×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

How to make a helix follow a curve in UG NX4!

How to make a helix follow a curve in UG NX4!

How to make a helix follow a curve in UG NX4!

(OP)
Hi there all,

I am trying to get a spring to follow a curve in UG NX4 but the helix function only allows me to create a straight spring.

Can anyone please advice how to get this helix to follow a curve?

Cheers in advance

Chris.

RE: How to make a helix follow a curve in UG NX4!

(OP)
Thanks I will take a look.  

RE: How to make a helix follow a curve in UG NX4!

(OP)
Hey there.

This is good start but how do I get it to follow a spline?  

RE: How to make a helix follow a curve in UG NX4!

I don't have NX4 so I cannot post an example but this is how I would do it.

First create the spline you want to follow.  Then create a line segment at one end of the spline, perpendicular to the spline and with the length equal to the helix radius.  Then create a swept feature using the line as the section and the spline as the guide and choose "Angular Law" as the orientation method.  Law type should be linear, starting at zero and ending with a value of the number of coils*360.

See attached picture.
 

RE: How to make a helix follow a curve in UG NX4!

(OP)
Thanks. Seams simple when you put it like that.

RE: How to make a helix follow a curve in UG NX4!

Simon,

I remembered this from an earlier thread, searched but couldn't find the thread.  Would have saved me a bit of typing and creating a new model.

RE: How to make a helix follow a curve in UG NX4!

Any time someone posts a model (useful ones and even ones that need work) I save them off into a folder for future reference, even if the thread is of no particular interest or I have not replied, you would be surprised how useful and how much I have learnt from doing so.  smile

Best regards

Simon NX4.0.4.2 MP10 - TCEng 9.1.3.6.c - (NX6.0.3.6 MP2 native)

www.jcb.com

Life shouldn't be measured by the number of breaths you take, but by the number of times when it's taken away...

RE: How to make a helix follow a curve in UG NX4!

Hi all,

I am trying to create a helix so that the circular ends are flat to parallel surfaces, does anyone know how to do this?

Cheers for any help

RE: How to make a helix follow a curve in UG NX4!

HollyT,
Unless I have misunderstood the question, you would set up the WCS so that the X direction is parallel to your surface and then make the number of turns a multiple of 0.5. Or you could create an arbitrary helix and trim the ends appropriately.

RE: How to make a helix follow a curve in UG NX4!

You mean as in a compression spring with what is called a 'Closed' end (or perhaps even a 'Closed and Ground' end)?

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.
 

RE: How to make a helix follow a curve in UG NX4!

I have drawn a sketh of what I am trying to do which may explain it better.
The helix I have created looks like that on the left but I am wanting the ends to end up with the circular cross section flat to parallel surfaces as shown by the sketch on the right.

RE: How to make a helix follow a curve in UG NX4!

The easiest way that I can think of would be to create the helix, then draw lines near the ends of the helix and use the 'bridge curve' function to connect them. If you are going to make a solid tube out of the result you will need to make sure the radius of curvature in the bridge section isn't too small for your wire diameter.

See attached part; if you increase the tube diameter much it will fail unless you move the straight lines around and/or fiddle with the bridge curve parameters.
(the attached file is NX6)

RE: How to make a helix follow a curve in UG NX4!

Thanks for your help, I think I've got it sorted now.

RE: How to make a helix follow a curve in UG NX4!

I quote what John.R Backer wrote: (may be there is another way to quote, but I couln't find it, sorry!)

"You mean as in a compression spring with what is called a 'Closed' end (or perhaps even a 'Closed and Ground' end)?"

YESSSSSS, exactly what i would need.....I need to design the spring exactly as reality, because of overall dimension issues.
Springs with "close and ground" ends are very common, but designing ends with NX4 is driving me crazy....
Did anybody already solve this issue?

Thanks everybody in advance for any help...

Bye
Umberto

RE: How to make a helix follow a curve in UG NX4!

Unfortunately I can't open the file, I'm working on NX4...
Anyhow, cheers for any help!

Umberto Orsini
Tenneco-Marzocchi

RE: How to make a helix follow a curve in UG NX4!

I was trying to do a helix on a helical path by extruding a section along a helix with an orientation by angular law  (ft/t etc.).

So i ended up with entering like 150 turns on this path but the programm refused to carry it out, error message was  something like "wrong definition"

So i examined the problem by using linear rule for angle orientation end entered end value of 50000 degree which resulted again in the above mentionend error i went to to around 35000 degrees at wich it was able to create the extrusion.

So my question now is, why has this "Limitation" been set and how can modify it, can it be modified at all??

NX6

RE: How to make a helix follow a curve in UG NX4!

You will probably have to break it into chunks. Pick some convenient number below the maximum, then create another swept using the face edges of the previous one and unite them together. Repeat until you get the length you need.

RE: How to make a helix follow a curve in UG NX4!

Try using a smaller Position Tolerance value in the Swept Body dialog Settings section.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.
 

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources