How to extrude cut in SolidWorks?

An extruded cut is used to cut away material from a body. To create an extruded cut, a body must already exist. This tutorial will investigate the options that are available to create and extruded cut.

From

Start Conditions specify where to start the cut. The options available for the start condition are explained below:

Sketch Plane – Creates a cut starting from the sketch plane to the specified depth.

Surface/Face/Plane – Starts a cut from a reference surface, face or plane. This option is useful to offset the start of a cut to another surface.

Vertex – Instead of inputting an offset or using a plane, this option will start a cut from a vertex or sketched point.

Offset – This starts a cut from using a specified offset value, the flip direction button controls the direction of the cut.

Direction

End condition specify where the cut ends. The list of end conditions are explained below:

Blind – Creates an cut in one direction, the direction is controlled by the “Reverse Direction” option.

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Through all – This creates a cut in a single direction, the length is set to the end of the part. See the example to follow for more details.

Through all Both – Sets direction 1 and 2 to through all.

Up to Next – This is similar to through all, but is dependent on what part of the body the sketch intersects. If the sketch intersects any portion of the longest section, then this end condition functions like through all. Refer to the example for more detail.

Up to Vertex – Sets the end condition to either a sketch point or the vertex of a body.

Up to Surface – Creates a cut up to the selected surface.

Offset from Surface – Use this option to create a cut up to a specified distance from a reference plane or face.

Up to Body – In a multibody part, this creates a cut though one body, up to the selected face of another.

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Mid Plane – Creates a cut in both directions, the length is determined by user input.

Depth – The specified length of the cut.

Draft On/Off – Without this option, the faces of cuts are parallel. Use this option to create a cut with a taper. Tapers can be turn on/off and have different values for directions 1 and 2.The direction of the taper is controlled using the “Draft outward” tick box.

Direction 2 – Available so long as mid plane has not been selected for direction 1. Direction 2 must be opposite to direction 1, making any end condition listed above bi-directional. End conditions and tapers can be set independently for either direction.

Example

Extrude1 – Sketch an 85mm Square on the front plane, coincident with the origin. Use the following extrude options: Sketch plane, mid plane, depth = 30mm.

Extrude2 – On the back face of the square, sketch a rectangle 250x115mm. Set the extrude options to: Sketch, Blind, depth = 10mm.

Cut-Extrude1 – Sketch a rectangle (25x15mm) on the right plane, and make the corner coincident with the top edge of extrude1. Set the end conditions for direction 1 and 2 to “Up To next”. Switch between “Up to Next” and “Through all Both” to see the difference in the preview of the cut.

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Cut-Extrude 2 – Sketch the same rectangle as cut-extrude1. Constrain the center point to horizontal with the origin, and coincident with the back edge of extrude1. Set the end conditions for direction 1 and 2 to “Up To next”.

To confirm that up to next acts as through all both, an extrude was positioned in its path. The final result and a side view of the cut on the extrude are shown below.