In this tutorial you’ll learn how to make a bolt and a nut and also how to make simple animation.
Part 1. The bolt.
Start by selecting New Document icon from Standard toolbar, then select Part:
In the feature manager design tree, select top plane and open sketch:
Select Polygon and locate the zero point:
Make a drawing:
Use Smart Dimension to set the size to 18.6 millimeters.
Accept, then go to Zoom to Fit and select OK.
The drawing is not fully defined, so we need to add some relations. Select 3 points while holding the Control key, and add horizontal relation:
Exit the sketch, select Extrude Boss/Base from the command manager. For the depth, type 7mm and select OK:
Select this base and open a new sketch:
Click on Normal To View and draw a circle:
Add relation, tangent:
Click on isometric view. Exit sketch.
Go to Extrude Cut. Set Flip side to cut and Draft On, type 60 degrees.
On the opposite face open a new sketch. Select Normal To View and draw a circle. Smart dimension it to 10mm:
Select isometric view and exit sketch, then select Extrude Boss Base, type 45 mm:
Now we need some fillet. Select fillet command and set its size to 1mm:
Also, we need to add some chamfer. Select chamfer, also 1mm, 45deg and select this sketch:
Go to isometric view.
Now create helix. Select this face and open sketch:
Select this edge and click on convert entities:
Go to Surfaces tab and find Curves / Helix and Spiral:
Select the helix and under Defined By choose Height and Pitch. For parameters, select Variable Pitch. For Region Parameters, enter values as on the screenshot, select Reverse Direction. Start Angle: 0 degrees, set Clockwise:
Now we have our helix.
On the Sketch tab, select Right Plane and open new sketch. Select Normal To View:
Zoom in. Draw 3 lines to form a triangle, and set horizontal relation:
Make the two sides of the triangle equal by selecting them and pressing the equal sign from the pop-up. Then use Smart Measurement to set the angle to 59 degrees and set the heigh of the triangle to 1.732:
In the toolbar at the top, find Point and use it to set point at the center of the triangle. Then select this point and the previously created helix and click Pierce Relation from the Add Relations dialog:
Draw a center line on the bolt, add another point to the triangle, as shown on the screenshot, and use Smart Dimension to set the measurement to 4.513:
Draw a circle inside the triangle, and make it coincident to the two sides by creating tangent relations:
Click Trim Entities at the top and select lines to trim to get the following figure:
Set dimensions as on the screenshot:
Make the dots on the side lines coincident with the lines themselves:
Now our sketch is fully defined.
Exit sketch and go to the Features tab, then select Sweep Cut at the top.
Under Profile and Path, set the first entry to the figure we’ve just drawn (Sketch5) and the second entry to our helix:
Select OK — and this is our bolt:
Save this part.
Part 2. The nut.
Now let’s draw a nut.
Select New Document, then Part, OK.
Select Top Plane and open the sketch:
Click on polygon tool, find 0 and draw a polygon:
Smart dimension it and add relations:
Go to isometric view and exit sketch.
Extrude Boss/Base, type 8 mm:
Open sketch on this face:
Click Normal To View. Then draw a circle, add relations, tangent:
Exit sketch, select Extrude Cut, set Flip Side To Cut and Draft On, 60 degrees:
Do the same thing on the other side:
Now let’s make a hole.
Select this face and open sketch:
Select circle, smart dimension it to 8.5mm:
Go to isometric view and exit sketch. Then click on Extrude Cut and for End Condition select Through All.
Now we need to add some chamfers. Select chamfer command, type in 1mm, 45deg, then select the two edges of the hole:
Our nut is almost complete now.
Go to File / Save As and type in Nut.
In a new window, open the previously saved bolt. Go to Insert menu and select Part. In the part selection dialog select Nut:
Now we can see the nut.
Check that the Launch move dialogue is selected:
Shift the nut by -35mm:
Now we have the assembly of our bolt and nut. But we don’t have our thread on our nut yet…
Click Mold Tools and select Combine. Set operation type to Subtract, for Main Body select the nut and for Bodies to Subtract select the bolt:
Here’s our thread:
Go to File / Save As and type Nut1.
Part 3. Animation.
Now we’re going to make an animation.
Go to New and open Assembly:
Click Browse, open the Bolt document. Then go to Insert Component and select the Nut:
Click on Mate, under Standard Mates choose Concentric and select the two threads:
Click and hold the nut to move it along the bolt.
Under Mates, go to Mechanical Mates, select Screw and for Distance/Revolution type in 2mm:
Right-click the bolt as shown on the screenshot and select Hide:
Select the thread of the nut, then go to the tree, right-click the Bolt and select Show:
Then select the thread of the bolt and under Mates / Mechanical Mates / Screw set the Distance/Revolution to 2mm:
Now when you click and hold one of the sides of the nut, you’ll be able to spin it and move it along the thread:
Click the Evaluate tab and select Interference Detection. Click Calculate… And we have some interference:
Click the Ignore button, go to File menu and save the Assembly.
Go to Motion Study:
Right-click Orientation Camera Views and select Disable Playback of View Keys:
Click the Motor icon:
Under Motor Type, select Linear Motor.
For Motor Location, select a side of the nut:
For Component to Move / Relative To, select the bolt:
Under Motion chose Constant Speed and set the animation speed to 1mm per second.
Set the duration to 10 seconds by dragging the slider on the time scale and the Calculate icon:
…And that’s all for this lesson. Enjoy!