Adding Threads

1. On the CommandManager, click Features > Reference Geometry > Plane.
2. Click on the top face of the model geometry.
3. Set the Distance value to 5 and check the Flip offset option.
4. Click OK; a new reference plane is created.

1. Start sketch on the new reference plane.
2. On the CommandManager, click Sketch > Convert Entities.
3. Click on the outer edge of the cylindrical feature and click OK.

1. Click Exit Sketch.
2. On the CommandManager, click Features > Curves > Helix and Spiral.
3. Select the circular sketch.
4. On the PropertyManager, select Constant pitch.
5. Type-in 7 in the Pitch box and check the Reverse Direction option.
6. Type-in 2 in the Revolutions box.
7. Set the Start Angle value to 0.
8. Uncheck the Taper Helix option.
9. Click OK.

1. On the CommandManager, click Features > Reference Geometry > Plane.
2. Click on the helix and its start point.

1. Click OK.
2. Start a sketch on the new reference plane.
3. On the Heads-Up toolbar, click View Orientation drop-down > Normal To.
4. Activate the Line command and specify the points of the line-chain, as shown.

1. Activate the Centerline command and horizontal line.

1. Press the Ctrl key and select the left endpoint of the centerline. Next, select the helix.

1. On the PropertyManager, click the Pierce icon; the endpoint of the centreline is pierced with the endpoint of the helix.

1. Press the Ctrl key and select the lower endpoint of the vertical line of the sketch. Next, select the centreline.

1. Click the Coincident icon on the PropertyManager.
2. Click and drag the left vertical line of the sketch such that it is inside the model geometry.

1. Activate the Sketch Fillet command and type 0.5 in the Fillet Radius box on the PropertyManager.
2. Select the corner point of the right vertical and inclined line, as shown.

1. Click OK on the PropertyManager.
2. On the CommandManager, click the Mirror Entities button, and then select all the sketch elements except the centreline.
3. On the PropertyManager, click in the Mirror about selection box, and then select the centreline.
4. Click OK to mirror the selected elements about the centreline.

1. Add dimensions to sketch using the Smart Dimension command.

1. Click Exit Sketch.
2. On the CommandManager, click Features > Swept Boss/Base.
3. Click on the thread profile and the helix.

1. On the PropertyManager, expand the Options section and check Merge result.
2. Click OK.

1. Start a sketch on the end face of the thread.

1. On the CommandManager, click Sketch > Covert Entities and select the thread profile of the Swept feature from the FeatureManager Design Tree.

1. Click OK.

1. Click Exit Sketch.
2. Activate the Revolved Boss/Base tool and click on the vertical line of the sketch.
3. On the PropertyManager, set Direction 1 Angle to 100.
4. Use the Reverse Direction button, if the preview of the revolved feature is displayed inside the model.
5. Check the Merge result option.

1. Click OK.
2. Rotate the model and click on the other end of the thread.

1. Press the Ctrl key and select the sketch used for the previous revolved feature.
2. On the Menu bar, click Insert > Derived Sketch; the sketch is projected onto the sketch plane.

1. Press Esc to deselect the sketch.
2. On the CommandManager, click Display/Delete Relations > Add Relations.
3. Click on the inclined line of the sketch and the inclined edge of the end face.

1. On the PropertyManager, click Collinear.
2. Press the Ctrl key and click on the end-points, as shown in figure.

1. On the PropertyManager, click Coincident.

1. Create a revolved boss using the sketch.

1. Save the model and close it.