Inventor Self-paced ecourse Autodesk Inventor Module 8 Coils and Threads Advanced Learning Outcomes When you have completed this module, you will be able to: 1 Describe a coil and a thread. 2 Apply the COIL command to create coils. 3 Apply the COIL and SPLIT commands to create real life threads either cut into or added onto the part. Coils and Threads Coils or springs and threads are created using the COIL command. Coils Coils or sometimes called springs are constructed by drawing a profile and then rotating it around at an axis or centerline. See Figure 8-1. You can specify the shape of the spring by altering the profile, center diameter, pitch, revolution and height. If you specify the pitch and the number of revolutions, Inventor will calculate the height. If you specify the pitch and the height, Inventor will calculate the number of revolutions. Figure 8-2 External Threads Threads Threads that are created using the Figure 8-1 THREAD command (see Module 19 of the Coil or Spring Inventor Modules) are not actual threads constructed on the solid model. They are simply a graphical representation of the threads. The COIL command creates actual real life threads. This is done by drawing the thread profile (the profile shape of one thread) and then rotating it around the center line of the cylinder. See Figure 8-2. You control thread construction by specifying the pitch, revolution and, height. If you enter the number of revolutions instead of the height, the COIL command will calculate the height. To draw the profile of one thread, it is best to draw it on a work plane that you create through the center of the cylinder. Internal threads can also be created as shown in Figure 8-3. Figure 8-3 Internal Threads
8-2 Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 Drafting Lesson Springs and Threads Study the Figure 8-4 shown below to learn the terms used when drawing springs and threads. Pitch is an important term that you must understand and is required when using the COIL command. Figure 8-4 Threads and Spring Shape and Terminology The threads created by the THREAD command are not actual threads constructed on the solid model. They are simply a graphical representation of the threads. A real life solid model created from the Inventor part file would not be threaded. To create real life threads on your model, you must use the COIL command to either add material onto the part in the shape of the thread or remove the material in the shape of the thread.
Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 8-3 Inventor Command: COIL The COIL command is used to create a spring or thread by rotating a profile around a center line. Shortcut: None Inventor Command: SPLIT The SPLIT command is used to split a solid model into two parts or slice off a portion of a solid model. Shortcut: None
8-4 Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 Creating a Spring Step 1 Using the NEW command, start a new part using the template: English-Modules Part (In).ipt. Step 2 Save and name the part: Inventor Advanced Workalong 08-1. (Figure Step 2A and 2B) Figure Step 2A Figure Step 2B The Completed Spring Step 3 Draw the Base sketch on the Front view (XZ Plane) and project the Center Point onto it. Step 4 Draw a centerline of any length starting at X0Y0Z0. (Figure Step 4) Figure Step 4
Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 8-5 Step 5 Draw a circle for the profile of the spring wire with its center located along the X axis. Dimension the circle diameter and the spring diameter. (Figure Step 5) Figure Step 5 Step 6 Enter the COIL command. The Coil dialogue box will automatically select the circle as the shape since it is the only profile in the current sketch. (Figure Step 6) Figure Step 6
8-6 Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 Step 7 Enable the Axis icon and select the centerline. (Figure Step 7) Figure Step 7 Step 8 Enable the Solid icon in the Output box. Step 9 Enable the Rotation Direction icon. Step 10 In the Coil Size tab, fill it in as shown in the figure. Click OK. (Figure Step 10A and 10B) Figure Step 10A Step 11 Save and close the part. Figure Step 10B
Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 8-7 Creating A Square Thread Step 1 Using the NEW command, start a new part using the template: English-Modules Part (In).ipt. Step 2 Save and name the part: Inventor Advanced Workalong 08-2. (Figure Step 2A and 2B) Figure Step 2A Completed Solid Model Figure Step 2B Multiview Drawing Step 3 onto it. Draw the Base sketch on the Right Side view (YZ Plane) and project the Center Point
8-8 Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 Step 4 Draw a circle locating the center at X0Y0Z0 and dimension it. Extrude the circle 5 inches to create the cylinder. (Figure Step 4A and 4B) Figure Step 4A Figure Step 4B Author's Comments: You will see later in the workalong why I extruded the cylinder 5 inches instead of 4 inches. Step 5 Create a work axis along the centerline of the cylinder. Start a new sketch on the end of the cylinder and draw a construction line along the center line. (Figure Step 5) Figure Step 5
Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 8-9 Step 6 Create a work plane through the center of the cylinder using the construction line and the work axis you created in Step 5. (Figure Step 6) Figure Step 6 Step 7 Start as new sketch on the work plane and then press F7 to slice the graphics. (Figure Step 7) Figure Step 7
8-10 Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 Step 8 On the sketch, draw four lines to form a rectangle along the top of the cylinder. The bottom right corner must be on the edge of the cylinder. (Figure Step 8) Figure Step 8 Step 9 Add a Fix constraint to the bottom and right lines. (Figure Step 9) Figure Step 9 Step 10 Dimension the lines as shown in the figure. Your square thread is a 0.125 inch square as shown in the multiview drawing on page 8-6. (Figure Step 10) Figure Step 10
Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 8-11 Step 11 Enter the COIL command and with the Profile icon enabled in the Shape box select the square sketch. Set all other items in the Coil Shape tab as shown in the figure. (Figure Step 11) Figure Step 11 Step 12 In the Coil Size tab, set it as shown in the figure. (Figure Step 12) Figure Step 12
8-12 Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 Step 13 Disable the Visibility of the sketch and the work plane that you created in Steps 5 and 6. (Figure Step 13) Author's Comments: If you disable the visibility of unconsumed sketches and work features as you finish using them, you will find it easier to continue model construction without obstructions. Step 14 Create a new work plane on the end of the cylinder and offset it -0.125 inches. (Figure Step 14) Figure Step 13 Figure Step 14 Step 15 Enter the SPLIT command. In the Split dialogue box, enable the Remove icon in the Method box, the appropriate Remove Direction icon and select the work plane as the Split Tool. (Figure Step 15A, 15B, and 15C) Figure Step 15A
Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 8-13 Figure Step 15B Step 16 Create another work plane offsetting it 4 inches from the end of the threaded shaft. (Figure Step 16) Figure Step 15C Author's Comments: The next step to creating a thread is to cut it off so that you get the correct length of thread. That is why cylinder was extruded longer then 4 inches in Step 4. Figure Step 16
8-14 Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 Step 17 Using the SPLIT command, remove the other end of the threaded shaft. (Figure Step 17) Step 18 Add the ends of the model by creating new sketches and extruding the cylinders. Add the fillets and chamfer. (Figure Step 18A and 18B) Figure Step 17 Figure Step 18A Figure Step 18B Step 19 Change the color to Chrome Polished and the color property of the end cylinder face to Metal-Steel (Knurled). (Figure Step 19) Figure Step 19 Step 20 Save and close the part.
Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 8-15 Creating A Screw Thread Step 1 Using the NEW command, start a new part using the template: English-Modules Part (In).ipt. Step 2 Save and name the part: Inventor Advanced Workalong 08-3. Step 3 Draw the Base sketch on the Top view (XY Plane) and project the Center Point onto it. Step 4 Using the multiview drawing, draw the bolt to the point shown in the figure. Extrude the cylinder 2.50 inches. (Figure Step 4A and 4B) Figure Step 4A Dimensioned Multiview Drawing Figure Step 4B
8-16 Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 Step 5 Create a work plane along the center of the model. (Figure Step 5) Step 6 The figure shows the dimension and shape of the screw thread that you will be creating in this workalong. (Figure Step 6) Figure Step 5 Figure Step 6 Step 7 Create a new sketch on the work plane and then using the commands LOOK AT/VIEW FACE and SLICE GRAPHICS, change the model to appear as shown in the figure. (Figure Step 7) Figure Step 7
Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 8-17 Step 8 Draw one construction line along the top of the cylinder and another along the end. The length of the lines is not important. (Figure Step 8) Step 9 Draw an inclined line from the intersection of the two construction lines and then a horizontal line. (Figure Step 9) Figure Step 9 Figure Step 8 Step 10 Dimension the lines as shown in the figure. See Figure Step 6 for the dimension used in this figure. (Figure Step 10) Figure Step 10
8-18 Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 Step 11 Draw a vertical line from the midpoint of the horizontal line at any length. (Figure Step 11) Figure Step 11 Step 12 Using the MIRROR command, mirror the inclined line to complete the opposite side. (Figure Step 12) Figure Step 12 Step 13 Add a line across the top of the V thread profile to complete the profile. (Figure Step 13) Figure Step 13
Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 8-19 Step 14 Finish the sketch and enter the COIL command. In the Coil dialogue box, set the items in the Coil Shape tab to match the figure. (Figure Step 14) Figure Step 14 Step 15 Set the items in the Coil Shape tab to match the figure. (Figure Step 15) Figure Step 15
8-20 Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 Step 16 Create a work plane on the end of the bolt and offset it -0.0625 units. (Figure Step 16) Figure Step 16 Step 17 Enter the SLICE command and slice off the bolt using the work plane as the cut plane. (Figure Step 17) Figure Step 17
Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 8-21 Step 18 Start a new sketch on the work plane and then draw circle the diameter of the bolt. (Figure Step 18) Figure Step 18 Step 19 Extrude the circle to add 0.0625 inches onto the end of the bolt. (Figure Step 19) Figure Step 19
8-22 Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 Step 20 Using the CHAMFER command, chamfer the end of the bolt using 0.0625 as the distance. (Figure Step 20) Figure Step 20 Step 21 Change the color to Copper - Polished. (Figure Step 21) Figure Step 21 Step 22 Save and close the part. The Key Principles in Module 8 1 Coils or springs are constructed by drawing a profile and then rotating it around at an axis or centerline. 2 Threads that are created using the THREAD command (see Module 19 of the Inventor Modules) are not actual threads constructed on the solid model. They are simply a graphical representation of the threads. 3 The COIL command creates actual real life threads. This is done by drawing the thread profile (the profile shape of one thread). It is then rotated around the center line of the cylinder.
Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 8-23 Lab Exercise 8-1 Time Allowed: 3 Hrs Name: Inventor Advanced Lab 08-1 Project: Inventor Advanced Course Units: Inches Template: See below Color: See below Material: N/A Step 1 Create the following parts. Each part must have its own file. In each part, ensure you do the following: A Project the Center Point onto the Base plane. B Select your own location of X0Y0Z0. C Draw the necessary sketches and extrude or revolve them to produce the solid model shown. Apply all of the necessary geometrical and dimensional constraints to maintain the objects shape and size. D Apply the color and material shown. E Ensure you draw each part in the correct orientation so that they can be assembled together. Figure Step 1A Thread Details Part: Bolt Part Name: Inventor Advanced Lab 08-1A Template: English-Modules Part (in).ipt Color: Steel Polished (Figure Step 1A, 1B, and 1C) Figure Step 1B Dimensioned Multiview Drawing Figure Step 1C Completed Part - Home View
8-24 Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 Part: Nut Part Name: Inventor Advanced Lab 08-1B Template: English-Modules Part (in).ipt Color: Steel Polished (Figure Step 1D and 1E) Figure Step 1D Completed Part - Home View Figure Step 1E Dimensioned Multiview Drawing Author's Comments: Extrude the nut 0.67955 inches. Split 0.07955 off the end. Part: Washer Part Name: Inventor Advanced Lab 08-1C Template: English-Modules Part (in).ipt Color: Semi-Polished (Figure Step 1F and 1G) Figure Step 1F Completed Part - Home View Figure Step 1G Dimensioned Multiview Drawing
Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 8-25 Part: Spring Part Name: Inventor Advanced Lab 08-1D Template: English-Modules Part (in).ipt Color: Light Gray (Figure Step 1H and 1J) Figure Step 1H Coil Specifications Pitch - 0.250 inches 6 Revolutions Figure Step 1J Solid Model - Home View
8-26 Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 Part: Lock Washer Part Name: Inventor Advanced Lab 08-1E Template: English-Modules Part (in).ipt Color: Smooth Off-White (Figure Step 1K, 1L, and 1M) Figure Step 1K Coil Hint Figure Step 1L Solid Model - Home View Figure Step 1M Solid Model - Orbited View Author's Comments: Create a 0.995 revolution. A full revolution will cause an error.
Inventor Self-paced ecourse - Autodesk Inventor Advanced - Revised 2015-06-01 8-27 Assembly Name: Inventor Advanced Lab 08-1 Template: English-Modules Assembly (in).iam (Figure Step 2A and 2B) Step 2 Assemble the parts that you created in Step 1 to create the assembly shown in figures below. There are two washers. Save the assembly using the name shown above. Figure Step 2A Assembly - Home View Figure Step 2B Assembly - Orbited View