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How to extrude at an angle in SolidWorks?

The feature to be used will depend on the direction required.  An extrude can only ever be applied if the direction is normal to the sketch plane. The only option, where extrude is desired, is to apply a taper to the faces of the extrude. Alternatively, “Swept Boss/Base can be used to create an “extrude” at an angle that is not normal to the sketch plane. This tutorial will explore these two options in detail.

Using Swept Boss/Base

Begin by creating the profile of the extrude, in this case an 85mm square was used. On either perpendicular plane, create the sketch of the length of the extrude, use a reference from sketch 1 to set an angle. Alternatively, an angled plane can be used for the sketch of the path.

If the screenshot below is the desired result, there is no need to continue on.  Alternatively, if this is not the desired result, you may be looking for an extrude with a taper applied.

Using Extrude

From

The options for the Start Condition are as follows:

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Sketch Plane – Starts the extrude from the sketch plane.

Surface/Face/Plane – Use this to offset the start of the extrude using a surface, face or plane as a reference.

Vertex – This option will start the extrude from a defined point, either a sketch point or vertex of a body.

Offset – To start an extrude offset from the sketch plane. This requires an offset value, the direction is controlled by the flip direction button.

Direction

The options for the End Condition are as follows:

Blind – Extrudes the sketch profile in a single direction. Use the “Reverse Direction” button to control the direction of the extrude.

Up to Vertex – Ends the extrude from a defined point, either a sketch point or vertex of a body.

Up to Surface – Extrudes the profile up to a surface or flush with the face of a body.

Offset from Surface – Extrude the profile up to a specified distance from a plane or face.

Up to Body – Use this option when sketches are on offset planes. This will end the extrude at the selected face of an existing body.

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Mid Plane – This option creates a bi-directional extrude to the specified depth value.

Depth – User input for the depth of the extrude, this is only available with the blind or mid plane end condition. This changes to Offset distance for extrudes offset from a surface.

Merge result – This option is available if a feature/body exists. When ticked the extrude will become a part of the existing body, otherwise the extrude will form a new body. The image below shows Extrude2 with “Merge result” disabled.

Draft On/Off – This will taper the faces along the extrude. Tick “Draft outward” to alter the taper direction. The shape of the taper is affected by the selected End condition. A midplane extrude is the only bi-directional end condition, that does not allow tapers to be specified independently for either direction.

Direction 2 – Not available if the end condition for Direction 1 is set to “Mid plane”. This effectively makes the extrudes bi-directional, as the only direction available is opposite to that of direction 1. The end conditions can be the same or different. Tapers can be set independently for either direction.

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Example

Extrude 1 – Sketch an 85mm square on front plane. Select “Sketch Plane” for the start condition, set the end condition to “Mid Plane” and 30mm depth.

Extrude 2 – Sketch a rectangle (25x15mm) on right plane. Make the rectangle coincident with the top edge of extrude 1. Use the “Offset” start condition and set it to 15mm. Set the end condition to “Offset from surface”, input a value of 10mm and use the left face of extrude1 as the reference.

Extrude 3 – Create an offset plane 40mm from the front plane. Sketch a Ø30mm circle coincident with the origin. Use the “Sketch Plane” as the start condition. Set the end condition to “Up to Body”, select the front face of extrude1 as the reference. Turn on draft and set a 5° draft angle, and tick the draft outward option.

The final result is shown below.