Tutorial: Wooden snail with variable coss-section

Here is what I came up with. did it the way Jeff suggested by doing a cut-sweep along a helix.

Answer: "Wood snail"

  1. Step 1:

    open a sketch on top plane and make a square.

  2. Step 2:

    extrude the square up to make a cube.

  3. Step 3:

    add fillets

  4. Step 4:

    Make this sketch on the front plane and make the bottom horizontal line colinear with the top of the cube and the left verticle line verticle to the origin.

  5. Step 5:

    do a revolve.

  6. Step 6:

    select the flat face on the top of the revlove and convert entities. this will be the circle we use to make a helix.

  7. Step 7:

    create a helix using the circle. I adjusted it untill it look correct acording the pictures I was trying to duplicate. Make sure the start angle is set to 0 as this will make thing easyer in later steps.

  8. Step 8:

    select the top face of the revolve and open a sketch. use the offset entities to make a circle larger then the flat face.

  9. Step 9:

    take this sketch and do a boss extrude in two directions. one as tall as the helix and the other to the round surface of the revolve.
    ***Be sure to un-check the merge results. We will merge the two bodies in a later step.

  10. Step 10:

    create a fillet on the front plane and add a point to the right side of it. Pierce this point to the helix. This is why we want to start the helix at 0 deg.

  11. Step 11:

    do a cut sweep with the circle and the helix

    *** be sure to go to geature scope and select only the upper cylinder to cut. That is why we wanted two bodies.

  12. Step 12:

    in the upper part of the feature tree there should be a folder that says you have two bodies, open this and select the bodies and a window should come up with a combine icon. use this to make one body. I am not sure where this is in the ribbon.

  13. Step 13:

    add fillets to the edges on either side of the cut sweep. I adjusted this as large as I could to get it to look smooth and rounded.

  14. Step 14:

    on the face at the top the spindle, open a sketch and make a circle centered on the origin and just large enough to cover the profile.

  15. Step 15:

    extrude in two directions.

  16. Step 16:

    on the front plane, make a sketch of a circle and pierc the center of the circle to the bottom edge of the extrude. make sure the top of the circle meets the sketch of the extrude.

  17. Step 17:

    do a cut sweep (you may need to make the sketch from the extrude visable to be able to select it for the path.

  18. Step 18:

    Add a fillet

  19. Step 19:

    on the top face open a sketch and make a square. I added a mate to the base cube instead of adding dimensions.

  20. Step 20:

    extrude the square up.

  21. Step 21:

    Create this sketch on the front plane. there is a verticle construction line is verticle over the origin and will be used for the axis of a revolve cut. The 175 is the diameter of the upper arc. I had to adjust this sketch a few times after the revolve cut to achieve the desired results.

  22. Step 22:

    do a cut revolve using the verticle construction line as the axis of revolution.

  23. Step 23:

    The revolve cut creates an undesirable space. Select this face and convert entities. This makes a circle to extrude.

  24. Step 24:

    Use the circle sketch and extrude to surface.

  25. Step 25:

    add fillets

  26. Step 26:

    Here is the completed feature tree.