Sweeps

In my on-going quest to build AN fittings, I have a need to build sweeps tha follow a curve. Try as I might, I cannot draw a curve that is normal to the plane of the entity I want to sweep. The curve is always parallel to the surface of the entity. Obviously, I am missing a very important conceptual idea, but I cannot determine what it is. I thought perhaps changing which plane I begin the sweep from might affect it, but so far, I am not able to do it. Any help or amazing insights will be greatly appreciated.

In general the sweep path starts at a point on the sweep profile plane, and the start of the path is usually (note usually) perpendicular to the profile plane. So, you can draw the path curve in two ways:
1. On a plane that is perpendicular to the profile plane draw a 2D sketch that includes a curve that starts at the start point and whose tangent is perpendicular to the profile plane, or
2. draw the path in a 3D sketch in such a way that the tangent to the path curve at the curve start point is perpendicular to the profile plane.

Am I making sense, or have I confused you more?

Let me see if I am even close to understanding this - if I want the curve to follow (or be drawn in) the front plane, I need to select a plane perpendicular to it ( say, the right plane ) and draw my curve there. Then, when I select the entity, the sweep will be in the front plane?

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Originally Posted by Hstaton

In my on-going quest to build AN fittings, I have a need to build sweeps tha follow a curve. Try as I might, I cannot draw a curve that is normal to the plane of the entity I want to sweep. The curve is always parallel to the surface of the entity. Obviously, I am missing a very important conceptual idea, but I cannot determine what it is. I thought perhaps changing which plane I begin the sweep from might affect it, but so far, I am not able to do it. Any help or amazing insights will be greatly appreciated.

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Post your part in Dropbox or somewhere we can get to it, so we can look at what you are doing. Then post the link to the file here.

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Originally Posted by Hstaton

Let me see if I am even close to understanding this - if I want the curve to follow (or be drawn in) the front plane, I need to select a plane perpendicular to it ( say, the right plane ) and draw my curve there. Then, when I select the entity, the sweep will be in the front plane?

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Yep - You sketch the profile on the right plane and then the path curve in the front plane - just make sure the start point of path curve is also on the profile plane (right plane).

Quote:

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Originally Posted by Hstaton

Let me see if I am even close to understanding this - if I want the curve to follow (or be drawn in) the front plane, I need to select a plane perpendicular to it ( say, the right plane ) and draw my curve there. Then, when I select the entity, the sweep will be in the front plane?

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Pictures are easier to understand :

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Originally Posted by Jeffrey Meyer

Yep - You sketch the profile on the right plane and then the path curve in the front plane - just make sure the start point of path curve is also on the profile plane (front plane).

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SolidWorks Help explains it better than I ...

A few thoughts on sweeps, regardless of Boss/Base or Cut which I wasn't clear on from original post, with intent of design flexibility and stability:

Regarding planes used from questions in post #3, I avoid using primary planes for profile. I'll explain why:
Anytime that I create a sweep, I generate the path first. It is rarely flat 2-dimensional, so normally a 3D Sketch. Then, at one end of the path, I create a reference plane and rename it (Profile Plane1, etc.) to associate it with the sweep feature I'm about to create. Specifically, I create the profile reference plane by selecting an end point and its line/arc/curve/spiral then creating the plane from that. With endpoint and attached sketch entity, the plane generated is defined as perpendicular to the sketch entity and coincident with the endpoint. For flexibility and stability, the reference plane can move with the path if its constraints (i.e., location, orientation) are altered, instead of relying on primary planes. The Pierce relationship to the path sketch is key to add in the profile sketch, if you want it to remain with its reference point, and stay fully defined. As demonstrated above, these constraints are not necessary to begin with, but do allow for more dynamic use, variations, and alterations.

One benefit of renaming planes you create is that both profile and path sketches will be absorbed, thus moved to within the expanded tree of the feature. At any time in the future, if you wish to refer to or alter either one, it is useful to name them to distinguish. It saves the brief examination of which is which by selecting and seeing if this was the one you're after. Ref. Planes do not get absorbed, though, so generally precede a sweep feature in the design tree. Naming those keeps things straight in language as well as its vertical tree parent/child relationship.

I mentioned spiral above. The Helix/Spiral tool is great for defining threads or springs as features. It can handle tapers and other variables. It gets treated as a 3D Sketch, so it is similarly absorbed by features that are defined by it, and can be shared to other features by expanding the 1st feature that absorbed it.

Finally, if generating a Swept Cut, I've learned to start the path away from the object instead of abruptly beginning its cut at an awkward angle located at the edge of the body. This results in a feature similar to physical tooling of taps, by imagining the complete path of the tool instead of its logical but troublesome start-here condition.

SUCCESS! It is a marvelous thing. Thanks to all of you for helping me make this jump! It had everything to do with angles. I was able to make two successful sweeps today, and it feels marvelous!