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Help! Can't sweep an intersect curve?

njensen
1-Newbie

Help! Can't sweep an intersect curve?

Hi!


I'm in a situation where i want to model a torsion spring with an intersect curve for a special reason.

But i can't make CREO complete the sweep feature, only if i choose: Automatic under Horizontal/Vertical control and that ends up in a twisted cross section through the curve which is not want i want to achieve.

Can anybody tell me whats wrong? I have attached the part file with this message.

Best regards

Nicolai


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1 ACCEPTED SOLUTION

Accepted Solutions
TomD.inPDX
17-Peridot
(To:kdirth)

The logic to letting a sweep like this use the trajectory as normal so that your section is the same as the raw material.

In the case of round wire, you don't see twists, but when you go to square stock wire (typical of magnet wire for high current transformers) you need to manage rotation along the origin.  Using an offset curve as a reference lets you manage the rotation.

I suspect that if you were to use a round wire without rotation control, you might send Creo analysis for a loop.  This is one area that is not obvious to many nor critical to others.  However, I did see "knots" in a helical sweep in the past and that was a s/w bug.  Again, not sure if it is really fixed but it was reported fixed.  The knot was at every "end" of a 360 degree sweep and they were not continuous.

View solution in original post

20 REPLIES 20
dschenken
21-Topaz I
(To:njensen)

Check out One method to make wound springs. There are others, but I wrote this one.

What I find is that if picking a horizontal/vertical reference causes the sweep to fail it is because at some point along the sweep the direction makes no sense. For example, if a plane is selected as the orientation reference and some part of the spring is perpendicular to the plane.

What do you mean by "the sweep the direction makes no sense"?

dschenken
21-Topaz I
(To:njensen)

Where there is a place where a horizontal reference doesn't determine a horizontal direction.

You skip all of those problems with graph driven curves. If you need control of orientation, then add a second curve that has an increased radius as the reference.

Graph driven curve? Graphs are 2D? And what do you mean with a curve with a radius? I tried making a similar curve which is offset in the radial direction relative to the current curve and it didn't help.

dschenken
21-Topaz I
(To:njensen)

It's explained in the link I provided.

That method is not possible to apply in my case? Because of the hooks at the spring ends

dschenken
21-Topaz I
(To:njensen)

Add the hooks separately. The ends of the graph can do everything but the last turn.

If you post a picture of the spring you want then I can be more helpful.

I uploaded the part file with the intersect curve, but here are some pictures of the curve:

Torsion_spring.jpg

I want to sweep a rectangular cross section along the curve. The reason why i want to create the spring with a continuous curve is because it has to fit in a top down assembly design driven by a skeleton. Also, to obtain better simulation results in Abaqus, it's necessary to have tangency everywhere no edges in the curvature, and it can be difficult to add the hooks with tangency to a helical sweep.

If you are doing anything other than a round wire, you probably want to use a reference curve parallel to the origin curve.  Depending on how the master curve was made, it can have a twist in it that you can only see with analysis.  The reference curve can be used to manage orientation along the sweep.

Also, what version are you using?  These is a bug as long ago as Creo 2.0 M040 that causes errors at every 180 degree of the turn.  It was reported fixed but never verified it or know which version fixed it.  You will see it with a comb analysis as a "knot".

dschenken
21-Topaz I
(To:njensen)

Notice the direction reversal. Very much like the hook you want. Since you are using rectangular wire, you'll need a guide curve which will have a similar graph set, probably just needs a radial offset.

Helical sweeps can not correctly model springs, particularly at the ends, where you have problems.

Also - not everyone is on the same revision, same license, or has immediate access to software required to open files that are posted. Posted files require others to have to download the file, open the related software, and then open the file. In my case, I am not going to use my employer's software for non-work related purposes.

Thanks for the help guys. I don't remember the specific CREO version I'm using at work, but it's CREO 3.

I'll try to investigate how to sweep with a guided curve and see what happens, I'll return when i have tried.

Is this something like what you are trying to get.  I found that removing the horizontal and vertical constraints was necessary to remove warping.

Capture.JPG


There is always more to learn in Creo.
TomD.inPDX
17-Peridot
(To:kdirth)

The logic to letting a sweep like this use the trajectory as normal so that your section is the same as the raw material.

In the case of round wire, you don't see twists, but when you go to square stock wire (typical of magnet wire for high current transformers) you need to manage rotation along the origin.  Using an offset curve as a reference lets you manage the rotation.

I suspect that if you were to use a round wire without rotation control, you might send Creo analysis for a loop.  This is one area that is not obvious to many nor critical to others.  However, I did see "knots" in a helical sweep in the past and that was a s/w bug.  Again, not sure if it is really fixed but it was reported fixed.  The knot was at every "end" of a 360 degree sweep and they were not continuous.

Patriot_1776
22-Sapphire I
(To:njensen)

Frankly, I never use helical sweeps, for anything.  I either use datum curves driven by graphs, or I wrap curves.  I feel i have far more control over the outcome.

I found out how to create the model another way, by leaving the helical sweep as a feature and making the hooks after that.

But now when you guys mention this guided curve option. How do i do that? I can't find out how en CREO and i can't find a guide either.

Thanks for the help so far! 🙂

This post has a lot of relevant information.

Technically, an equation curve can be duplicated with a slightly larger or smaller R value.

This also covers what to look for in your version to see if it creates knots.

Another equation curve approximation error

Need more info and probably should start a new port.

I'm thinking a cabernet blanc would go better than port. Each to his own.

Ha!  Post!   

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