Revolved Boss Question

The journey continues; starting to work on the Revolved Boss/Base function.

I can define a centerline, I can use sketch to outline a complex cross-section, then use the Revolved Boss to rotate it around the centerline to form a circular object.

Whoops. My sketch was 1/2" too far from the centerline; the diameter of the revolved boss object is an inch too much. The same centerline is used for another object, so I don't want to move it.

Is there an easy way to move the whole sketch closer to the centerline? Hate to have to redefine each individual sketch point's location.

Ron Wanttaja

There are a couple of ways but it sounds like you didn't dimension the profile sketch to the rotational axis for some reason so that's the direction I would go.

First, pick something in the profile to use as a reference for all the other geometry. I did this on my version of your sight model;

Attachment 7659

Attachment 7661

The profile is fully defined and the reference point is horizontal of the origin (I added a horizontal centerline from the origin the illustrate this). The .250 vertical line defines the outside face of the profile and is dimensioned as a diameter from the vertical centerline at the origin. In the second image I edited the 4" diameter to 3.5" to move the profile closer to the vertical C/L which is the rotational axis.

Quote:

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Originally Posted by cwilliamrose

....The profile is fully defined and the reference point is horizontal of the origin (I added a horizontal centerline from the origin the illustrate this). The .250 vertical line defines the outside face of the profile and is dimensioned as a diameter from the vertical centerline at the origin. In the second image I edited the 4" diameter to 3.5" to move the profile closer to the vertical C/L which is the rotational axis.

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OK, thanks. I think the fundamental problem is that I did know how to use the smart dimensions to define a distance OUTSIDE a given sketch (e.g., define the distance to the separate centerline). Fiddling around, it looks like it's a control-click.

I was able to define the radial dimension from the vertical centerline to the midpoint of one of the structure lines. With this ability, what's the significance of a separate designated "Reference Point"? Also, when I create one, it just puts text next to the point...not separately with a line and arrow. Am I creating the wrong kind?

Thanks again. Lemme get this one figured out and I'll get out of your hair. :-)

BTW, the specific project that triggered this question wasn't the sight, it was to build an adapter to use a 1 3/4" shop vac nozzle on a 1 1/4" hose. Sure, I could have just returned it to Amazon, but couldn't resist designing a PRACTICAL object....

Ron Wanttaja

The reference point I noted above was my attempt to show where the profile was being located relative to the axis of rotation and the origin. It's being used as the anchor point for the profile. If you think of that profile it's like a sub-sketch and it is fully defined within itself. The only thing it needs is an X-Y location to lock it into place. If it was not constrained horizontal to the origin and that 4" dimension wasn't there all the entities in the profile part of the sketch would be blue and you could drag the profile around the sketch (it would retain it's shape and size). Adding the 4" dimension only would result in being able to drag the profile up and down but not left and right. Once you have defined an X-Y location for any point in the profile all the entities will turn black and you would not be able to move the profile in any direction by dragging.