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Elbow.jpg

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..

Check the attachment for finished model file.

 

 

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.
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BSP Pipe Thread.jpg

This tutorial will display how to create relation based sketches in Creo Parametric. As an example we will create a sketch profile of a British Standard Pipe Thread. The pitch of the profile is 1/14 inch.

 

Transcription of Video

  1. Start a new part file from scratch with the default template and give it a name ‘BSP_Thread_Profile.
  2. You can see the English template is opened by default.
  3. Select the Front Datum plane and create a new sketch on this plane.
  4. Click the Sketch View icon to orient the sketching plane parallel to the screen.
  5. Clear the screen by closing the visibility of Spin centre, Datum Planes, Axis, Points etc.
  6. Go to setup panel and define the Grid settings.
  7. In the Grid setting dialogue box activate Static Grid spacing option and modify the X and Y spacing as displayed.
  8. Open the visibility of Grid from Sketcher display filters.
  9. Now zoom the window quite considerable to view the Grid.
  10. Draw a sketch with the help of line tool as displayed.
  11. You will see that some constraints are automatically applied and intimated time to time by the software.
  12. Create a centreline for our sketch.
  13. Apply dimensions related to our profile specification.
  14. Lock this dimension to preserve it from any modification.
  15. Again, apply an angular dimension.
  16. Apply constraints according to the demand of the sketch.
  17. Quit the sketching mode.
  18. Switch to Annotate Tab.
  19. Activate Show Annotation Tool and select the sketch.
  20. All the applied dimensions in the sketching environment will be visible.
  21. Terminate the command.
  22. Select this dimension in the design window that will be highlighted in Model Tree.
  23. Open its property from the context menu.
  24. Change its display name to ‘P’ and apply changes.
  25. Go to model Tab—Model Intent Panel and expand it to find Switch Symbol Command.
  26. Click it to display names of dimension in spite of values.
  27. Re-edit the sketch.
  28. Draw an arc tangent to both the lines.
  29. Define the Angular dimension and apply a Lock over this dimension.
  30. Exit the sketching mode and again redefine the names of the dimensions.
  31. Remove the Prefix otherwise dimension will display Rr name that will be very confusing.
  32. Expand the Model Intent Panel and Activate the Relation command.
  33. Start adding the values according to the profile. You can type or paste the values.
  34. Execute and verify the relations.
  35. Select the dimension of pitch with the help of selection filters easily.
  36. Move it to new location.
  37. Re-edit the sketch.
  38. Add more dimensions to the sketch and change its name.
  39. Give away relation according to the profile.
  40. Adding this dimension is conflicting with a previously placed constraint, so remove that constraint.
  41. Similar operations are being performed as done earlier.
  42. Again re-edit the sketch.
  43. Select these two lines and convert them to construction lines.
  44. Complete the sketch by adding few more arcs and lines.
  45. Select these sketches and duplicate using Mirror Tool.
  46. Now sketch is complete so finish the sketch and save the file.
  47. If you change the pitch, the profile will change simultaneously.
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Hacksaw Blade.jpg

In this video tutorial creation of a Hacksaw Blade is displayed. Viewers will be able to watch application of many part modelling tools like Extrude, Round, Hole, Mirror and Pattern as well as 2D sketching techniques are also shown.

 

Transcription of Video

  1. Start a new part file from scratch and give it a name ‘Hacksaw Blade.’            
  2. Select the Top Datum plane and create a new sketch on this plane.
  3. Click the Sketch View icon. This will orient the sketching plane parallel to the screen.
  4. Close the visibility of the Datum Planes, Axis and Points etc. to make the screen clear.
  5. Pick the Centre Rectangle tool from the Sketching panel.
  6. Draw a Rectangle and apply the dimensions as displayed.
  7. As soon as the new dimensions are applied the software will automatically adjust the view of design window so that the sketch can be seen clearly.
  8. Click green check mark to finish the sketch.
  9. Activate the Extrude Tool from the Shape Panel.
  10. Select the sketch and define the depth value.
  11. Select extrude both side of the sketch equally option and execute the command.
  12. Change the colour of the part according to your wish so that it can be acknowledged easily in the design window.
  13. Activate the Reorient tool and position the model in an isometric view using navigation tools.
  14. Save this view for future reference.
  15. Save the part file.
  16. Activate the Round Tool from the Engineering Panel.
  17. Select four outer edges of the model.
  18. Define the radius of the round and execute the command.
  19. Activate the Hole tool.
  20. Select the Top Face of the model to define the Placement Reference.
  21. Enter the Diameter Value for the drilled hole.
  22. Set the offset references of the hole and fill the corresponding offset values.
  23. Select through all option and execute the command.
  24. Open the visibility of Datum Planes.
  25. Select the Hole 1 in the Model Tree and activate the Mirror Tool from the Editing Panel.
  26. Select Right Datum Plane as Mirroring Plane and execute the command.
  27. Select the top face of the model and start a new sketch on this face.
  28. Specify two references for the sketch.
  29. Draw a sketch with the help of line tool as displayed.
  30. Apply the dimensions as displayed.
  31. Click green check mark to finish the sketch.
  32. Activate the Extrude Tool and select the sketch.
  33. Flip the Depth Direction.
  34. Select Remove Material option and Through all option.
  35. Click the green check mark to apply and save the changes.
  36. Select the Extrude 2 in the Model Tree and activate the Pattern Tool from the Editing Panel.
  37. Set Direction as the type of pattern.
  38. Select the front edge of the model to define the direction of the pattern.
  39. Enter the number of members to be patterned.
  40. Define the spacing between the pattern members.
  41. Click the green check mark to apply and save the changes.
  42. So fully developed model is visible in the graphics window.
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Defining and Saving a Custom (Isometric) View in Creo Parametric

 

In this tutorial you will see how to utilize the View Manger Tool to save a custom view and to navigate precisely in the graphics window.

 

Transcription of Video
  1. Click the View Manager Tool to display its dialogue Box.
  2. At present Orient tab is active. From here different type of views can be set and created/deleted.
  3. Here create a new view named Isometric View.
  4. Type the name and click the middle mouse button.
  5. Now Re-define this view.
  6. Orientation dialogue box will be opened.
  7. From here define the orientation of the model by specifying the Front and Top reference of the model.
  8. Switch to Dynamic Orient Tab.
  9. Here you can see Pan, Zoom and Spin navigation tools that are used to adjust the view of the graphic window. You can drag the slider or fill a precise value to operate them.
  10. Now spin the model 45° vertically and 30° horizontally.
  11. Hit Ok to exit.
  12. Now you can switch between the different views and set the view of your choice at any time.

 

A new update to this topic

 

That was a manual way to set up Isometric View in Creo Parametric. But by watching this video you learned to utilize View Manager Tool, Re-orient Tool and other navigation tools.

To set up Isometric View by default in Creo Parametric go options--Model Display--Model orientation and select Isometric in the dropdown of Default model orientation. That is so simple.

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Setting up a Hinge (Pin) Mechanism in Creo Parametric 2
Video Tutorial with caption and audio narration
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In this Assembly Modeling Tutorial of Creo Parametric a mechanism of a Hinge is created by using predefined Pin constraint that is available in the software. First of all, the previously created components of Hinge will be placed in the assembly and then mates will be applied to set up the mechanism.

 

Transcription of Video

  1. We have following components of Hinge, which we will place in an assembly.
  2. Later we will test its mechanism with the help of Drag Component tool.
  3. Create a new assembly with default template.
  4. Give it a name Hinge.
  5. Place the part_1 in the assembly.
  6. Drag the part so that you can see the Datum Planes of Assembly clearly.
  7. Constraint Type is set to Automatic by default.
  8. Apply a constraint between Right Datum plane of assembly and Right Datum Plane of part_1.
  9. Add a new constraint and select Front Datum Planes of assembly and Front Datum Planes of part_1 to apply a coincident constraint automatically.
  10. In the same way apply a coincident constraint between Top Datum Plane of Assembly and Top Datum Plane part_1.
  11. Now STATUS area indicates that the component is fully constrained in the assembly.
  12. Click the green check mark to apply and save the changes.
  13. Now place the part_3 in the assembly.
  14. Drag the part_3 and re-align it in the graphic window.
  15. Select the axis of part_1 and axis of part_3 to apply a coincident constraint between them.
  16. Drag the part_3 in the graphics window and apply a coincident constraint between its front datum plane and Front datum plane of the assembly.
  17. Now the component is fully constrained in the assembly.
  18. Place part_2 in the assembly.
  19. Rotate the part and re-align it.
  20. Select a predefined constraint named Pin.
  21. Select the axis of part_2 and axis of part_3 to apply a coincident constraint between them.
  22. Now click the Placement tab and define the reference of translation.
  23. The STATUS area indicates the Connection Definition is complete.
  24. Click the green check mark to apply and save the changes.
  25. Give away different colours to the parts of the assembly so that they can be recognized easily.
  26. Align the model in an isometric view using Re-orient tool.
  27. Clear the screen by closing the visibility of Datum planes, axis, points and everything else.
  28. Select the top face of part_2 and drag it with the help of Drag Component tool to check the mechanism of Hinge assembly.
  29. Only part_2 of Hinge can be moved because we applied a pre-defined Pin constraint on it.
  30. Re-generate the file and save it.