ACCEPTED SOLUTION
Accepted Solutions
In both cases, the problem is the linear dimension that was auto-generated as you first made the section sketch. Then the trajpar relation will vary the angle but that linear dimension will go to 0 when trajpar=0 and that's when the section immediately fails - but Creo sure doesn't give you any clues as you have demonstrated in both videos.
So try instead of this:
Doing this:
and then applying the trajpar relation to the angular dimension:
-->
and then you should be able to go on from there:
Three things in your "test_file":
You need to select Variable Section
Your relation is for only 10° of rotation. Cange it to: sd3=trajpar*360*2 for 2 full rotations.
Third, your sketch dimension scheme is wrong. The distance dimension is to the vertical reference. The better option is a construction line between the center reference and the center of the circle.
this may not get you exactly what you want for a wire. Look at this discussion for a better way to create twisted wire: Creo Parametric Community Challenge 5 - Curves and... - PTC Community
You can control the twist using trajpar in a relation of a variable section sweep. Example model enclosed for review. The 36 constant represents the # of turns that will apply over the length of the trajectory. The first term in the relation "0" is the clocking angle used to define where the twist starts at the proximal end of the trajectory.
Hello @kdirth and @tbraxton - thanks for your responses.
@kdirth I tried to build it like you said but creo wont accept the condition. every time I set it up and press "ok" on the relation window there I put the relation trajpar... in, it wont accept it and reopens the window and yes, I chose the correct measurement. I changed it to variable section (I had it before too but there was an even worse outcome before I started this post so I switched back to constant section). Also the trajpar solution I copied out of the post with the stranded / twisted wires. Even with you relation it will not accept it. and the third hint, the construction line, was new so I made it as I understood but also no result. I attached the file, maybe you can test to fill in the relation.
Strangely the file "test_file..." which you attached, I couldn't open.and the linked post I will dive in deeper - I know this post and it will help me to understand it more I guess.
@tbraxton your solution works fine. I had not the time so far to rebuild it myself but the separation of the sweeps seems logic even though I would like to avoid the second sweep "spiral" as an reference for the main spiral of the "wire". When I want to introduce more than one spiral, it will turn into a "non-round" shape:
Is there any way to avoid this behaviour and to keep it round, all the way of the spiral?
Thanks in advance.
Your latest model has a horizontal constraint on the construction line; the angle is missing. Removing the horizontal constraint, adding the angle, and creating the relation, I get the following.
I only have access to Creo 7 and Creo Plus (running on Creo 12). I had to open your file in Creo 12, so the save file is Creo 12.
The distortion can be eliminated by sweeping a twisted ribbon and sweeping a solid along the outer edge of the ribbon.
In both cases, the problem is the linear dimension that was auto-generated as you first made the section sketch. Then the trajpar relation will vary the angle but that linear dimension will go to 0 when trajpar=0 and that's when the section immediately fails - but Creo sure doesn't give you any clues as you have demonstrated in both videos.
So try instead of this:
Doing this:
and then applying the trajpar relation to the angular dimension:
-->
and then you should be able to go on from there:
