Chain-Inventor Studio (Upgraded Design) - Autodesk Inventor 2013

Serial No. 220

Chain-Inventor Studio (Upgraded Design) - Autodesk Inventor 2013

This video displays a setting up of 70 chain links and 3 sprockets along a defined paths in Autodesk Inventor’s  Assembly modelling environment.  First of all some base sketching afterward some advance pattern, adaptive features and assembly mates are to be applied to set up an animation matching the real world scenario… Later the whole mechanism consisting of required mates are driven by using Inventor Studio functionality of the software……

 

Click the following link to get the model file: -http://bit.ly/2nIJIRH

Handle of Tack Hammer-Autodesk Inventor 2013 (with caption and audio narration)

Serial No. 209

Handle of Tack Hammer-Autodesk Inventor 2013 (with caption and audio narration)

Here we focused on the design of handle of Tack Hammer (also called Upholstery Hammer), since the design of hammer has already being discussed in our previous video named ‘Hammer’, so it is not described here.

 

Click the following link to get the model file: - http://bit.ly/2nMONbS

Transcription of Video

1. Open the Assembly file of ‘Hammer’.

2. A pre-constructed Part1 file is placed in this assembly.

3. Create a new component with an English template by using Create Component tool.

4. And change the name of file Part2.

5. Select the back face of the model as a base plane for creating a new component.

6. Create a new sketch on this face.

7. Turn off the transparency, so we can see the Part1 more clearly.

8. Use the Project Cut Edges command to get the model edges.

9. Convert all the projected lines into the construction except to this rectangle.

10. Create a base sketch of handle with the given dimensions by utilizing line, circle and arc tool.

11. Now the sketch is complete, exit from the sketching environment.

12. Activate the Extrude command.

13. Select the each individual profiles.

14. Set the value in the distance field.

15. Click OK to execute the command.

16. Close the visibility of Part1 and Work Plane1 to see the Part2 (handle) more clearly.

17. Change the colour of model to ‘Birch – Solid Stained Light No Gloss’.

18. Open visibility of Sketch1 in the Extrusion1 feature.

19. Create a new sketch over the front face of Part2 to create a wedge on the handle.

20. Take a project of the rectangle by using Project Geometry tool.

21. Finish the 2D sketch.

22. Close the visibility of Sketch1 in the browser bar.

23. Activate the extrude command once again.

24. Fill the value in the distance field and execute the command.

25. Return back to the assembly environment.

26. Open the visibility of Part1 to complete the assembly.

27. Check the interface between Part1 and Part2.

28. Save the Hammer assembly.

Tub-Rectangular through Sheet Metal-Autodesk Inventor 2013 (with caption and audio narration)

Serial No. 186

Tub-Rectangular through Sheet Metal-Autodesk Inventor 2013 (with caption and audio narration)

In this  video we will create a rectangular tub using sheet metal features (Face tool and Flange tool).

 

 

Click the following link to get the model file: - http://bit.ly/2ofTr23

 

 

 Transcription of Video

1. Create a new Sheet Metal (in).ipt part file.
2. Go on the ribbon > Setup panel > click Sheet Metal Defaults icon.
3. The Sheet Metal Defaults dialogue box will be opened in the graphics window.
4. Uncheck the ‘Use Thickness from Rule’ option to specify the thickness value 1/16 inch manually.
5. Create a new sketch on the XY Plane.
6. Draw a rectangle of dimension 32 ¼ inch x 27 inch with the help of ‘Three Point Centre Rectangle’ tool.
7. Exit from the sketching environment.
8. Activate the ‘Face’ tool from the marking menu.
9. The sketch profile will be automatically selected.
10. Click OK to apply face feature.
11. Save the file with the name 'Tub (Rectangular)'.
12. Change the colour of the model to ‘Flaked Reflective – Beige’.
13. Activate the ‘Flange’ tool from the marking menu.
14. On the Shape tab, click the ‘Loop Select Mode’ and click the bottom edge of the part.
15. A preview of flange is visible in the graphics window.
16. Click the Flip Direction button in the Height Extents field.
17. And set the height extents value to 6 3/16 inch.
18. Click OK to create the new flanges.
19. Activate the ‘Flange’ tool once again.
20. And select the four outer edges of the part.
21. Fill the value 1 1/16 inch in the height extents field.
22. Switch to the Corner tab, ‘Apply Auto-Mitering’ option is checked by default.
23. Uncheck the Auto Mitering option to see the effect.
24. Click OK to create the new flanges.
25. Go on the ribbon > Flat Pattern panel > click Create Flat Pattern icon to generate the flat pattern of the model.
26. Double-click the ‘Folded Model’ icon at the top of the Model browser to return to the folded model.

Application of ‘Text’ tool and ‘Emboss’ tool-Autodesk Inventor 2013 (with caption and audio narration)

Serial No. 192

Application of ‘Text’ tool and ‘Emboss’ tool-Autodesk Inventor 2013 (with caption and audio narration)

In this exercise a pre constructed part file ‘Anvil’ is used.

 

Click the following link to get the model file: - http://bit.ly/2nJyMTG

 

 

 Transcription of Video

1. Open the Anvil (.ipt) file.
2. At present a pre constructed part file of ‘Anvil’ is visible in the isometric view.
3. Create a new sketch on the blue face of the Anvil with the help of ‘Create 2D Sketch’ tool.
4. Take the project of the model by using ‘Project Cut Edges’ tool.
5. Select the projected model edges in the design window and convert them into construction geometry.
6. Start the ‘Text’ tool from the Draw panel of the Sketch tab.
7. In the graphics window, click to place the insertion point for the text box and drag to define the area of the text box.
8. Format Text dialogue box is visible in the graphics window.
9. In the ‘Format Text’ dialogue box, enter the text ANVIL in the specified area.
10. Select text and choose Center Justification and Middle Justification in the ‘Style’ option.
11. Enter the value 0.8 in the ‘Size’ field.
12. Change the text colour to Red.
13. In the ‘Font’ field, select ‘Calibri’ font from the drop down list.
14. Click OK to place the Text.
15. Right click in the graphics window and click OK to finish the command.
16. Apply Vertical constraint and Coincident constraint on the text to position it properly.
17. Finish the 2D sketch.
18. Activate the ‘Emboss’ tool from the Create panel of the 3D Model tab.
19. Emboss dialogue box is visible in the design window.
20. The profile selection is activated by default.
21. Select text as profile.
22. In the ‘Depth’ field enter the value 0.25 inch.
23. Change the direction of the feature by clicking the flip direction button.
24. Click OK to execute the Emboss feature.
25. Select the Emboss feature in the browser bar and activate the ‘Adjust’ tool from the ‘Quick Access Tool Bar’.
26. Adjust the appearance tinting of the feature and click OK to apply.

Can (Autodesk Inventor 2013)

Serial No. 185

Can (Autodesk Inventor 2013)

 

Click the following link to get the model file: - http://bit.ly/2mPuGJP

Application of ‘Extrude’ tool (Join operation) Autodesk Inventor 2013 (with caption and audio narration)

Serial No. 191

Application of ‘Extrude’ tool (Join operation) Autodesk Inventor 2013 (with caption and audio narration)

 

  

Click the following link to get the model file: - http://bit.ly/2omKELY

 

 

Transcription of Video

1. Open the Part1 file.
2. A pre constructed sketch1 is visible in the design window.
3. Double click the Sketch1 in the browser bar.
4. Take the Offset of sketch, of the value 1/4 inch inside the enclosed profile.
5. Activate the extrude command from the marking menu.
6. Extrude dialogue box is visible in the design window.
7. The Profile selection button is active by default.
8. Select the profile enclosed by the yellow sketch and enter the distance value 3/8 inch.
9. Click OK to apply the extrude feature.
10. Open the visibility of Sketch1.
11. Activate the Extrude command once again from the Create panel.
12. Select the profile enclosed by the yellow lines and extrude it 1 inch in upward direction.

Creating a Realistic Thread (Autodesk Inventor 2013)

Video Tutorial with caption and audio narration

 

The Screw file displayed in the video is taken from our model ‘Knob of Switch’.

First of all get the model files required to complete this tutorial by visiting the following link:- http://bit.ly/32leYVx 


 

 

 

Transcription of Video

1. Open the part file of Screw.
2. Select the 'Thread' tool in the Modify panel of 3D Model tab.
3. 'Face' selection button is automatically activated in the Thread dialogue box.
4. Select blue cylindrical face of the Screw.
5. Click the Specification tab, here it has automatically detected features/values like 'Thread Type', 'Size', 'Designation', 'Class' and 'Right Hand thread'.
6. If anyone wants to change the properties/features, it can be edited very easily.
7. Click OK to apply the thread feature.
8. Select the 'Thread Modeler' tool in the Thread Modeler panel of Tools tab.
9. Select Thread feature in the Browser Bar.
10. The Thread Modeler tool has automatically detected the pitch of the thread in the Thread Modeler Control dialogue box.
11. Click OK to apply realistic thread on the screw.
.....................................................................................................................................................

Visit Autodesk exchange Apps site on the following link to get  the ‘Thread Modeler Tool’ which is an external application utilized with the software :-

http://apps.exchange.autodesk.com/INVNTOR/de/Detail/Index?id=appstore.exchange.autodesk.com%3Athreadmodeler_windows32and64%3Aen

Knob of Switch-Autodesk Inventor 2013 (with caption and audio narration)

 

Serial No. 184

Knob of Switch-Autodesk Inventor 2013 (with caption and audio narration)

 

Click the following link to get the model file: - http://bit.ly/2nI2Q2o

 

 

 Transcription of Video

Modelling a ‘Knob of Switch’ (Autodesk Inventor 2013)

1. Open a New Standard (in).ipt file.
2. Create a new 2D sketch on the XY Plane.
3. Draw a circle of 1 ¾ inch diameter, coincident with the auto projected part origin.
4. Click Finish 2D Sketch command from the marking menu to exit the sketching mode.
5. Activate the ‘Extrude’ Command.
6. It will automatically select the circle as profile.
7. Enter the extrusion value ¼ inches and click OK.
8. Change the colour of the model to ‘Flaked Reflective – Beige’.
9. Save the file with the name ‘Knob of Switch’.
10. Change the view of the model by using View Cube.
11. Set the view as Home View by clicking the toggle next to View Cube.
12. Start a new sketch on the top face of the model.
13. Take the project of circular edge and Y Axis.
14. Convert this vertical line and circle into construction geometry.
15. Draw an arc over the projected edge of the model with the help of Centre Point Arc tool.
16. Apply a Coincident Constraint between mid-point of Arc and projected Y Axis line.
17. Give a linear dimension 1/4 inch between both the end points of the arc.
18. In the same way, draw another centre point arc as displayed.
19. Apply a Coincident Constraint between mid-point of arc and Y Axis.
20. Give a linear dimension 1/2 inch between both the end points of the arc.
21. Finish the sketch.
22. Create a new Work Axis on the one end of the arc, parallel to Z Axis of the model.
23. Create a new Work Point at the intersection of Work Axis 1 and bottom circular edge of the model.
24. Create a new work plane by using Three Point work plane tool.
25. Close the visibility of Work Point1 and Work Plane1.
26. Start a new sketch on this work plane.
27. Take the project of the model by using Projected Cut Edges tool.
28. Draw two vertical lines on both the end points of the top projected edge of the model.
29. And apply dimension 1 inch on these two lines.
30. Close the profile by using line tool.
31. Convert the sketches into construction geometry which are presently not in use.
32. Exit from the sketching environment.
33. Create another Work Axis on the second end point of the arc, parallel to Z Axis of the model.
34. Create another Work Point at the intersection of Work Axis 2 and bottom circular edge of the model.
35. Create a new work plane by using Three Points work plane tool.
36. Start a new sketch on this work plane.
37. Take the project of the model by using Projected Cut Edges tool.
38. Draw two vertical lines on both the end points of the top edge of the model.
39. And apply dimension 1 inch on these two lines.
40. Close the profile by using line tool.
41. Convert the sketches into construction geometry which are presently not in use.
42. Exit from the sketching environment.
43. Create another 3 Point work plane on the top end points of these lines.
44. Create a new sketch on this work plane.
45. Take the project of both arcs on this work plane.
46. Finish the sketch.
47. Start the Loft tool.
48. First select both the closed sketch profiles in the design window.
49. Then select four arcs as rails.
50. Click OK to create the Loft feature.
51. Create a new sketch on the top face of the model.
52. Take the project of top face of model by using Project Geometry tool.
53. Create a new sketch profile with the help of Offset tool.
54. Affix offset distance 1/32 inch between the lines.
55. Take the offset of upper and lower segment of arc.
56. Affix offset distance 5/16 inch between the arcs.
57. Snap the end points of arcs with the adjacent lines by using coincident constraint tool.
58. Erase the extra lines and arcs with the help of Trim tool.
59. Finish the 2D sketch.
60. Cut the enclosed area (defined by Sketch6) 1/32 inch towards downward direction by using Extrude Command.
61. Pick up the Fillet tool.
62. Select this circular edge of the top face, enter the value 1/4 inch in the Radius input box and click OK.
63. Apply another fillet of value 1/8 inch on the opposite side of the previous circular edge.
64. Rotate the model by using View Cube.
65. Create a new sketch on the bottom face of the model.
66. Take the project of bottom face of the model with the help of Project Geometry tool.
67. Create a new circle with the help of Offset tool.
68. Affix offset distance 1/8 inch between these two circles.
69. Finish the sketch.
70. Cut the enclosed area (defined by Sketch7) 3/16 inch towards downward direction by using Extrude Command.
71. Create a new sketch on the inner circular face of the model.
72. Draw a circle of diameter 5/8 inch and extrude this circle to 1/8 inch.
73. Create a new sketch on the YZ Plane of Knob-Switch.
74. Right click in the design window and select Slice Graphics command.
75. Take the project of Z Axis of the model and outer vertical edge.
76. Select both the vertical lines and change their colour to white.
77. Draw a horizontal line.
78. Place dimension ¼ inch between bottom edge of the model and horizontal line.
79. Select both the vertical lines and convert them into construction geometry.
80. Draw a vertical line of 1/32 inch length over the projected Z Axis of the model.
81. Draw an arc coincident with these two points with the help Three Point Arc tool.
82. Create another horizontal line and apply a tangent constraint between arc and this line.
83. Activate the Revolve tool from the right click context menu.
84. It will automatically select the sketch profile.
85. Click on this line to specify the axis of revolution and click on green checkmark.
86. A smooth oval face is created.
87. Rotate the model on the back side.
88. Create a new sketch on the blue circular face.
89. Draw a circle of diameter 5/16 inch, coincident with the centre point of the model.
90. Finish the sketch.
91. Create a new work plane, 5/8 inch downward from the blue face.
92. Create a new sketch on this new work plane.
93. Draw a circle of diameter 3/16 inch, coincident with the centre point.
94. Finish the sketch.
95. Pick up the Loft tool.
96. Select upper and lower circles in the design window.
97. Click Cut option in the loft dialogue box.
98. Click OK to create the loft feature.
99. Align the model in the desired position by using View Cube.
100. Create a new sketch on the blue circular face.
101. Take a project of inner circle and convert it to construction geometry.
102. Draw a line of length 3/16 inch parallel to X Axis.
103. Snap one end point of line on the circle with the help of coincident constraint tool.
104. Draw an arc between both the end points of the line by using Centre Point Arc tool.
105. Finish the 2D sketch.
106. Create a new sketch on the YZ Plane of the Knob.
107. Right click in the design window and select Slice Graphics command.
108. Take the project of the model by using Projected Cut Edges tool.
109. Select all the sketches and convert them into construction geometry.
110. Draw a line of the length 3/16 inch, along the slant edge of the taper hole.
111. Activate the Sweep tool from the right click context menu.
112. It will automatically select sketch as profile and taper line as path for sweep.
113. Click OK to create the sweep feature.
114. Create a new sketch on the blue circular face.
115. Take the project of the model by using Project Cut Edges command.
116. Right click in the design window and select Slice Graphics command.
117. Draw two vertical lines on the opposite quadrants of the circle.
118. Extrude this enclosed profile 1/32 inch.
119. Create a new sketch once again on the blue circular face.
120. Take project of the model by using Project Cut Edges tool.
121. Take the project of Y Axis of the model by using Project Geometry tool.
122. Select all the sketches and convert them into construction geometry.
123. Activate the Slice Graphics command.
124. Draw a vertical line between Point1 and Point2.
125. And convert this line into construction geometry.
126. Create a rectangle of dimension 3/16 inch x 5/16 inch, on the midpoint of the vertical line with the help of ‘Three Point Centre Rectangle’ tool.
127. Finish the 2D sketch.
128. Open the visibility of Work Plane4.
129. Create a new sketch on this Work Plane.
130. Click Visual Styles icon from the Appearance panel of the View tab.
131. Select Wireframe option.
132. Take the project of centre point of the rectangle.
133. Activate the Slice Graphics command.
134. Draw a Three Point Centre Rectangle of dimension 1/8 inch x 5/24 inch on this point.
135. Finish the 2D sketch.
136. Pick up the Loft tool.
137. Select upper and lower rectangles in the design window.
138. Click Cut option in the loft dialogue box.
139. Click OK to create the loft feature.
140. Create a new sketch on the blue selected face.
141. Take project of the model by using Project Cut Edges tool.
142. Take the project of Y Axis of the model by using Project Geometry tool.
143. Select all the sketches and convert them into construction geometry.
144. Activate the Slice Graphics command.
145. Draw a vertical line between Point1 and Point2.
146. And convert this line into construction geometry.
147. Create a square of side 1/4inch, on the midpoint of the vertical line with the help of ‘Three Point Centre Rectangle’ tool.
148. Finish the sketch.
149. Create a new work plane, 17/32 inch downward from the blue face with the help of ‘Offset from Plane’ tool.
150. Create a new sketch on this work plane.
151. Click Visual Styles icon from the Appearance panel of the View tab.
152. Select Wireframe option.
153. Take the project of centre point of the rectangle.
154. Activate the Slice Graphics command.
155. Draw a square of side 1/6 inch on this point by using ‘Three Point Centre Rectangle’ tool.
156. Finish the 2D sketch.
157. Pick up the Loft tool.
158. Select upper and lower rectangles in the design window.
159. Click Cut option in the loft dialogue box.
160. Click OK to create the loft feature.
161. Create a new work plane on Point1 which is parallel to the XY plane of the model.
162. Create a new work plane tangent to blue face of the model and parallel to XZ Plane with the help of ‘Tangent to Surface and Parallel to Plane’ command.
163. Create a new sketch on this work plane.
164. Take the project of Z Axis of the model and Work Plane7 of the model.
165. And convert them into construction geometry.
166. Draw a circle of diameter 3/16 inch whose centre lies on projected Z axis of the model.
167. Apply a tangent constraint between circle and projected edge of Work Plane7.
168. Finish the 2D sketch.
169. Activate the ‘Extrude’ Command.
170. It will automatically select the circle as profile.
171. Select Cut option to remove the material.
172. In the ‘Extents’ drop down of Extrude dialogue box, select ‘To’ option.
173. Select XZ Plane of the model to specify end of extrude feature.
174. Click OK to create the feature.

Creation of Exploded View of a Model-Autodesk Inventor 2013 (with caption and audio narration)

 Serial No. 125

Creation of Exploded View of a Model-Autodesk Inventor 2013 (with caption and audio narration)

 

  

 

Click the following link to get the model file: - http://bit.ly/2nskR4s

 

 

Transcription of Video

Creation of Exploded View of a Model in a Presentation File (Autodesk Inventor 2013)

1. Create a new Standard (in).ipn Presentation File.
2. Click ‘Create View’ icon in the Create panel of Presentation Tab.
3. In the Select Assembly dialogue box, click ‘Open an existing file’ button under the File section.
4. Select the ‘Vise’ Assembly and Click Open.
5. Explosion Method should be selected to ‘Manual’.
6. Click Ok.
7. Save the file with the default name.
8. Click ‘Tweak Components’ tool on the Create panel.
9. Select front face of Vise to set the Direction.
10. Select Sub Assembly-3 in the Browser Bar as Component.
11. Place the cursor in the empty area of Design window and drag the component in Z direction.
12. Enter the value 40 inch in Tweak Distance input box under the ‘Transformations Section’ to precisely move the component.
13. Click green check mark to apply.
14. Hold the Ctrl key and click the Sub Assembly-3 to remove it from the selection.
15. Select the Sub Assembly-2 in the Browser Bar.
16. Drag the Component 22 inch away in the Z direction.
17. Click Close to finish adding tweaks to the exploded view.
18. Adjust the model in the design window by using Navigation Tools: Zoom and Pan.
19. Set the Current View as Home view by using the toggle next to View Cube.
20. Click the ‘Browser Filters’ icon in the Browser Bar.
21. Select ‘Sequence View’ from the context menu.
22. Double click the Task1.
23. In the Edit Task & Sequences dialog box, select ‘Sequence2’ from drop down menu of Sequences.
24. Click Set Camera button then Apply it.
25. Click Play Forward button to check the Animation Sequence.
26. Click Reset to set the Animation back to the beginning.
27. Now set the camera for the ‘Sequence1’ in the same manner.
28. Adjust the view of the model by using Navigation Tools.
29. Set the Camera and click Apply.
30. Check the Animation Sequence by clicking the Play Forward button.
31. Click Ok to close the Edit Task & Sequences dialogue box.
32. Click Animate Tool on the Create panel.
33. In the Animation dialogue box, fill the value 50 in ‘Interval’ Input box and click Apply.
34. Click ‘Play Forward’ button to see the animation.
35. Click Reset button and close the dialogue box.
36. Now Zoom the window so that Sub Assembly-1 can be seen clearly.
37. Activate Tweak Component Tool.
38. Select Front Face of Sub Assembly-1 to set the Direction.
39. Select both the Screws as component and drag them 4 inch away in Z direction.
40. Hold the Ctrl key and click both the screws to remove them from the selection.
41. Select the Jaw Plate and drag it 2 inch away in the Z direction.
42. Click Clear button, it will clear the settings in the dialog box.
43. Now it is ready to setup for another tweak.
44. Click the cylindrical face of Screw to set the direction, select Screw again.
45. Change the Transformation type from Linear to Rotational by clicking the Rotational Radio Button.
46. Enter the Transformation value (-720) degree and click the green check mark.
47. Click Clear Button.
48. In the same manner create another Tweak for the second screw.
49. Select cylindrical face of screw then click the screw.
50. Enter the Transformation Value (-720) degree and click green check mark to apply.
51. Close the Tweak Component dialogue box.
52. Expand the Sequence1, 2, 3 and 4 in the Browser Bar to show the Hidden folders.
53. Select the Sub Assembly-2 and Sub Assembly-3, drag and drop them under all the Hidden Folders visible.
54. By doing so both the Sub-Assemblies will be hidden, during the Animation of Sequence1, 2, 3 and 4.
55. Open the Animate Tool.
56. Click more button to expand the Animation dialogue box.
57. Click Play Forward Button.
58. At present both the Screws are rotating separately.
59. Click Pause Button and Reset the Animation Player.
60. Select Sequence 1 and Sequence 2 from the Animation Sequence list by holding Ctrl Key.
61. Click Group Button to combine two tweaks into Sequence1 and Apply it.
62. Click play button to see the effect.
63. Click Pause Button and Reset the Animation Player.
64. Click the Sequence 1 in the Animation Sequence List and click the Move Down button two times.
65. Now this Sequence will be labeled as Sequence 3.
66. Click Apply.
67. Now play the animation to see the effect.
68. Click Reset Button and close the dialogue box.
69. Double click the Task1 in Browser Bar to open Edit Task & Sequences dialog box.
70. Set the Camera for Sequence 1, 2 and 3 as displayed.
71. Click OK to close the dialogue box.
72. Adjust the design window with the help of navigation tools, so that the Part-1 of Sub Assembly-1 can be seen clearly.
73. To do so, take the help of common navigation tools and Precise View rotation Tool.
74. Activate Tweak Components tool.
75. Select front face of Vise as Direction.
76. Then the select Part-1 as Component.
77. Click Y button in the Linear Transformation type option.
78. Drag the Part-1 (-0.625) inch away.
79. Now select Z button in the Linear Transformation type option to move the ‘Part-1’, 8 inch away in Z direction.
80. Close the Tweak Components dialog box.
81. Double click the Sequence 2 in the Browser Bar to open Edit Task & Sequences dialog box.
82. Set Camera for the Sequence 2 and 1.
83. Close the Edit Task & Sequences dialog box.
84. Expand the elements of Sequence2 and put the Sub Assembly-2 in its Hidden folder by using drag and drop method.
85. Re-Adjust the design window using Navigation tools so that Jaw of Sub Assembly-2 can be seen clearly.
86. Activate the Tweak Component Tool.
87. Select the front face of Sub Assembly-2 as Direction.
88. Select both the Screws as Component.
89. Drag them 4 inch away in Z direction.
90. Hold the Ctrl key and click both the screws to remove them from the selection.
91. Select the Jaw Plate and drag it 2 inch away in the Z direction.
92. Click Clear button, it will clear the settings in the dialog box.
93. Now it is ready to setup for another tweak.
94. Click the cylindrical face of Screw to set the direction then select Screw again.
95. Change the Transformation type from Linear to Rotational by clicking the Rotational Radio Button.
96. Enter the Transformation value (-720) degree and click the green check mark.
97. Click Clear Button.
98. In the same manner create another Tweak for the second screw.
99. Select cylindrical face of screw then click the screw.
100. Enter the Transformation Value (-720) degree and click green check mark to apply.
101. Close the Tweak Component dialogue box.
102. Open the Animate Tool.
103. Click more button to expand the Animate dialogue box.
104. Select Sequence 1 and Sequence 2 from the Animation Sequence list by holding Ctrl Key.
105. Click Group Button to combine two tweaks into Sequence1 and Apply it.
106. Click the Sequence 1 in the Animation Sequence List and click the Move Down button two times.
107. Now this Sequence will be labeled as Sequence 3.
108. Click Apply.
109. Now play the animation to see the effect.
110. Click Pause button and close the dialogue box.
111. Double click the Task1 in Browser Bar.
112. Set the Camera for Sequence 1, 2 and 3 as displayed.
113. Click OK to close the dialogue box.
114. Re-Adjust the design window using Navigation tools, so that the ‘Pin’ of Sub Assembly-3 can be seen clearly.
115. Double Click the Pin of Sub Assembly-3 to activate the Tweak Component tool.
116. Select the top face of Pin to set the direction.
117. Drag the Pin 3.5 inch away in Z direction.
118. Click Clear Button.
119. Select the front face of Washer to set the Direction.
120. Select the Washer and drag it 2.5 inch away in Z direction.
121. Hold the Ctrl Key and click the Washer to remove it from the selection.
122. Now select the Spring and drag it 2 inch away in Z direction.
123. Click Clear button.
124. Select the cylindrical face of the Handle to set the Direction.
125. Select the Handle and drag it (-2.5 inch) away in Z direction.
126. Close the Tweak Component dialogue box.
127. Double click the Task1 in Browser Bar.
128. Set the Camera for Sequence 1, 2, 3 and 4 as displayed.
129. Click OK to close the dialogue box.
130. Go to Home View, to readjust the design window.
131. Activate the Animate tool.
132. Clear the screen by activating the Clean screen command.
133. Click ‘Play Forward’ Button to play the Animation.
134. Click Reset Button to restore the Assembly in Exploded mode.

Cam and Follower-Dynamic Simulation-Autodesk Inventor 2013 (with caption and audio narration)

Serial No. 183

Cam and Follower-Dynamic Simulation-Autodesk Inventor 2013 (with caption and audio narration)
In this video, we will demonstrate how to apply the different type of mates in the assembly environment for creating the Dynamic Simulation of the ‘Cam and Follower’. 

 

Click the following link to get the model file : - http://bit.ly/2maTL1C

 

Transcription of Video

Display of motion in ‘Cam and Follower’ through Dynamic Simulation

1. Click the New icon under the Work tab in the Welcome Screen of Autodesk Inventor Professional 2013.
2. Select Metric Template in the Create New File Dialogue Box.
3. Create a Standard (mm).iam Assembly file.
4. Save it with the name ‘Cam and Follower-Dynamic Simulation’.
5. Select Place component from the marking menu and place the ‘Cam’ in the Assembly.
6. Align the Cam in correct position by using View Cube.
7. Set the current view as Home View by using the toggle next to View Cube.
8. Select the Cam in the design window and remove its ‘Grounded’ position from the context menu.
9. Click the Degrees of Freedom icon in the Visibility Panel of View Tab.
10. At present there are six Degrees of Freedom in Cam and it can be moved in any direction in the Assembly.
11. Apply an Axis Mate between the Z Axis of Assembly and Z Axis of Cam.
12. Apply a Flush Mate between the XY Plane of Assembly and upper most front face (Red coloured) of Cam.
13. Now this time only one ‘Degrees of Freedom’ persist and Cam can be moved only on its Z Axis.
14. Place the ‘Follower’ in the Assembly.
15. Re-orient the Follower against the Cam using Rotate Component Tool.
16. Apply a Flush Mate between the upper most front face (Red coloured) of Cam and face of small pulley (Black coloured) of Follower.
17. Apply a Mate Constraint between YZ Plane of Assembly and YZ Plane of Follower.
18. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab.
19. Click the view Tab and change the View of the model to ‘Shaded with Edges’ in the Visual Style drop down.
20. Activate Insert Joint from the Marking menu.
21. Select ‘Sliding: Cylinder Curve’ from the drop down menu of Insert Joint dialog box.
22. Select the outer edge of Cam in ‘Curve’ selection option and select circular edge of small pulley of Follower in ‘Cylinder’ selection option.
23. Click OK.
24. Select Revolution:1 joint in the Browser under the Standard Joints folder, right click and select Properties from the context menu.
25. Click dof 1 (R) tab and select Edit imposed motion button and check the Enable imposed motion option.
26. Click the arrow to expand the input choices, and click Constant Value.
27. Enter the value 360*2 deg/s and click Ok.
28. In Simulation Player fill the value 400 in the Images field area.
29. Clear the screen by activating the Clean Screen command.
30. Click Run in the Simulation Player to display motion in Cam and Follower.

Pipe Wrench-Dynamic Simulation-Autodesk Inventor 2012 (with caption and audio narration)

Serial No. 182

Pipe Wrench-Dynamic Simulation-Autodesk Inventor 2012 (with caption and audio narration)

In this video, we will demonstrate how to apply the different type of mates in the assembly environment for creating the Dynamic Simulation of the ‘Pipe Wrench’.

 

Click the following link to get the model file: - http://bit.ly/2mT1v8y

 

Transcription of Video

Display of Motion in ‘Pipe Wrench’ through Dynamic Simulation.

1. Create a New ‘Standard (in).iam’ Assembly and save it with the name ‘Pipe Wrench-Dynamic Simulation’.
2. Select Place component from the marking menu and place the ‘Base Frame’ in the Assembly.
3. Re-orient the model in the design window by using View Cube.
4. Set the current view as Home View by using the toggle next to View Cube.
5. Place the ‘Supporting Bracket’ in the Assembly.
6. Apply an Axis Mate between hole on the Base Frame and hole on the Supporting Bracket.
7. Apply a Flush Mate Between XY Plane of Base Frame and XY Plane of Supporting Bracket.
8. Activate Angle Constraint Command first select side face of Base Frame; then select side face of Supporting Bracket and at the last select top face of Supporting Bracket.
9. Enter the value -4.76 degree in the Angle Input Box and click OK.
10. Place the ‘Rivet-1’ in the Assembly.
11. Fix the Rivet-1 in the hole of Supporting Bracket by the use of Insert Mate as displayed.
12. Place the ‘Supporting Strip-1’ in the Assembly.
13. Place the Supporting Strip -1 on the hole of Base Frame with the help of Insert Mate.
14. Apply an Angle Constraint between top face of Supporting Strip -1 and top face of Base Frame.
15. In the Solution Type, select Directed Angle.
16. Place the ‘Rivet-2’ in the Assembly.
17. Fix the Rivet-2 on the hole of Supporting Strip-1 with the help of Insert Mate.
18. Place the ‘Supporting Strip-2’ in the Assembly.
19. Place the Supporting Strip -2 on the hole of Base Frame with the help of Insert Mate.
20. Apply an Angle Constraint between top face of Supporting Strip -2 and top face of Base Frame.
21. In the Solution Type, select Directed Angle.
22. Drag the Rivet-2 from the Browser Bar in the Assembly. This will place a copy of Rivet-2 in the Assembly.
23. Fix the Rivet-2 on the hole of Supporting Strip-2 with the help of Insert Mate.
24. Place the ‘Sliding Frame’ in the Assembly.
25. Apply a Flush Mate between XY Plane of Base Frame and XY Plane of Sliding Frame.
26. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser.
27. Apply a Mate Constraint between X Axis of Sliding Frame and Work Plane 7 of Supporting Bracket.
28. Place the ‘Wheel’ in the Assembly.
29. Apply a Mate Constraint between X Axis of Sliding Frame and Axis of Wheel.
30. Apply a Mate Constraint between Work Plane 5 of Supporting Bracket and Work Plane 1 of Wheel.
31. Apply a Mate Constraint between Jaw of Base Frame and Jaw of Sliding Frame in the Assembly.
32. Select the previous applied ‘Mate: 5’ under the Constraints folder in the Browser Bar, Right click and choose ‘Supress’ from the context menu.
33. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab.
34. Select Insert Joint in the Marking menu.
35. Select ‘Screw’ from the drop down menu of Insert Joint dialog box.
36. In the Insert Joint dialog box, select Circular edge of Sliding Frame in ‘Component 1’ selection option and select Circular edge of Wheel in ‘Component 2’ selection option.
37. Enter the value 0.205 in the ‘Pitch’ input box. Click OK.
38. Select Revolution:2 joint in the Browser under the Standard Joints folder, right click and select Properties from the context menu.
39. Click dof 1 (R) tab and select Edit imposed motion button and check the Enable imposed motion option.
40. Click the arrow to expand the input choices, and click Constant Value.
41. Enter the value (-360/0.205) deg/s and click OK.
42. In Simulation Player, fill the value 1000 in the Images field area.
43. Clear the screen by activating the Clean Screen command.
44. Click Run in the Simulation Player to display motion in Pipe Wrench.

Ashtray (New Design) - Autodesk Inventor 2012

 

Serial No. 179

Ashtray (New Design) - Autodesk Inventor 2012

 

Click the following link to get the model file: - http://bit.ly/2nEbXAW

Bibcock (Autodesk Inventor 2013)

Serial No. 176

Bibcock (Autodesk Inventor 2013)

 

Click the following link to get the model file: - http://bit.ly/2nzQI3f

Inspection Cover for Sewage System (Autodesk Inventor 2012)

Serial No. 175

Inspection Cover for Sewage System (Autodesk Inventor 2012)

 

Click the following link to get the model file and drawing sheet: - http://bit.ly/2ohdvRG

iLogic Basic (Autodesk Inventor Video Tutorial)

 

iLogic enables rules-driven design, providing a simple way to capture and reuse your work. Use iLogic to standardize and automate design processes and configure your virtual products.


This tutorial covers the following topics of iLogic:
Work with Parameters
■ Create numeric, true/false, and text parameters.
■ Create multi-value parameters.
■ Use Key parameters as search filters.
■ Modify parameters.
Work with Rules
■ Create rules.
■ Construct conditional statements.
■ Activate and deactivate features.
■ Control part dimensions using a rule.
■ Modify an existing rule.
To get files used in the video visit the following links :--
bracket_no_rule.ipt-----http://a360.co/1beup3k

bracke.ipt---------------- http://a360.co/1beum7n