sweep cut creo vs solidworks

[asifcad]

hello, I am stuck on cutting this profile on the sphere by sweep command but another hand in solid work this cut feature is so simple just like 123 and done... I need to know how to make this cut in creo...please check the pic and video

https://www.youtube.com/watch?v=Mpd3U3dI2BU&t=9s

time at 7:00 to 8:00 minutes.

[tbraxton]

There are two options in Creo that come to mind to twist the profile for a sweep. From the video it appears that a variable section sweep should match.

1) Variable section sweep using the trajpar parameter to control the twist of the profile along the length of the trajectory.

About the Trajpar Parameter

2) Helical sweep feature

[kdirth]

I agree with @tbraxton, the variable section sweep using the trajpar variable is the way to go.  Can be accomplished just as fast as the processes in the video.

[kdirth]

3 features:

[asifcad]

Can you please share the model you mentioned in your post or any example video related to this command? 

[tbraxton · Accepted solution]

PTC tutorial for use of trajpar with VSS.

Use Trajpar with Solid Features | Tutorial | PTC Learning Connector

You need an angle dimension in the sketch of the sweep that controls the "clocking", use this dimension in the sketch relation inside the variable section sweep. The relation would be sd#=180*trajpar. This will twist the sketch from 0-180 degrees along the length of the trajectory.

Here is how it is used to twist a ribbon through 180 degrees.

Example sketch:

180 degree twist of the above sketch

[kdirth]

Creo 7.0 attached.

[asifcad]

thanks, brother it really helped to understand the approach