Creating Realistic Knurling on the Cylindrical Surface-Siemens NX 10 Tutorial (with caption and audio)

Serial No. 17

This Siemens NX video tutorial demonstrates the way to create a realistic looking knurling on a cylindrical face in Siemens NX.……………………………………………………………………………………………………….

Note:-

To get faster update in feature pattern and better knurling change the following settings in Swept (10) feature:-

1. Turn on the ‘preserve shape’ option in the selection location field.

2. Change the orientation method of the sweep from ‘Fixed’ to ‘Face Normal’.

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The model displayed in video is used as a component in the assembly of Pipe Wrench created earlier by us.

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The modeling process of Pipe wrench which is available in two volumes, can be watched on following link... (1) https://youtu.be/8scpgSsermQ, (2) https://youtu.be/4o-ggjtTia4

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The video covers the application of 2D sketching, 3D features like Extrude, Wrap Curve, Swept, Circular Pattern, Subtract, Offset Face and Mirror Geometry.

Click the following link to get the model file: - http://bit.ly/356q6Z3
  

Transcription of the Video

1. Let us open ‘model4’ part file.
2. Go to the feature panel and choose ‘Datum Plane’ command.
3. Select the cylindrical surface of the part and then click OK.
4. Create a new sketch on this datum plane.
5. Right-click in the design window and choose ‘Orient View to Sketch’ option, or choose the F8 key on your keyboard.
6. Draw a slant line and apply midpoint constraint.
7. Make an angle 30 degree between X-axis and line.
8. Apply the linear dimension 0.4167” between Y-axis and endpoint of the line.
9. Finish the sketch and back to the Isometric View.
10. Go to the Menu button > Insert > Derived Curve and activate the ‘Wrap/Unwrap Curve’ command.
11. This time ‘Wrap’ option is selected by default under the ‘Type’ area.
12. Select the line and choose ‘Select face’ option, then select the cylindrical face of the model.
13. In the ‘Specify Plane’ option, select the ‘Datum Plane (5)’ in the design window.
14. Click Apply button to finish the command.
15. Hide the Datum plane and sketch both to watch the effect.
16. The sketch is wrapped on the cylindrical face of the model with the help of ‘Wrap Curve’ command.
17. Apply the chamfer both side of the cylinder.
18. Save the model file.
19. Create a new sketch over the YZ Plane and apply the section view.
20. Create a triangle with the given dimensions.
21. Apply the constraints to place in proper position.
22. Finish the sketch and return back from the section view.
23. Choose isometric view and save the part file.
24. Go to the ‘Surface’ tab and activate the ‘Swept’ command.
25. In the ‘Sections’ option, select the triangle in the design window.
26. In the ‘Guides’ option, select the guide rail.
27. Click OK to execute the command.
28. Triangle is wrapped on the path of guide rail by the help of ‘Swept’ command.
29. Go to the Menu button > Insert > Offset/Scale and activate the ‘Offset face’ command.
30. Set a suitable offset value and apply in the front and back face of triangle.
31. Click OK, now the face is extended both side of the cylinder.
32. Activate the ‘Mirror Geometry’ command.
33. Mirror this feature with respect to XZ Plane.
34. Activate the ‘Subtract’ command.
35. Select the target body as a main body (cylinder) and afterward select triangle as a tool body.
36. Click OK to observe the result.
37. Go to the ‘Feature’ panel and activate the ‘Pattern Feature’ command.
38. In the ‘Layout’ section, choose ‘Circular’ option.
39. In the ‘Feature to Pattern’ section, select the ‘Subtract (14)’ feature from the Part Navigator bar.
40. In the ‘Rotation Axis’ section, select the X-axis.
41. In the ‘Specify Point’ section, click the point dialog button and click OK.
42. In the ‘Angular Direction’ section, choose ‘Count and Span’ option.
43. Set the Count Value 70 numbers and Span angle 360 deg.
44. Click OK to finish the Pattern Feature command.
45. Now see the result, pattern feature is created.
46. Follow the same procedure as we have done earlier on the opposite side of the Mirror Geometry feature.
47. Save the part file.