Wednesday, September 2, 2015

SolidWorks Tutorial || Bolt and Nut Modeling

Bolt and Nut with captions (YouTube Icon)

In this SolidWorks tutorials we are going to demonstrate the modeling of a bolt and nut which covers detailed topics of the software along with basics of part with assembly modeling.
In part modeling topic we will learn about basic sketching, Extrude Boss/Base Feature, Extruded Cut, Revolved Cut, Chamfer, Helix and Spiral Curve, Swept Cut etc.
From Assembly modeling section we will learn about Beginning a new assembly with a previously created component, Inserting additional components, Move with Triad Command, Application of Mates etc.
Addition to this some detailed topics like creating Global Variables and using them over sketches and 3D Features, relating two features with equations, using previously created sketches in the current files etc.
So let’s start the tutorial and watch everything in action……..


Transcription

Creation of Bolt…

  1. Create a new part file.
  2. Start a new sketch over front plane.
  3. The units of the file must be set to IPS (inch, pound, second).
  4. Fractional and Decimal setting should be set as displayed.
  5. Create a circle over sketch origin.
  6. Now activate Equation tool.
  7. Create a Global Variable named ‘D’. All the other dimension now further will be related to this dimension.
  8. Apply the recently created Global Variable dimension over the Circle.
  9. Activate the Display Dimension Names.
  10. Convert the Circle into construction Geometry.
  11. Draw a 6 sided polygon coincident to sketch origin.
  12. Apply the dimension over it in relation to Global Variable.
  13. Display the relation between the sketches by activating ‘View Sketch Relation’ command.
  14. Apply a vertical relation between the sketch center point and edge point of polygon.
  15. The sketch is complete so save the file with the name Bolt.
  16. Now switch to the Feature Tab and activate Extrude Boss/Base Tool.
  17. The sketch has already been selected as profile for extrude.
  18. Fill the depth value and execute the command.
  19. Now change the model colour as per your wish.
  20. Now start a new sketch over Right Plane.
  21. Activate the Section View along the Right Plane to see the new sketch easily.
  22. Change the view orientation parallel to sketching plane.
  23. Activate the Intersection Curves command to take the project of the entire intersecting edges of previously created part.
  24. Convert the projected sketch into construction geometry.
  25. Draw the sketch as displayed along with dimensions.
  26. The sketch is complete so exit from the sketching mode.
  27. Activate the Revolved Cut tool.
  28. Select the sketch profile and define the axis of revolution.
  29. Click the green check mark to execute the command.
  30. Deactivate the Section View command by pressing its button once.
  31. Open the visibility of Sketch1 form the Design Tree.
  32. Start a new sketch over back face of the model.
  33. Take the project of previously drawn circle on Sketch1 into the current sketch using Convert Entities tool.
  34. Close the visibility of Sketch1.
  35. Draw the sketch as displayed.
  36. The sketch is complete so exit from the sketching mode.
  37. Activate Extruded Cut Tool.
  38. Select the sketch and place a check mark over, flip side to cut option.
  39. Fill the depth of cut and execute the command.
  40. Activate Extrude Boss/Base Tool and draw a sketch over back face of model along with dimensions.
  41. Exit the sketch and fill the depth of the extrude 2”.
  42. Hit enter key to execute the command.
  43. Select this edge of the model and activate Chamfer Tool.
  44. Fill the distance and angle values.
  45. Click green check mark to execute the command.
  46. Again create a new sketch over Right Plane as displayed.
  47. We will not create the thread profile here for the Bolt, instead we will past it from the file.
  48. Open the file named ‘UNF Screw External Thread Profile’
  49. Here you can see a sketch profile is drawn. The pitch of the profile is 1/20 or 0.05 inches which governs all the other dimensions by some relations.
  50. Copy the sketch present in the file and return back to the previous file.
  51. Now paste the thread profile here.
  52. Properly position the sketch using Rotate and Move Entities Tools.
  53. Exit from the sketching mode.
  54. Next draw a circle along with dimensions over back face of the model.
  55. Do not exit the sketch and switch to Features Table.
  56. Activate Helix and Spiral Tool.
  57. First reverse the direction of the curve.
  58. We will define the curve using Height and Pitch.
  59. Fill the height and pitch values as shown.
  60. To coincident the curve start point with the profile end point adjust the start angle.
  61. Click the green check mark to execute the command.
  62. Activate the Swept Cut Tool.
  63. First define the profile then the path and execute the command.
  64. The model is complete so save the file and close it.

Creation of Nut …

  1. Start a new part file.
  2. Start a new sketch over front plane.
  3. Set the units of file in the same way as we did in our first part.
  4. Create a circle coincident to the sketch origin.
  5. Create a Global Variable named ‘D’. All the other dimension now further will be related to this dimension.
  6. Apply the dimension over the circle.
  7. Convert the Circle into construction Geometry.
  8. Draw a 6 sided polygon coincident to sketch origin with dimensions.
  9. Apply sketch relation to fully define the sketch.
  10. The sketch is fully defined so exit from the sketching mode.
  11. Save the file with the name Nut.
  12. Activate Extrude Boss/Base Tool.
  13. Fill the depth value and execute the command.
  14. Now change the model colour as per your wish.
  15. Next start a new sketch over Right Plane.
  16. Activate the Section View along the Right Plane to see the new sketch easily.
  17. Change the view orientation parallel to sketching plane.
  18. Activate the Intersection and take the project of entire intersecting edges of the model.
  19. Convert the projected sketch into construction geometry.
  20. Draw the sketch as displayed along with dimensions.
  21. The sketch is complete so exit from the sketching mode.
  22. Activate the Revolved Cut tool.
  23. The sketch profile is automatic selected so define the axis of revolution and execute the command.
  24. Open the bolt file and draw a sketch over Right Plane as displayed.
  25. We are creating this sketch to get the dimensions for the hole that would be applied over our Nut.
  26. Here we got our required dimension so switch back to the Nut file.
  27. Activate Extruded Cut Tool.
  28. Draw a sketch over back face of the model with dimension we got previously.
  29. Exit the sketch and in Direction 1 filed select through all option.
  30. Execute the command to create hole.
  31. Close the file of the Bolt that is still open and return back.
  32. Activate Chamfer Tool and apply it over the following edge of the model with the displayed parameters.
  33. Start a new sketch over Right Plane.
  34. Take the project of the model edges and convert them into construction geometry.
  35. Again we will past the thread profile from the file ‘UNF Screw Internal Thread Profile’
  36. Copy the Sketch and return back to the Nut File.
  37. Paste the copied profile in the current sketch.
  38. Properly position the sketch using Move Entities Tools.
  39. The sketch is complete so exit from the sketching mode.
  40. Create a circle over back face of the model as displayed.
  41. Activate Helix and Spiral Tool.
  42. First select the circle.
  43. We will use Height and Pitch to define the curve.
  44. Fill the pitch value as displayed and execute the command.
  45. Select Helix/Spiral feature from the Design Tree and activate Equation Tool.
  46. Select the height dimension from the design window to add it in the Equation field it would be equal to the depth of Boss-Extrude feature.
  47. Apply and save all the changes.
  48. Activate Swept Cut tool.
  49. First select the profile then the path and execute the command.
  50. The file is complete so examine the threads and close the file that are open after saving.

Assembly of Bolt and Nut

  1. Create an assembly file.
  2. First place the Bot file in the assembly coincident to the origin.
  3. Save the file with the name Bolt and Nut.
  4. Open the visibility of Temporary Axis.
  5. Activate Insert Components Tool
  6. Browse the Nut file and place it.
  7. Select the Nut part and activate Move with Triad command from right click context menu.
  8. Rotate the model as displayed.
  9. Select the both axis of parts and activate Mate command.
  10. The coincident mate has been applied automatically so execute the command.
  11. Clear the screen by closing the visibility of Temporary axis and origin of file.
  12. The model is complete so save the file.

    download-Link

Get the finished model file by visiting the following link:--
http://a360.co/1mUnR2D

 

 

Video Screenshot

The image showing the process of relating two feature with equation in Solidworks….