Autodesk Inventor - How to cut Irregular Helical Groove
See tutorial below
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Step 1:
[1]
Create 2D sketch:
- when entering the height: hhh=200 in text box
- select any dimension > right-click > dimension properties > Document Settings tab: Select "show Expression" in Modeling Dimension Display
- this is to be able to see which dimension has got what label (name); e.g. dia = d3 & height is hhh [as shown by the red arrows]
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Step 2:
[2]
Create 3D skecth:
- helical curve
- pitch&height
- "d3" in diameter
- "hhh" in height
- "3.142*d3" in pitch (45deg slope = 1 revolution = 1 pitch)
- rotation direction as required
- (1) pick bottom point of 2d sketch centerline
- (2) pick top point of 2d sketch centerline
- (3)then the end of the base line
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Step 3:
[3]
Create workplane for swept surface:
- new workplane
- pick 3d helix
- pick endpoint
-
Step 4:
[4]
New 2d sketch:
- pick workplane
- right-click > "new sketch"
- project geometry > point
- draw horizontal line (line must intersect surface of vase when swept: therefore from centerline out past solid)
-
Step 5:
[5]
Sweep:
- surface
- profile
-
Step 6:
[6]
Revolve Solid:
- revolve
- pick axis
-
Step 7:
[7]
3d sketch for swept cut:
- create 3d sketch
- intersection curve
- (1) select helical surface
- (2)(3) select vase (all surfaces)
-
Step 8:
[8]
Switch off unneccesary surfaces/workplanes
-
Step 9:
[9]
Ceate workplane on end of new 3d sketch:
- new workplane
- helix
- endpoint
-
Step 10:
[10]
New sketch to be cut from solid:
- pick workplane
- right-click > new sketch
- project point
- draw circle
-finish sketch
-
Step 11:
[11]
Swept cut:
- (1) sweep
- (2) cut
- (3) path
-
Step 12:
[12]
Circular array:
- (1) Circular
- (2) select sweep feature
- (3) Axis > (4) select vase solid
- (5) 12
-
-
Step 13:
[13]
Finished product
