Extruded Boss/Base

We had exposure to Extruded Boss/Base in the last chapter but didn’t explore its full potential. The Extruded Boss/Base feature has many options controlling the depth of a feature: how deep the feature is extruded, which direction is the feature extruded, does the extrude taper, does it go up to a certain point or is offset from a certain point, etc.

When you start a boss extrude, either from a sketch or with intent to specify a new sketch, you are able to modify the property manager for the extrude feature. The following options are available:

From

Specify where your extruded feature will begin. The most common option is from the sketch plane, but you might want to start it from a different face/plane/vertex or offset it from the sketch plane for special situations.

End Condition

Specify where extruded feature will end.

• Blind: You can have it end a distance from the sketch plane
• Up to Vertex: The feature will extrude to the depth of a selected point.
• Up to Surface: The feature will extrude to the depth of a selected face or plane.
• Offset from Surface: The feature will extrude to the depth of a selected face or plane plus/minus a specified offset distance.
• Mid Plane: A popular option that allows the extruded feature to be centered about the sketch plane and end an equal distance from the sketch plane on both sides.

Extrude Direction

The default direction is 90 degrees from the sketch plane so you don’t usually need to specify anything in this box, but for instances when you want to extrude at an angle different from 90, you can select a model edge or reference line to specify a new direction.

Draft

Draft adds a taper to the extruded feature along the depth of the feature.

Direction 2

You can specify a second direction usually going in the opposing direction of the first. This is useful for specifying different depths/conditions from the sketch plane (which becomes the center of the extrude in this scenario).

Selected Contours

If you don’t want to extrude your entire sketch, you can specify the areas (or contours) that you want to extrude. This is a great efficiency tool we will learn about later that when used can reduce sketch time by almost a factor of ten. It eliminates the need to trim which is one of the most time-consuming tasks in sketching!

Extruded Cut

The Extruded Cut tool is another extrude feature that is used to make cut outs, pockets, etc. into your existing solid model.

An extruded cut can’t be your first feature in a part because you must cut into something, so you at least need to have one extruded feature in the model before you can use cut extrude. Extruded cut is a Sketch-Based Feature, so you start a sketch on a plane or a face in the model, sketch your cut profile, and then use cut extrude to specify the details of the depth of cut.

Sketching on Model Faces

Sketching on a model face is very similar to sketching on a plane. The key advantage however is that when you sketch on a model face, your extruded features will by default originate from that face. This fact is very useful in making the part shown in figure 4.4.

When sketching in a model that already has a feature in it, in your new sketch you can utilize the edges and faces from that already existing feature. For example, say for the model in figure 4.4 instead of specifying a length and width for the rectangular cutout, you wanted to specify that the rectangular cutout be an offset distance away from the exterior rectangle. You can then select the face of the exterior rectangle and use the offset command to offset the internal rectangle the distance you desire. You can also use Convert Entities to reuse model edges in a new sketch.

Cutting with Open Sketches

Another option that exists with the Cut Extrude tool is cutting models with open sketches. For example, if you wanted to saw off tubing at a 45-degree angle, instead of drawing a closed sketch that would completely miss your design intent, you can just draw a line at 45 degrees (Figure 4.5).

Hole Wizard

The hole wizard is a macro tool that combines sketching, extrudes, and revolved features into one highly customizable tool for creating standard holes. Think of the holes that fasteners and pins go into; this is the tool to quickly specify these kinds of holes! The hole wizard has two tabs: The type tab and position tab (Figure 4.7).

Type Tab

The type tab is used to specify the type of hole you want to specify such as whether it is a counterbore, countersink, tapped hole, etc. This is also where you specify the depth of your hole or if your hole goes all the way through the part, if it has a nearside or far side countersink, if the hole bottom needs to be flat or can have the shape of a drill bit, and much more.

Positions Tab

The positions tab is for placing your hole. This tab works more as a sketch where you select the face (this can be a planar or a curved face) where your hole will start and then sketch to define the location. Holes are placed with the point sketch tool . You have access to all the sketch tools you usually have in a sketch when on the positions tab of the Hole Wizard.