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M
Model_197512-Amethyst
12-Amethyst
April 28, 2025
Solved

Stranded Wire over a Curve

  • April 28, 2025
  • 3 replies
  • 1989 views

Hello,

 

I need help or some recommendations. Creo is testing me once again and I am almost giving up.

 

I would like to design a stranded wire over a curve. I tried myself but it was too complex and not as smart as your solutions. So I wanted to try the solution from this topic: Help modeling a stent - PTC Community

I also found this: How to create Twisted wires - PTC Community

The second link is more suitable for what I need so I tried the trajpar function but it did not went as well as in the topic.

 

I drew the curve in one plane. After this I sketched a circle on an angled centerline going through the start point, then I defined the angle dimension using a relation in sketcher - like it was written in the topic but it seems as it cannot be that "easy".

 

Could you maybe tell me, what I did wrong or where my mistake is? Attached you can find the test file, rough a example of what I want to achieve (looks wise) and my straight version which maybe can be converted into a bend version...

 

I use creo 9.0.4.0. - Thanks in advance.

 

Best answer by pausob

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:

pausob_0-1746455772822.png

 

 

Doing this:

pausob_5-1746455948355.png

 

 

and then applying the trajpar relation to the angular dimension:

pausob_2-1746455820296.png

 

-->

pausob_3-1746455833294.png

 

and then you should be able to go on from there:

pausob_4-1746455865766.png

 

 

 

3 replies

kdirth
21-Topaz I
kdirth21-Topaz I
21-Topaz I
April 28, 2025

Three things in your "test_file":

 

You need to select Variable Section

kdirth_0-1745852325814.png

 

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.

kdirth_1-1745853055162.png

kdirth_2-1745853077460.png

kdirth_3-1745853202802.png

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

 

 

There is always more to learn.
tbraxton
22-Sapphire II
tbraxton22-Sapphire II
22-Sapphire II
April 28, 2025

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.

tbraxton_1-1745854663166.png

tbraxton_0-1745854972457.png

 

 

 

 

 

 

M
Model_197512-AmethystAuthor
12-Amethyst
April 30, 2025

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: 

Model_1975_1-1745993360662.png

Is there any way to avoid this behaviour and to keep it round, all the way of the spiral?

 

Thanks in advance.

 

 

 

kdirth
21-Topaz I
kdirth21-Topaz I
21-Topaz I
April 30, 2025

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.

kdirth_0-1746015002329.png

kdirth_1-1746015028629.png

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.

 

There is always more to learn.
kdirth
21-Topaz I
kdirth21-Topaz I
21-Topaz I
April 30, 2025

Here is an example of the ribbon method created in Creo 7.

kdirth_2-1746016209562.png

 

There is always more to learn.
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