Siemens Nx Tutorial--Unified National Fine (UNF) Thread profile (Along with audio narration)

Hello viewers in this tutorial, we are going to create a Unified National Fine (UNF) Thread profile in Siemens Nx software. External and Internal profiles will be created separately. That would be used in creating Bolt and Nut which will be demonstrated later in another video.

 

Video Transcription

1. Start a new file using inch units.
2. Fill the name of the file UNF Screw External Thread Profile.
3. Create a new sketch over XZ plane.
4. Before starting the sketch we will set some preferences of the software.
5. Here in Drafting Preference under the text, set the decimal places of units to 5 and ‘Decimal Delimiter’ to the period instead of a comma.
6. Create a line and apply a dimension of 1/20 inches to it.
7. Apply a coincident constraint between the midpoint of this line and sketch origin.
8. Switch to Tools Tab and click over the ‘Expression’ command, here you can see the last dimension we applied over the line, named p0, change its name to Pitch which will be used as constant later.
9. Convert this line to a reference line.
10. Create two more lines in the sketch and apply a 60° angle between them.
11. We can see a vertical constraint has been automatically applied by the software between the intersection of newly created two lines and sketch origin.
12. Convert these two lines into reference line.
13. Create two more lines parallel to the previous lines as shown here.
14. Apply between horizontal constraints between the endpoints of these lines and convert them into reference lines.
15. Create another reference line and apply a horizontal constraint over it.
16. Apply a dimension of Pitch/6 over it.
17. In the same way, create another reference line collinear to the previous line on the other side.
18. Next add another reference line over here and apply a dimension of Pitch/8 over it.
19. Activate Arc tool and draw an arc tangent to these three lines and apply constraints as required.
20. Next, draw another arc coincident to the midpoint of this line and tangent to the adjacent line by applying constraints.
21. Mirror this arc to the other side using Mirror Curve tool.
22. Connect these arcs using lines to complete the sketch which we require.
23. Here we can see an auto dimension is still applied which means something is missing.
24. Fully constrain the sketch by applying a horizontal constraint over this line.
25. The sketch is complete so exit the sketch and save it.
26. Addition to this we need to create another Thread Profile for the Internal screw too, to do so, save as, this file with the name ‘UNF Screw Internal Thread’ Profile.
27. So we can see the file saved as for Internal Thread Profile is currently active next make some changes in the sketches.
28. Delete these sketches.
29. Change the value of this dimension to Pich/4.
30. Draw these lines using Profile Tool as shown.
31. Here apply a coincident constraint between the endpoints of the line which was not created automatically.
32. See the sketch is now fully constrained.
33. Chang back this reference line into normal line.
34. Our sketch is complete so exit from the sketching mode.
35. Save the file.

 

Visit the following link to get the model file…
http://autode.sk/2jt0hi8

 

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