Hi everyone,
I am very new to Inventor and need some experienced opinion on the problem that I am facing with the following idea:
Basically I have this column created with revolve and I would like to place these grooves on it like on the following example created with Coil:
I would like to preserve the number of grooves at the base and for them to "compress" accordingly at the narrow middle section of the first column. I tried accomplishing this by creating a new 2D sketch at the base of the column, but it wouldn't let me edit the base circle for the grooves to become "coilable" if you know what I mean. What am I doing wrong and is this the correct way of attempting to implement this idea?
Solved! Go to Solution.
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Solved by JDMather. Go to Solution.
Something like one of these images?
I prefer to use a Coil Surface to create the curve as much easier to edit.
See attached example.
Hi again,
I tried implementing your suggestion today, but I run into "axis intersects profile" error when trying to coil round that column. Any advice? Thanks.
@Broomanyollo wrote:
... Any advice?
Attach your *.ipt file here.
Also, do you think Inventor is the best software for this sort of geometry as it honestly feels quite unintuitive when creating such features?
iProperties would seem to indicate that you have not installed Service Packs 1 and 2 and Update 3.
You are missing a dimension and constraint in Sketch1?
Yet when I add the missing dimension - it is perfect! What happened to the missing dimension?
For Sketch2 I would change the circle to Construction linetype and I would create a construction line to constrain the normal line at the midpoint.
Going back to your Sketch1 - I do not see a logical reason for using a Spline in place of a simple Arc?
The difference between the two would be less than the thickness of a sheet of paper?
Using this logic - attached is my Sketch1.
Note: No repeated dimensions.
Note: In my Sketch2 the Projected construction line and the normal line to midpoint (turn off Visibility of Sketch1 to see).
I am not sure how this would be done any more logically or "intuitively" in any other CAD program?
Once the parametric coil geometry is created - it is easy to get the 3D intersection curve for Sweep path.