Creating Parts

A. Extrude the Sketch

Extrude turns a flat sketch into a solid part

Using Extrude to turn the sketch into a solid part

1. Select the Extrude tool
2. Select the sketch you completed in the previous chapter
3. Set the depth to 1.5 in
4. Check Symmetric (extrudes equally on both sides, 0.75 in each)
5. Click the green checkmark ✓ to confirm

Congratulations! You just created your first solid part in context!

B. Add Fillets and Cutouts

Turn Off Assembly Context

The following operations don't need the assembly for reference. Set Assembly context to None in the left panel for a cleaner view.

Add Fillets

The Fillet tool rounds sharp edges

Using the Fillet tool to round edges

1. Select the Fillet tool (shortcut Shift+F)
2. Select the two short vertical edges of the part and set the fillet radius to 0.5 in
3. Then select the bottom rear edge and set the fillet radius to 0.25 in
4. Click the green checkmark to confirm

Create a Cutout Sketch

Draw a rectangle on the bottom face, then use Extrude Remove to cut through

Creating the cutout sketch on the bottom face

1. Create a new Sketch on the bottom face of the part
2. Switch to the Bottom view
3. Use the Use tool (U key) to select the bottom edge, then press Q to convert it to Construction (reference line)
4. Use Corner rectangle (shortcut G) to draw a 0.25 x 0.5 in rectangle
5. Dimension the rectangle to be 0.375 in from the left edge
6. Use the Mirror tool with the Right plane as the mirror axis to mirror the rectangle to the other side
7. Commit the sketch

Cut the Slots

Using Extrude Remove to cut through the part

1. Select the Extrude tool
2. Select the rectangle sketch you just created
3. Set the type to Remove (subtract material)
4. Set End type to Through all (cut through the entire part)
5. Click the green checkmark to confirm

In the feature tree on the left, right-click and rename this part to Base.

C. Mounting Holes and Sensor Mount

Reference Tube Holes

Switch back to Assembly context and Use the tube holes to position mounting holes

Referencing tube holes to create mounting holes

1. Switch Assembly context back to Context 1
2. Create a new Sketch on the top face of the Base part
3. Hide the Base part so you can see the tube below
4. Use the Use tool to select two holes on the tube
5. Unhide the Base part
6. Use Extrude Remove → Through all to cut these two holes through the Base

Create the Sensor Mount

Use the sensor's outer edge and mounting holes, then extrude the sensor mount

Creating the sensor mount

1. Create a new Sketch on the back face of the sensor area on the Base
2. Use the Use tool to select the sensor's outer edge and mounting holes
3. Commit the sketch
4. Use Extrude to extrude 0.125 in
5. Rename the new part to Sensor Mount in the feature tree

D. Support Structure and Details

Add Support Structure

Use Extrude to add support posts connecting the Base and Sensor Mount

Drawing the support structure sketch

Extruding the support structure to connect Base and Sensor Mount

1. Create a new Sketch on a side face of the Base
2. Use Center point circle (shortcut C) to draw a circle
3. Use the Use tool to reference the right edge
4. Draw tangent connecting lines
5. Use Extrude Add, set Merge scope to Sensor Mount, and End type to Up to face

Second Support

1. Extrude again with End type set to Up to face
2. Also set Second end position (bidirectional extrude to face)

Using Mirror to replicate the support structure to the other side

Drill Holes

Using the Hole tool to drill standard-spec holes

1. Select the Hole tool
2. Set the type to Simple
3. Set the spec to ANSI #8
4. Select a mate connector to position the hole
5. The hole should pass through both parts

Nut Recess

Using a hexagonal cutout to accommodate a nut

1. Create a new Sketch and select Inscribed polygon
2. Set to 6 sides (hexagon, to fit a nut)
3. Width: 0.345 in
4. Use Extrude Remove with a depth of 0.1875 in

Keyboard Shortcuts Review