iTwist Drill -- Autodesk Inventor 2013 Tutorial (with caption and audio narration)

Serial No. 288

iTwist Drill -- Autodesk Inventor 2013 Tutorial (with caption and audio narration)

In this part modelling tutorial of ‘Autodesk Inventor,’ we will create a model named ‘iTwist Drill ’. We will start our work by defining some User Parameters that will be used to create a mathematical relation between the dimensions applied in the due course of modelling the ‘Twist Drill’.
Then we will create a circle and extrude it. Next, we will create some user-defined work planes at specified spots. These planes will be used to draw some more sketches, to be used as a base profile for cutting flute (rounded grove) over the round bar. Then a coil feature and an extrude feature with a cut operation will be applied to create flute. Then using a circular pattern tool we will duplicate the same at an angle of 180°. Next, we will create some sketch profiles to cut lip and lip relief on the edge of the drill bit. The process will be the same as applied earlier. Later more coil feature will be applied to complete the model.
The highlight of the videos is the after creating the model with full parameters the iPart creation of the model is also displayed.
Watch the video to understand all the process clearly
.................................................................
To more understand the creation process of an iParts in Autodesk Inventor watch a related video at the following link:---
https://youtu.be/KNCrDJdPm-s.

Click the following link to get the model file: - http://bit.ly/2mFTa8o 
 

 

 

Transcription of the Video

1. Create a new inch part file.
2. Go to the Manage tab and activate the ‘Parameters’ command.
3. Add the Parameter name ‘diaMajor’ in the ‘User Parameters’ tab by using 'Add Numeric' key and set the value 7/16 ul in the equation area.
4. In the same manner, add two more parameters and click OK.
5. Create a new sketch over XY Plane.
6. Create a circle and place the dimension, select the ‘List Parameters’ and choose diaMajor and click OK.
7. Right-click the dimension and select ‘Expression’.
8. Finish the sketch and activate the ‘Extrude’ command.
9. The sketch profile will automatically select and set the distance value relating in terms of parameters, click OK.
10. Save the file as ‘iTwist Drill’.
11. Change the colour of the model as you wish.
12. Activate the ‘Plane’ command and create a plane inside from this face.
13. And place the dimension.
14. Change the name of the plane as ‘ShankEnd’ and create an Axis in the centre of the part, name it as majorAxis.
15. Activate the Axis command and select WorkPlane1 and XZ plane.
16. A new axis will form on the intersection of these two planes.
17. Change the name of this axis, call it as ‘Intersection Helix Origin Planes’.
18. Now activate the ‘Point’ command and create a work point at the intersection of this vertical plane and axis .
19. Activate the ‘Parameters’ command and add HelixAngle in the ‘User Parameters’ tab with the help of ‘Add Numeric’ button.
20. Now see, different kinds of measurement options are visible here, you choose only one option at a time as per your design.
21. In the Unit Type dialogue box, select degree option and click OK.
22. Set the Helix angle to 30 degrees and click OK.
23. Activate the ‘Plane’ command and select ‘Intersection Helix Origin Planes’ axis and XZ Plane, set the specified angle relating to parameters.
24. Change the name of this plane, as ‘helix Origin Plane1’.
25. Close the visibility of ‘ShankEnd’ plane and ‘Intersection Helix Origin Planes’ axis.
26. Add two more parameters name as ‘web’ and ‘diacutter’.
27. Create a new sketch on this plane.
28. Rotate the model parallel to the inclined plane by using ‘Look at Plane’ command.
29. Activate the slice graphics command.
30. Take the project of ‘Intersection Helix Origin Planes’ and ‘Work Point1’ with the help of ‘Project Geometry’ command.
31. Create a circle and set the desired dimensions to fully constrain the sketch.
32. Finish the sketch and change the name of the sketch as ‘diacutter’.
33. Add one more parameter call it as ‘helixPitch’.
34. Activate the ‘Coil’ tool, it will automatically select the sketch profile, select the major axis and select the ‘Cut’ option in the Coil dialogue box.
35. Go to the Coil Size tab and select the ‘Pitch and Height’ option.
36. In the Pitch area select from the List Parameters click ‘HelixPitch’ and in the Height area select from the List Parameters, click ‘fluteLen+diaMajor’.
37. Click OK to create the coil feature.
38. Open the visibility of ‘diacutter1’ sketch.
39. Activate the ‘Extrude’ command, select the ‘All’ option in the Extents field and choose ‘Cut’ option and click OK.
40. Change the name of this extruded cut feature as ‘blend’.
41. Activate the ‘Circular Pattern’ tool and select the Coil1 and blend feature from the browser bar, select the major axis as a rotation axis and fill the value of Occurrence count and angle.
42. Click OK to execute the command.
43. Create a new sketch on this face.
44. Take the project of these four curves and circle.
45. Draw a circle and tangent it to this curve.
46. Select all the sketches and convert it construction geometry.
47. Create two points on the intersection point of this circle and curve.
48. Draw a line passing through the centre of the circle and add coincident constraint between line and point.
49. Take the project of ‘Intersection Helix Origin Planes’ axis.
50. Set the angular dimension between these two lines.
51. Finish the sketch and change the name of the sketch as ‘TipRef1’.
52. Make a Work Axis on this line.
53. Change the name of the axis as ‘lipReliefGeom’.
54. Activate the ‘WorkPlane’ command and select these two axes.
55. Change the name of the plane as ‘lipReliefGeom’.
56. Now the plane is created along the axis.
57. Activate the ‘Angle to Plane around Edge’ command.
58. Select the ‘lipReliefGeom’ plane and ‘majorAxis’, set the angle 90 degrees, click OK.
59. Add the parameter ‘tipangle’ and set the angle 118 degrees.
60. Create a new sketch over the ‘lipReliefGeom’ plane.
61. Activate slice graphics command, take the project of this edge and major axis.
62. Draw a vertical line and add coincident constraint between the midpoint of a line and centre line.
63. Draw a horizontal line and join it to the midpoint of the projected line.
64. In the same manner, draw another line on the opposite side of the sketch and add the equal constraint between these two horizontal lines.
65. Add the Symmetric constraint between these two lines.
66. Set the dimensions relating to the parameters on all the sketches.
67. Finish the sketch and activate the ‘Extrude’ command.
68. Select the sketch profile, click ‘Cut’ option and select ‘Symmetric’ option, select ‘Through all’ option and Click OK.
69. Change the name of Extrusion as ‘ptangle’.
70. Add the parameters ‘lip relief angle’ and ‘lip clearance angle’ and finally set the angle values.
71. Activate the ‘WorkPlane’ command, select this face and edge and set the value 90-degree, click OK.
72. In the same way, create another work plane in opposite side of the previous plane, the two workplanes has been created along the taper face.
73. Change the name of workplane as ‘liprelief’.
74. Create a new sketch over the ‘lipRelief’plane.
75. Activate the ‘Look at plane’ command and select the ‘lip relief’ plane for rotating the model along the plane.
76. Activate the slice graphics command, take the project of ‘major axis’ and ‘lipReliefGeom’ axis.
77. Draw a circle over the intersection point of vertical and horizontal lines.
78. Set the dimension, select ‘diaMajor’ from list parameters.
79. Select all the sketch and convert it to construction geometry.
80. Draw a horizontal line and a vertical line.
81. Draw another line from the endpoint of a vertical line passing through center line and connect to the opposite side of the circle.
82. Apply the angular dimension, select ‘lipClearanceAngle’ from list parameters.
83. Apply another angular dimension, select ‘lipReliefAngle’ from list parameters.
84. Create a line from the endpoint of horizontal line and connect to the opposite side of the circle.
85. Finish the sketch and activate the ‘Extrude’ command.
86. Choose the ‘Cut’ option → select ‘Symmetric’ option → select ‘All’ option in the Extents field and click OK.
87. Change the name of Extrusion Cut as ‘liprelief’.
88. Activate the ‘Circular Pattern’ tool and select the liprelief cut feature → click ‘Continue’ button for selecting as a rotation axis → set the occurrence count and angle value and Click OK.
89. Activate the ‘Parameters’ command and add the one more parameter named ‘fluteReliefSetback’.
90. Set the desired value in terms of equation.
91. Click Ok.
92. Create a new sketch over the YZ Plane and activate the slice graphics command.
93. Take the project of the major axis and shankEnd workplane.
94. Create a rectangle and apply the preferred dimensions.
95. Change the name of the sketch as ‘clearanceDia’.
96. Activate the ‘Coil’ tool → select the major axis → go to the Coil Size tab → select the ‘Pitch and Height’ option.
97. In the Pitch area select ‘HelixPitch’ from the List Parameters and in the Height area select ‘fluteLen+helixpitch’ from the List Parameters.
98. Go to the Coil Shape tab, select ‘Cut’ option and click OK.
99. Open the visibility of ‘clearanceDia’ sketch.
100. Activate the ‘Coil’ tool once again → choose ‘Cut’ option → select the Coil size tab but this time ‘Pitch and Revolution’ should be selected in ‘Type’ area in place of ‘Pitch and Height’ option → set the pitch value as ‘helixPitch’ and set the revolution value 0.25 and taper angle 3 degrees.
101. Click the ‘Axis’ button to go in the reverse direction of coil feature.
102. Click OK to create coil feature.
103. Replicate the pattern of these two coil feature twice times with the help of ‘Circular Pattern’ tool.
104. Activate the ‘Create iPart’ command.
105. Remove all the key except ‘diamajor’, ‘oal’, ‘fluteLen’ parameters in the ‘ipart Author’ dialogue box.
106. Insert new row for creating a new member of different size.
107. Change the value of diamajor, oal and fluteLen column.
108. Click Verify button to apply the new member.
109. Click OK.
110. Go to the browser bar, under the Table, Let watch here, two row has been created.
111. The first row is default size and the second row is our new size.
112. Select each one by one to activate it and observe the result.
113. Activate the ‘Edit via Excel Spreadsheet’ command.
114. In the same manner, several members have been created with different sizes in the excel sheet.
115. We showed some examples of different sizes.
116. Save the excel file and close it.
117. Let see here it automatically updates all the family members, which had been added in the browser bar.
118. Select each one by one to activate it and observe the result.
119. Save the part file.

Twist Drill (SolidWorks 2014Tutorial)

Serial No. 23

Twist Drill (SolidWorks 2014Tutorial)

In this part modelling tutorial of ‘SolidWorks’ we will create a model named ‘Twist Drill ’. We will start our work by defining some Global Equations that will be used to create mathematical relation between the dimensions applied in the due course of modelling the ‘Twist Drill’.

Equations applied in modeling of Twist Drill with Solidworks

Then a circle will be extruded to form a 3D solid. Next some planes will be created to draw new 2D sketch profiles. Then Helix curve will be created. By using Sweep Cut tool on the basis of previous 2D sketch profiles and Helix curve our first flute will be cute over the rounded bar. Again a relevant Cut Extrude command will be applied. Then both the features will be duplicated using circular pattern tool at an angle of 180°. Next we will create some more sketch profiles to cut lip and lip relief on the edge of drill bit. The process will be the same as applied earlier. Later some more Sweep Cut feature will be applied to complete the model. The highlight of the video is to show the usage of work planes with precision and usage of circular pattern tool to save time.

Features
applied in creation of
Twist with Solidworks

   Watch the full tutorial on the video embedded below..

Click the following link to get the model file: -http://bit.ly/2onaj7c





To more understand twist drill geometry watch the following image and visit the associated  link..

TWIST DRILL GEOMETRY. 

Create a Twist Drill as an ‘iPart’ through-Autodesk Inventor 2013 (with caption and audio narration)

Serial No. 211

Create a Twist Drill as an ‘iPart’ through-Autodesk Inventor 2013 (with caption and audio narration)

iParts are different from standard parts they are table driven part factories with a group of parts. The parts have the different parameter and different features that are controlled by table. The table is controlled by iPart Author or Spread Sheet.

 
 
   

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

 

 Transcription of Video

1. Activate the ‘Create iPart’ command.
2. iPart Author dialogue box is visible in the graphics window.
3. Notice that columns for the named parameters were automatically displayed and iTwist Drill-01 has been added to the current file to define the first family member’s part number.
4. Only 3 named parameters are required, so discard the other parameters by clicking Remove arrow button one by one each time.
5. Right click the row of iTwist Drill-01, and click Insert Row in the context menu.
6. In the second row change the value of diameter Major, Overall Length and Flute Length for the new member.
7. Click OK to generate the iPart.
8. Parameter Table has been added in the browser bar.
9. Click the ‘+’ sign to expand the node.
10. Right click the iTwist Drill-02 node and choose ‘Activate’ option to change the size of the member.
11. Activate the first member once again.
12. Right-click the table icon and select ‘Edit via Spreadsheet’.
13. The iPart table is opened in Microsoft Excel.
14. More parameters can be added with the excel file.
15. Save the spreadsheet and close it.
16. In the browser bar, expand the table node, the family members have been automatically added, it can also be seen from the Edit Table.
17. Save the part file.

iTwist Drill (Autodesk Inventor 2013)

Serial No. 210

iTwist Drill (Autodesk Inventor 2013)
In this part modeling tutorial of ‘Autodesk Inventor’ we will create a model named ‘iTwist Drill ’. We will start our work by defining some User Parameters that will be used to create mathematical relation between the dimensions applied in the due course of modeling the ‘Twist Drill’.

Parameters used in iTwist Model with Autodesk Inventor

Then we will create a circle and extrude it. Next we will create some user defined work planes at specified spots. These planes will be used to draw some more sketches, to be used as base profile for cutting flute (rounded grove) over the round bar. Then a coil feature and an extrude feature with a cut operation will be applied to create flute. Then using a circular pattern tool we will duplicate the same at an angle of 180°. Next we will create some sketch profiles to cut lip and lip relief on the edge of drill bit. The process will be the same as applied earlier. Later more coil feature will be applied to complete the model.

Features applied in creation of iTwist with Autodesk Inventor

The highlight of the videos is the after creating the model with full parameters the iPart creation of the model is also displayed.
Watch the following video to understand all the process clearly

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

To properly understand the creation process of an iParts in Autodesk Inventor, read the related Blog Post mentioned below....

Create a Twist Drill as an 'iPart' (Autodesk Inventor 2013)

And to more understand twist drill geometry watch the following image and visit the associated  link..

TWIST DRILL GEOMETRY. 

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

Serial No. 197

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

 

Transcription of Video

1. This is the model of Twist Drill that is created by us earlier. A full-fledged video related to this can be found on our You Tube Channel.
2. Here from the Browser Bar you can check the history of its modelling. A lot of 2D sketches, Extrude, Coil features, Work features and Circular Pattern were utilized to create this model.
3. In this video we will describe about the Circular Pattern Tool that was used three times in its modelling. Watch the video to understand how the tool works.
4. Circular Pattern tool duplicates one or more features and arrange the resulting occurrences by a specific count and spacing in a circular path.
5. This tool is available on Pattern Panel of Model Tab.
6. First Circular Pattern Applied in the modeling of Twist Drill
7. After activating the Circular Pattern tool the Coil1 and Extrude2 are being selected as feature for the duplication.
8. Z axis of the model has been selected as axis of revolution.
9. The number of occurrences in the pattern is 2.
10. Degree of rotation is 180.
11. After clicking the ok button the result is in front of you. A duplicate feature is created easily.
12. Watch the past and current position of the model by suppressing and un-supressing the feature.
13. Second Circular Pattern Applied in the modeling of Twist Drill.
14. This time Extrude4 is selected as feature and the Rotation of Axis is same that is the Z axis of the model.
15. The Occurrence count will be 2 and the Occurrence angle180 degree.
16. After clicking the ok button the duplicate feature is created.
17. Third Circular Pattern Applied in the modeling of Twist Drill.
18. This time two Coil features are selected for the duplication.
19. All the other specifications of the Circular pattern will be the same as previous ones.
20. The final result is visible in the design window.

Twist Drill (Autodesk Inventor 2012 Tutorial)

 Serial No. 118

Twist Drill (Autodesk Inventor 2012 Tutorial)
In this part modelling tutorial of ‘Autodesk Inventor’ we will create a model named ‘Twist Drill ’. We will start our work by extruding a circle. Then create some user defined work pales at specified spots. These planes will be used to draw some more sketches, to be used as base profile for cutting flute (rounded grove) over the round bar. Then a coil feature and an extrude feature with a cut operation will be applied to create flute. Then using a circular pattern tool we will duplicate the same at an angle of 180°. Next we will create some sketch profiles to cut lip and lip relief on the edge of drill bit. The process will be the same as applied earlier. Later more coil feature will be applied to complete the model. The highlight of the video is to show the usage of user defined work planes with precision and usage of circular pattern tool to save time.

Features used in the modeling of Twist Drill

Watch the following video to understand all the process clearly

 

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





This model can also be developed as  an 'iPart' with full mathematical relations. Please visit the following link to find the full tutorial......

iTwist Drill (Autodesk Inventor 2013)

Visit the following link to get 2D drawings sheets of the model...

To more understand twist drill geometry watch the following image and visit the associated  link..

TWIST DRILL GEOMETRY.