Creating a sweep, cut along a curve WF 3.0

[tazengr]

Hello,
I am trying to perform a simple cut operation that has myself and a few other Pro/engineer Wildfire 3.0 users stumped. So I figured I would give this forum a try.

Basically I would like to cut constant section groove along a profile into my part.

First: I define the curve that is going to be the profile of the cut by doing the following.

Insert--> Model Datum--> Curve..
Then I select From equation and define the curve using Cylindrical Coordinates by defining
r = .5
theta = t*120
z = .280*t
where Pro/E defines t as varying from 0 to 1.

Then I end up with the curve I am looking for (curve that is a third of a circle that travels .280 in the z direction)

No problems so Far

Second: I attempt to perform the Cut along this path by the following steps:

Insert--> Sweep--> Cut...

Then the drop down menu asks me to select or sketch the trajectory, Section, and Material Side. However I can't even get past the Trajectory question which asks me to either select or sketch a trajectory.

So of course I would like to select it, but for some reason Pro/Engineer replies with this message: "Specified trajectory is not valid. Please reselect."

Can someone tell me why the trajectory I created through the equation is invalid to Pro?

Thanks,

TAZ Engr

 

[jeff4136]

A trajectory for Insert -> Sweep needs a section XY
orientation reference which doesn't exist as the curve
is not associated with a datum plane, surface, solid
face, etc.

There are several ways you could get to where you want
to be. Project your existing curve to the cylindrical
surface and use the resulting curve as a Sweep traj,
use a Helical Sweep, Wrap a planar curve on the
cylinder, ... Whatever you use; don't make the
assumption that your section XY orientation is correct
unless it's controlled and the control is understood.
A VSS using your existing curve as a traj may fool you.

(If it matters; also don't assume sweeping a planar
area section along a non-planar trajectory will give
you a good rep of the intended geometry.)

-Jeff Howard (wf2)
Sure it's true. I saw it on the internet.

 

[cadcamguy]

Another way is to make another curve just use the same equation and change the R value,then use a VSS.. using the other curve as your x-traj.

 

[tazengr]

thanks for the responses.
I have decided to go with a variable section sweep.
However I can only add material when I do this. Is there a way to use this feature and remove material?
Because I have not seen the remove material button anywhere.

 

[tazengr]

Disregard the previous post I found out how to remove material.
However, now the problem is that the section is not the same. I would like to cut out a section that has a rectangular shape. It starts out that way but by the time it gets to the end of the cut the section becomes triangular????

Is there a way to keep it a rectangular shaped cut through the entire length of the profile.
Thanks,
TAZ ENGR

 

[mjcole]

If You use a swept blend using 2 rectangular sections you can get rid of the twist.

Or add a another curve as your X direction reference and use XY cross hairs in Sketch for constraints to guide your Section. A Projected curve usually works well for this purpose.

Michael

 

[mjcole]

http://files.engineering.com/getfil...ed5f6027639&file=wf_VSS-control-alignment.PNG