Create a dome shaped part (Siemens-NX 10 Tutorial with Caption)

Serial No. 1

Create a dome shaped part (Siemens-NX 10 Tutorial with Caption)

 



Click the following link to get the model file: -http://bit.ly/31QVAA5

 

Transcription of Video
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1. Open the ‘dome.prt’ file.
2. Choose Isometric view from the Orient View Drop-down list.
3. Click the ‘Sketch’ icon on the ‘Direct Sketch group’.
4. In the Sketch Type group, select On Path.
5. Click anywhere on the lower spline to define the sketch plane.
6. In the Plane Orientation group, from the Orientation list, click the ‘Through Axis’ icon.
7. In the Plane Orientation group, click Specify Vector using the ‘Inferred Vector’ option.
8. Select the Z‐axis of the Datum CSYS.
9. In the Sketch Orientation group, from the Method list, select Use Curve Parameters.
10. To create the sketch, click the middle mouse button.
11. Click the ‘Restore Work View’ icon to return in previous view.
12. Make sure ‘Continuous Auto Dimensioning’ is disabled.
13. Create an intersection point on the upper spline.
14. Click the ‘Intersection Point’ icon on the ‘Direct Sketch group’.
15. Select the upper spline.
16. NX creates a point where the spline intersects the sketch plane.
17. Activate the ‘Line’ tool from the Direct Sketch group.
18. Select the upper Intersection Point and Point of Datum on Path.
19. Activate the ‘Arc’ tool from the Direct Sketch group and select the ‘Arc by Center and End points’ in the Arc Method option.
20. Click as shown to create the arc center point and end points.
21. Constrain the arc center to the Z‐axis, select the arc center and select the Z‐axis of the Datum CSYS and click Point on Curve.
22. Constrain the right end of the arc to the Z‐axis, select the datum axis and select the right end of the arc and click Point on Curve.
23. Construct a vertical line and horizontal line similar to the lines as shown.
24. Activate the ‘Rapid Dimension’ tool from the Direct Sketch group and place the dimension as shown.
25. Right‐click in the graphics window and choose Finish Sketch.
26. Activate the ‘Variational Sweep’ tool from the Surface group.
27. Choose ‘Connected Curves’ option on the Curve Rule drop down list.
28. Choose ‘Stop at Intersection’ option on the Top Border Bar.
29. Select the sketch geometry that you want to sweep, being sure to define the notch correctly.
30. If you have selected the wrong lines, shift‐click to deselect them.