How to model a knurled surface in Creo Parametric

This is an example of how to model a knurled surface in PTC Creo Parametric. This method will allow you to create a knurled surface fully dependent on the geometry of an initial cut that will rebuild fully with any subsequent changes i.e. changing the profile won't create regeneration errors.

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1 Answer

1. Create a new part
2. Sketch a circle on the top plane
3. extrude it upward
4. Select the "helical Sweep" tool from the search bar
5. Select "define section" from the feature manager
6. Select the "front" plane as your work area
7. Place a center line along the center axis of your cylinder
8. Place a line with one point coincident on the cylinders edge, ending beyond the other end of the cylinder
9. Select the "define profile" button from the top left of the toolbar. It looks like a pencil.
10. Sketch a triangle pointing inward towards the center-line of your cylinder. Dimension it as required. The vertical edge should be co-linear with the edge of the cylinder and coincident with the beginning of your helical sweep section sketched earlier.
11. Select ok.
12. Define the pitch as equal to the height of your cylinder .
13. Select the remove material option.
14. Select ok.
15. Click the helical sweep feature from the feature tree and select "geometry pattern"
16. Select "axis" as the pattern type from the drop-down menu
17. Select the center axis as the axis of rotation.
18. Select the number of instances and spacing you would like.
19. Click ok
20. Create a plane that is half the height of your cylinder
21. Select both the original helical sweep and the pattern feature from the feature tree.
22. Click "mirror"
23. Select the plane that divides the cylinder in half
24. Click ok
25. The fully knurled surface should be complete

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