Tuesday, May 27, 2014

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

Handle of Tack Hammer

Tack Hammer

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.

 

download-Link



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.

Sunday, May 25, 2014

Door (Panel with Frame) modified design--Autodesk Inventor 2013 (with caption)

Door (Panel with Frame) Modified Design_1

Door (Panel with Frame) Modified Design_2

Serial No. 208

Door (Panel with Frame) modified design--Autodesk Inventor 2013 (with caption)

This video tutorial features the designing process of a Door (Panel with Frame) with the aid of Autodesk Inventor's part and assembly modelling functionality. Here we have added some more feature i.e., design of rounded beading, cutting of rectangular slots around the Frame of Panel in our previously created model. The highlight of the video is application of 'Copy Components' feature that is quite a time saving utility available in the Assembly modeling environment.

 

download-Link

 


Click the following link to get the model file: - http://bit.ly/2nHK1w6

 

 

Transcription of Video

  1. Create a new assembly file with an English template.
  2. Place the Part 1 and Part 2 in the assembly.
  3. Apply constraints between Part1 and Part2 to position properly according to the design of the frame.
  4. Two more instances of the Part1 and Part 2 are required, so use the Copy components command to duplicate these parts.
  5. Activate the Copy Components command.
  6. Select the Part1 file to create its copy.
  7. Take a look on this green status button which is active by default, it means a copy of the component would be created that would not be associative to the source file.
  8. Click Next button.
  9. Click OK to generate the new component.
  10. Unground the Part1_CPY to apply the constraints.
  11. Rotate the component to position properly for applying new mates.
  12. Apply Mate and Flush constraints between Part1_CPY and Part2, so that the parts may fit with each other without any obstacle.
  13. Check the interface between Part1 and Part2.
  14. Also create a copy of Part2.
  15. Apply the mates as shown earlier.
  16. Now the assembly is complete.
  17. Save the file with the name Subassembly-1 and close it.
  18. Open the Part3 file from the Subassembly-2 folder.
  19. Draw a new sketch on this face to create the beadings with the aid of Project Cut Edges command and Arc tool.
  20. Activate the Extrude command and select Cut option to remove the extra material.
  21. Activate the Mirror Tool and select the Extrusion43 feature from the browser bar.
  22. Define the XZ plane of the model as a mirroring plane and execute the command.
  23. Create a Work Plane at a defined angle with respect to this edge.
  24. Start a new sketch over this Plane.
  25. Use Project Cut Edges command to convert the intersecting edges of the model as sketches.
  26. Exit the sketch and activate the Extrude command with Cut option to remove the excess material from the model.
  27. Remove the material from this face as done earlier.
  28. Repeat the same type of operations which were done earlier.
  29. Mirror these three features by using the mid plane of the model.
  30. Create a new work plane on this point perpendicular to this edge.
  31. Create another work plane at an offset distance of 1/16 inch from this work plane and close its visibility.
  32. Create a new sketch on the Work Plane30.
  33. Use Project Cut Edges command to get the model edges.
  34. Draw a rectangle with the given dimensions.
  35. Exit from the 2D sketch.
  36. Activate the Extrude command with Cut option to create rectangular slots around the rounded beading.
  37. Mirror these extrude features to complete the file.
  38. Save the Part3 file and close it.
  39. Open the Part4 file.
  40. Draw a new sketch on this face to create the beadings with the aid of Project Cut Edges command and Arc tool.
  41. Activate the Extrude command and select Cut option to remove the extra material.
  42. Activate the Mirror Tool and select the Extrusion25 feature from the browser bar.
  43. Define the XZ plane of the model as a mirroring plane and execute the command.
  44. Create a new work Axis by using these two points.
  45. Create a Plane at a defined angle with respect to this axis.
  46. Start a new sketch over this Plane.
  47. Use Project Cut Edges command to convert the intersecting edges of the model as sketches.
  48. Exit from the sketch and activate the Extrude command with Cut option to remove the excess material from the model.
  49. Mirror the Extrusion26 feature by using XY plane of the model.
  50. Create a new sketch over the front face of the model.
  51. Use Project Cut Edges command to get the model edges.
  52. Draw a rectangle with the given dimensions.
  53. Exit from the 2D sketch.
  54. Activate the Extrude command with Cut option for making slot over the beading.
  55. Mirror the cut feature by using XZ Plane of the model.
  56. Save the Part4 file and close it.
  57. Open the Part5 file.
  58. Repeat the same process as done earlier in the Part4.
  59. Now the model is complete.
  60. Save the Part5 file and close it.
  61. Create a new assembly file with an English template.
  62. Place the Part3 and Part4 files respectively by using Place Component tool.
  63. Apply the Mate and Flush constraints between these two components to fix it according to the design of Door Panel.
  64. Check the interface between these components.
  65. Place the Part5 file.
  66. Fix it in the same way as the Part4 was fixed with Part 3.
  67. Place another instance of the Part4 in the assembly by using Copy Component tool.
  68. Fix the Part4_CPY into the groove of Part3 by using mates.
  69. In the same way, place second instances of Part5 and Part3 and fix them to complete the frame.
  70. Place the Part9 component in this assembly and fix it inside groove of the frame.
  71. Place one more instance of Part9 in the assembly and fix it tending towards its completion.
  72. Place Part10 component in the assembly and fix it by applying mates.
  73. Check the interface between Part10 and Part3.
  74. Save the assembly with the name Subassembly-2.
  75. Create a new assembly with an English template.
  76. Place the Subassembly-2 file.
  77. Copy this subassembly by using Copy Component tool.
  78. Change the name of the newly created subassembly as subassembly-3.
  79. Utilize the ‘User Path’ option to define a new save location for Subassembly-3 along with its related components.
  80. Fix these components by applying Mate and Flush constraints between them.
  81. Save the assembly with the name ‘Subassembly of frame with Panel’.
  82. Cut the taper locking slot on the frame as shown.
  83. First create sketch and apply Extrude feature with cut option.
  84. Remove the extra material from this part also.
  85. Repeat the same steps for the remaining parts too.
  86. In this panel of door, perform similar type of operations as done earlier.
  87. Start sketching, afterwards apply Extrude feature with cut option.
  88. Look at the quick access tool bar, the Design Doctor indicates that there is an error in the assembly. So correct it by applying modification in an Assembly constraint.
  89. Open this Subassembly separately and find the mate where the problem exists.
  90. This constraint has gone missing, so delete this mate and apply it again.
  91. Return back to the assembly.
  92. Analyse Interface between these two subassemblies and close the file.
  93. Create a new assembly file and place Subassembly in this assembly.
  94. Now place the Subassembly of Frame with panel.
  95. Fix the Subassembly of Frame with Panel within the Subassembly of outer Frame of Door.
  96. In this mate, set the offset distance of ¼ inch to accommodate the hinges.
  97. Save the assembly with the name ‘Door (Panel with Frame) Modified Design’.

Sunday, May 18, 2014

Photo Frame (Design-2)--Autodesk Inventor 2013 (with caption and audio narration)

Photo Frame (Design-2)_1

Photo Frame (Design-2)_2

Serial No. 207

Photo Frame (Design-2)--Autodesk Inventor 2013 (with caption and audio narration)

This video tutorial features the designing process of a Photo Frame with the aid of Autodesk Inventor's part and assembly modelling functionality. The highlight of the video is application of 'Copy Components’ feature that is quite a time saving utility available in the Assembly modelling environment.

download-Link

 


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

 

 

Transcription of Video

  1. Create a new part file with an English template.
  2. Start a new sketch over XY plane.
  3. Draw a sketch with the help of Line tool and apply the dimensions as displayed.
  4. Use constraints to position properly and fully constrain the sketch.
  5. The sketch is complete, hence finish it.
  6. Activate the Extrude command and set the direction arrow to ‘Symmetric’ option.
  7. Enter the Extrude length and execute the command.
  8. Change the colour of model as your wish, so that it can be seen clearly in the design window.
  9. Save the file with the name Part1.
  10. Create a Plane at an angle with respect to this edge.
  11. Start a new sketch over this Plane.
  12. Use Project Cut Edges command to convert the edges of the model as sketches.
  13. Exit the sketch and activate the Extrude command to remove the excess material from the model.
  14. Create the same type of cut on the other side of the model, by utilizing the Mirror Tool.
  15. Activate the Mirror Tool and select the Extrusion2 feature from the browser bar.
  16. Define the XY plane of the model as mirroring plane and execute the command.
  17. Save the file and close it.
  18. Create a new assembly file with an English template.
  19. Place the Part 1 in the assembly.
  20. Save the file with the name Photo Frame (Design-2).
  21. Activate the Copy components command and select the Part 1.
  22. Take a look on this button which is active this time, it means a copy of the component will be created that will not be associative to the source file.
  23. Click Next button.
  24. In the Copy Components: File Names dialogue box, remove the check mark from the ‘Suffix’ option and give the name of the new copied component manually.
  25. Edit the Part2 to resize the model.
  26. Return back to the assembly environment.
  27. Unground the Part2 to apply the constraints.
  28. Apply Mate constrain between side faces of these two parts.
  29. Apply Flush Mate between top faces of these two parts.
  30. Apply another Mate constrain between vertical edges of each two parts.
  31. Check the interface between two parts.
  32. Activate the ‘Copy Components’ tool once again.
  33. Activate the ‘Suffix’ option in the Naming Scheme section and apply it.
  34. Change the grounded position of the newly created copy of the Part 1.
  35. Rotate the component to position it properly for applying new mates.
  36. Apply the same set of mates as shown earlier.
  37. Now create a copy of Part2 in the assembly and position it properly.
  38. Apply mates between the components to complete the model.

Photo Frame (Design-1)--Autodesk Inventor 2013 (with caption and audio narration)

Photo Frame (Design-1)_1

Photo Frame (Design-1)_2

Serial No. 206

Photo Frame (Design-1)--Autodesk Inventor 2013 (with caption and audio narration)

This video tutorial features the designing process of a Photo Frame with the aid of Autodesk Inventor's part and assembly modelling functionality. The highlight of the video is application of 'Copy Components’ feature that is quite a time saving utility available in the Assembly modelling environment.

download-Link



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



Transcription of Video

  1. Create a new Part file with an English template.
  2. Create a new sketch on the XY Plane.
  3. Create the base sketch of photo frame with the given dimensions and by utilizing line tool.
  4. The sketch is complete.
  5. Exit from the sketching environment.
  6. Activate the Extrude command from the marking menu.
  7. In the Extrude dialogue box, select ‘Symmetric’ option for the direction.
  8. Enter the value in the distance field and execute the command.
  9. Change the model colour to Flaked Reflective Beige.
  10. Pick the ‘Angle to Plane around Edge’ tool.
  11. Click the left vertical edge of the model and then select front face of the model.
  12. Enter the angle in the edit box.
  13. Click the green check mark to create a work plane for the new location.
  14. Create a new sketch on this plane.
  15. Use the Projected cut Edges tool to get the projected edges of the model.
  16. Finish the 2D Sketch.
  17. Activate the Extrude command to remove the side portion of the model.
  18. Close the visibility of this work plane.
  19. Apply the same type of cut feature on the opposite side of the model by using Mirror tool.
  20. Activate the Mirror tool and select Extrusion1 from browser bar.
  21. Select XY Plane of the model as a reference plane for the mirror.
  22. Click OK to create the mirror feature.
  23. Save the part file with its default name.
  24. Close the part file.
  25. Create a new Assembly file with an English template.
  26. Place the Part1 file by utilizing ‘Place Component’ tool.
  27. Save the assembly file with the name ‘Photo Frame (Design-1)’.
  28. Activate the ‘Copy Components’ tool.
  29. Copy Components dialogue box is displayed in the graphics window.
  30. Select the Part1 file in the graphics window.
  31. Blue double plus status button is selected by default.
  32. This button indicates; the newly generated component will be saved in a separate part file that will not be associative to the source part file.
  33. Click Next button.
  34. Uncheck the ‘Suffix’ option in the Naming Scheme section and apply it.
  35. Change the name of file Part2.
  36. Click OK to close the dialogue box.
  37. Edit the Part2 to resize the model.
  38. Unground the Part2 to apply the constraints.
  39. Rotate the Part2 by using Rotate Component tool.
  40. Apply Mate constrain between side faces of both parts.
  41. Apply another Mate constrain between two vertical edges of both parts.
  42. Apply Flush Mate between top faces of both parts.
  43. Check the interface between two parts.
  44. Activate the ‘Copy Components’ tool again.
  45. Activate the ‘Suffix’ option in the Naming Scheme section and apply it.
  46. Change the grounded position of the newly created copy of the Part 1.
  47. Rotate the component to properly position it for applying new mates.
  48. Apply the same set of mates as shown earlier.
  49. Now create a copy of Part 2 in the assembly and properly position it.
  50. Apply mates between the components to complete the model.

Thursday, May 1, 2014

Modelling an Elbow in Creo Parametric 2.0

Elbow

In this tutorial we will create an Elbow by utilizing part modelling capabilities of Creo Parametric 2.0

Viewers will be able to watch application of many part modelling tools like Sweep, Shell, Helical Sweep, Pattern and Round tool as well as 2D sketching techniques are also shown.

In cutting of threads I will utilize the same BSP Thread Profile that was shown a previous video by me..

Video Screen Shots

Transcription of Video

  1. Start a new part file from scratch with the default template and give it a name ‘Elbow’.
  2. Select the Top Datum plane and create a new sketch on this plane.
  3. Click the Sketch View icon to orient the sketching plane parallel to the screen.
  4. Clear the screen by closing the visibility of Datum Planes, Axis, Points, Spin centre, etc.
  5. Activate the line tool and draw the sketch as displayed.
  6. As soon as the lines are drawn the constraints are automatically applied.
  7. Change the dimension values as displayed.
  8. Activate the Circular Fillet tool and apply a fillet between these two lines.
  9. Fill the radius of the fillet.
  10. Select the dimensions and lock them.
  11. The sketch is complete so exit from the sketching mode.
  12. Activate the Sweep tool.
  13. Define the visible sketch as trajectory for the sweep.
  14. Flip the direction of the sweep.
  15. Click this icon to activate internal sketcher for creating the sweep cross section.
  16. Draw a circle at the end of trajectory and apply the dimensions as displayed.
  17. Click Ok to return to the Sweep tab.
  18. The preview of the feature is visible so click ok to execute the command.
  19. Change the colour of the model as per your wish.
  20. Activate the Shell tool.
  21. Select the surfaces of the model to be removed. Use ctrl key of your keyboard while selecting multiple surfaces.
  22. Specify the Shell thickness and execute the command.
  23. Save the model file.
  24. Open the visibility of datum planes and create a sketch over Top datum plane.
  25. First create a centerline in the sketch that will work as axis of revolution for the sweep.
  26. Take the project of the internal edge of the model.
  27. Delete this line.
  28. You can see a reference line still exists which will be used to create a new line for Helical sweep profile.
  29. Fill the dimension value which will be the length of thread.
  30. Exit from the sketching mode.
  31. Open the file named ‘BSP_Thread_Profile’.
  32. Here you can see a sketch profile of a British Standard Pipe Thread is drawn. The pitch of the profile is 1/14 inches which governs all the other dimensions by some relations.
  33. Copy this sketch profile.
  34. Now switch back to Elbow file.
  35. Activate the Helical Sweep tool.
  36. At present software prompts to select an open sketch to define Helix sweep profile so select this line.
  37. Fill the pitch value as displayed.
  38. Click this icon to create the sweep section or profile.
  39. Place a geometry point.
  40. Now paste the BSP Thread Profile that was copied earlier and which is still in the Windows Clipboard.
  41. As soon as you paste the sketch the move tool will activate.
  42. In the scale field fill the value 1.
  43. Rotate the profile by 90° in clock wise direction.
  44. Move the profile near to the geometry point and click Ok.
  45. Make some minor correction in the profile because in pasting it some constraints have gone missing.
  46. Again move the profile more near to the geometry point to apply some more constraints.
  47. Delete any constraint that gives error in placing new constraint.
  48. Now profile is properly positioned so exit the sketch.
  49. The preview of sweep is visible in the graphic window.
  50. Activate the remove material option and execute the command.
  51. Activate the shaded with edges option.
  52. Hide the visibility of visible sketch.
  53. Select the Helical sweep in the Model Tree and activate the Pattern Tool.
  54. Open the visibility of Coordinate System.
  55. Set Axis as the type of pattern.
  56. Select Y axis of Coordinate System as axis of rotation.
  57. Enter the number of members to be patterned.
  58. Define the Angle between the pattern members.
  59. Execute the command.
  60. Activate the Round Tool.
  61. Fill the radius of round.
  62. Select the edges and execute the command.
  63. The fully created model is in front of you.
  64. Switch between the Shading With Edges and Shading view.
  65. Save the model file.

download-Link


Get the Model file by visiting the following link:-
http://bit.ly/2m7Haw4