I am designing a piece and the shaft of it needs a 1.5 degree angle on it

[EH_8300888]

I am designing a piece and the shaft of it needs a 1.5 degree angle on in while keeping one side straight and I've done what I know but I was wondering if there was a different way I could actually use the angle instead of what I've got in the pictures. Or if there's any easier way to do this I would appreciate any help I can get thanks.

I am on Creo Version 9.0.1.0

[tbraxton]

Using the variable section sweep is a good way to model this IMO. It is efficient; using one feature to define the geometry. You may want to consider using part relations to drive the VSS sketch relations in trajpar as a function of the desired angle. This would support the designer setting the angle directly and using some trigonometry to derive the trajpar sketch relations.

[EH_8300888]

so is there a way to use an angle instead of two different diameters in the part relations 

[tbraxton]

I am making the assumption that you know the diameter at the start of the taper and the length of the taper in addition to the angle of the taper. If this is not the case, then describe what inputs you want to use to drive the design.

You have a right triangle when viewing the section along the taper from the proximal to distal end. Assuming you know the diameters of the taper at the proximal end, the length of the taper, and the desired angle before creating the VSS feature then you can use trigonometry to calculate what R2 (@ distal end) must be and use these values by passing them to the VSS feature sketch relations from the part relations.

You can see below that you can use a right triangle to solve for the values needed to drive the VSS sketcher relations.

[EH_8300888]

I am using a .25" start diameter its .75" long and it has a 1.5 degree angle on it

[KenFarley]

You could define a parameter for the angle, then use that angle, the tapered protrusion's length, and one of the diameters to calculate the other diameter. Just be sure to check the resultant angle to ensure you've got the math right and are conceptually correct.

[kdirth]

A swept blend may be a good option depending on the design intent.

Create a sketch to define the path:

I used the horizontal line as the trajectory and the angled line to set the diameter.

[kdirth]

Creo 7.0 attached.

[ByDesign]

For me, using that kind of sketch, it has always been easiest to break these pieces in half.  It looks like there is a plane of symmetry, so build one side, then mirror it.  Make your angle dim be the driver of the variable section (going from 15 to 0).  However, the approach might not be the best if you have to use a bunch of math -- But, if the cross section of the shaft doesn't really matter, then go for it.

On the other hand, if you need to maintain a circular cross section, I'd sweep the base circle to the profile trajectories.  (One straight, and one with the angle.)  Because of the hiccups PTC has always had with circles, again, you might do it with a half circle so you can attach the vertices to the trajectories.  Mirror it for the other side after.

I like variable section sweeps, but they do have limitations in control of the mid-sections.  Sweeping around the circles will give one result, and sweeping a circle along a liner set of trajectories will give a slightly different result.  Build the feature so you have control over the things that are important to you.

Good luck.

[pausob]

I'm thinking to construct a side-sketch that specifies the protrusion's length, diameter(s) / taper angle:

Then use that sketch curves as the basis of a 2-rail variable section sweep:

Note: add the 2nd rail (chain 1) by holding ctrl + clicking

The cross-section is a circle that needs to touch the 2 rails:

[Pettersson]

Yet another way is to make a datum plane with a 0.75 degree angle and use that as the pull direction for a 0.75 degree draft feature. This will cancel out the angle at one side, while doubling it to 1.5 degrees on the other.