Bolt and nut tutorial

Screen Shot 2016-03-09 at 7.46.38 PM

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:
Screen Shot 2016-03-09 at 7.49.03 PM

In the feature manager design tree, select top plane and open sketch:
Screen Shot 2016-03-09 at 7.52.02 PM

Select Polygon and locate the zero point:
Screen Shot 2016-03-09 at 7.55.22 PM

Make a drawing:
Screen Shot 2016-03-09 at 7.57.11 PM

Use Smart Dimension to set the size to 18.6 millimeters.
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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:
Screen Shot 2016-03-09 at 8.31.42 PM

Exit the sketch, select Extrude Boss/Base from the command manager. For the depth, type 7mm and select OK:
Screen Shot 2016-03-09 at 8.35.05 PM

Select this base and open a new sketch:
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Click on Normal To View and draw a circle:
Screen Shot 2016-03-10 at 8.30.18 PM

Add relation, tangent:
Screen Shot 2016-03-10 at 8.32.22 PM

Click on isometric view. Exit sketch.

Go to Extrude Cut. Set Flip side to cut and Draft On, type 60 degrees.
Screen Shot 2016-03-10 at 8.34.27 PM

On the opposite face open a new sketch. Select Normal To View and draw a circle. Smart dimension it to 10mm:
Screen Shot 2016-03-10 at 8.38.58 PM

Select isometric view and exit sketch, then select Extrude Boss Base, type 45 mm:
Screen Shot 2016-03-10 at 8.41.05 PM

Now we need some fillet. Select fillet command and set its size to 1mm:
Screen Shot 2016-03-10 at 8.43.46 PM

Also, we need to add some chamfer. Select chamfer, also 1mm, 45deg and select this sketch:
Screen Shot 2016-03-10 at 8.45.52 PM

Go to isometric view.

Now create helix. Select this face and open sketch:
Screen Shot 2016-03-10 at 8.47.52 PM

Select this edge and click on convert entities:
Screen Shot 2016-03-10 at 8.49.38 PM

Go to Surfaces tab and find Curves / Helix and Spiral:
Screen Shot 2016-03-10 at 8.54.51 PM

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:
Screen Shot 2016-03-10 at 8.59.25 PM

Select OK.
Now we have our helix.

On the Sketch tab, select Right Plane and open new sketch. Select Normal To View:
Screen Shot 2016-03-10 at 9.02.09 PM

Zoom in. Draw 3 lines to form a triangle, and set horizontal relation:
Screen Shot 2016-03-10 at 9.05.22 PM

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:
Screen Shot 2016-03-10 at 10.53.28 PM

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:
Screen Shot 2016-03-10 at 10.57.06 PM

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:
Screen Shot 2016-03-10 at 11.01.31 PM

Draw a circle inside the triangle, and make it coincident to the two sides by creating tangent relations:
Screen Shot 2016-03-10 at 11.05.29 PM

Click Trim Entities at the top and select lines to trim to get the following figure:
Screen Shot 2016-03-10 at 11.07.51 PM

Set dimensions as on the screenshot:
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Make the dots on the side lines coincident with the lines themselves:
Screen Shot 2016-03-10 at 11.12.53 PM

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:
Screen Shot 2016-03-10 at 11.19.41 PM

Select OK — and this is our bolt:
Screen Shot 2016-03-10 at 11.21.38 PM

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:
Screen Shot 2016-03-15 at 3.58.47 PM

Click on polygon tool, find 0 and draw a polygon:
Screen Shot 2016-03-15 at 4.01.07 PM

Smart dimension it and add relations:
Screen Shot 2016-03-15 at 4.03.07 PM

Go to isometric view and exit sketch.

Extrude Boss/Base, type 8 mm:
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Open sketch on this face:
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Click Normal To View. Then draw a circle, add relations, tangent:
Screen Shot 2016-03-15 at 4.10.16 PM

Exit sketch, select Extrude Cut, set Flip Side To Cut and Draft On, 60 degrees:
Screen Shot 2016-03-15 at 4.11.38 PM

Do the same thing on the other side:
Screen Shot 2016-03-15 at 4.15.13 PM

Now let’s make a hole.

Select this face and open sketch:
Screen Shot 2016-03-15 at 5.09.14 PM

Select circle, smart dimension it to 8.5mm:
Screen Shot 2016-03-15 at 5.11.13 PM

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:
Screen Shot 2016-03-15 at 5.17.08 PM

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:
Screen Shot 2016-03-15 at 5.22.49 PM

Now we can see the nut.

Check that the Launch move dialogue is selected:
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Shift the nut by -35mm:
Screen Shot 2016-03-15 at 5.25.35 PM

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:
Screen Shot 2016-03-15 at 5.27.32 PM

Here’s our thread:
Screen Shot 2016-03-15 at 5.31.01 PM

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:
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Click Browse, open the Bolt document. Then go to Insert Component and select the Nut:
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Click on Mate, under Standard Mates choose Concentric and select the two threads:
Screen Shot 2016-03-15 at 5.38.25 PM

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:
Screen Shot 2016-03-15 at 5.43.26 PM

Right-click the bolt as shown on the screenshot and select Hide:
Screen Shot 2016-03-15 at 5.44.23 PM

Select the thread of the nut, then go to the tree, right-click the Bolt and select Show:
Screen Shot 2016-03-15 at 5.50.20 PM

Then select the thread of the bolt and under Mates / Mechanical Mates / Screw set the Distance/Revolution to 2mm:
Screen Shot 2016-03-15 at 5.55.29 PM

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:
Screen Shot 2016-03-15 at 5.58.19 PM

Click the Evaluate tab and select Interference Detection. Click Calculate… And we have some interference:
Screen Shot 2016-03-15 at 6.00.59 PM

Click the Ignore button, go to File menu and save the Assembly.

Go to Motion Study:
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Right-click Orientation Camera Views and select Disable Playback of View Keys:
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Click the Motor icon:
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Under Motor Type, select Linear Motor.

For Motor Location, select a side of the nut:
Screen Shot 2016-03-15 at 6.08.32 PM

For Component to Move / Relative To, select the bolt:
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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:
Screen Shot 2016-03-15 at 6.14.21 PM

…And that’s all for this lesson. Enjoy!