Nosecone (page 3) | Onshape CAD Tutorial | Stage One Education

Finish the nosecone

in which we revolve a sketch

16. Start middle-of-nosecone sketch

Start a new sketch
Click the top face of your tube to start sketching on that face

Right click and select View normal to sketch plane to line up your view

17. Draw the middle-of-nosecone circle

Select the Use (Project/Convert) tool
Click on the outer circle

That line will bold, as it becomes part of your sketch

Draw another, larger circle, making sure to snap it to the center

18. Dimension the middle-of-nosecone circle

Select the dimension tool
Click your new circle's edge
Set the dimension to 0.781
Click the green check

19. Extrude the middle-of-nosecone

Select the extrude tool
Click on "Sketch 3"
Click on Add to add to your part instead of creating a new part
Set the Depth to 0.1 in
Click the "Opposite direction" button to make ring go down along tube
Click the green check

20. Start the cone sketch

Start a new sketch
Select the Front plane

Right click and select View normal to sketch plane to line up your view

21. Import lines to connect to

Select the Use (Project/Convert) tool
Click on the top of the larger circle
Click on the right side of the circle

Those lines will bold, as they become part of your sketch

22. Draw the nosecone

Select the "3 point arc" tool
Set the first point on the rightmost point in your sketch
Set the second point somewhere above your part
Set the third point so the arc looks like a nosecone

23. Constrain the arc

Select the "Tangent" tool
Select the arc
Select the line right below the arc, and you'll see the arc straighten to line up with that line

24. Draw top line

Select the "line" tool
Start: on the top of your arc
End: horizontal, to the center of the rocket

25. Offset nosecone lines

Select the "offset" tool
Can't find it? »
Try the Search tools feature, type "Offset" into the box.
Select the arc and the horizontal line
Drag the arrow to make the offset smaller than the arc
Press Enter and set the dimension to 0.05

26. Draw a line connecting to the offset

Select the line tool
Draw a line straight down from the outside to the inside of the nosecone

27. Constrain that line to be vertical

Select the "Vertical" tool
Click on the line from above
You should see that line turn black as it becomes fully constrained

28. Start dimensioning

Select the dimension tool
Click on the horizontal line and set its dimension to 0.15

29. Finish the nosecone sketch

Select the dimension tool
Click on the top line and then the bottom line and set the distance between them to 2.0
Click the green check

30. Revolve the nosecone

Select the "Revolve" tool
Select "Sketch 4"
Set the axis

Select the "Revolve axis" box
Select the tube

Click the green check

31. Fillet the top of the nosecone

Select the fillet tool
Click on the top ring of the nosecone
Set the radius to 0.10
Click the green check

You finished the nosecone!

It's now time to put together the assembly