Recreating Profiles from Splines

[JPM73]

Hi NX'ers,

I have handful of spline profiles & I wish to either convert them to sketches or recreate them using sketches.

What's the best method to use to get accurate profiles & hopefully, won't be to time consuming to constrain the sketches?

Thanks


Jason M.
Unigraphics NX Designer

 

[JohnRBaker]

To start with, what version of NX are you running?

When you say 'spline profiles' are we talking about a 'splined-shaft' or some arbitrary profile created using B-curves?

If the profile is what I suspect that it is (the 'splined-shaft' variety) and if it's made up of lines and arcs, all you have to do is create a new Sketch, add the existing curves to the Sketch and then run the Auto Constrain command and about 80% of your work is done. And with NX 7.5, once the curves are geometrically Constrained, you can now turn on 'Auto Dimensions' and the sketch will be fully dimensioned.

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.

 

[JPM73]

Hi John,

I'm using imported curves from other CAD applications and appears as some type of spline in NX (7.5).

I did try to select or add curves within the sketch mode, but my curves/splines were not selectable & if they were, only a handful were - mainly the straight lines.

Any suggestions to convert these splines to sketch curves would be appreciated.

Thanks

Jason M.
Unigraphics NX Designer

 

[JohnRBaker]

I just tested NX 7.5 and was able to add to an existing sketch a series of different types of curves including splines and various conics.

What you need to do is make sure that all of the curves are planar since non-planar curves cannot be added to a sketch. And even if they are planar, the sketch and curves will have to be on the same plane.

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.

 

[JPM73]

Hi John,

If take a Section-Cut on a planner or datum surface, shouldn't those curves be transferable to sketch curves?

If not, what is your recommendation to take a parasolid or dumb solid, get handful of cross-section profiles, then convert those splines to sketch curves or to make the model parametric (in NX 7.5)?

Thanks again.


Jason M.
Unigraphics NX Designer

 

[JohnRBaker]

If you're creating a section, are these associative curves (features)? If so, you need to remove the parameterization (i.e., make them 'dumb') before the curves can be added to a sketch. To remove the parameters, go to...

Edit -> Features -> Remove Parameters...

...and select the Section curve(s) and hit OK. Now you should be able to add them to your sketch.

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.

 

[JPM73]

Hi John,

I knew I was missing a step somewhere. It's been a while since I've last done this.

Thanks for the info.


Jason M.
Unigraphics NX Designer

 

[JPM73]

Hi John,

Wiith NX 7.5, is it possible to take a parasolid or or some type of parasolid & convert it into a 100% parametric model?

In my project, I have reverse engineering data that comes to me in .stl, igs, parasolid & Excel table formats. I'm seek ways to (quickly) take data & make 100% parametric models. Later, these known dimensions will be conveyed onto drawings.


Can I take a dumb model/solid & convert it? Later, I will want to modify these models using synchronous model features or any other NX features to make a 100% parametric model?

Thanks again

Jason M.
Unigraphics NX Designer

 

[JohnRBaker]

You can't really 'convert' a dumb model into something which you might consider as being 100% parametric. However, using Synchronous Modeling you can assign parametric constraints to those aspects of the model which you need to update later. This can include controlling the length or width of an object, the diameter of holes, the radius of blends, to size of chamfers, etc.

I would suggest that you review the section of the NX 7.5 Help documentation titled 'Synchronous Modleing'. There are sections covering all of the various tools and operations, many of which includes short video clips showing how the function works.

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.

 

[JPM73]

Hi John & Others,

I created a section cut (feature), which gave me a nice profile. I then did the:

Edit -> Features -> Remove Parameters... & this removed parameters as it's suppose to do.

I added the curves to a sketch & it appears they all converted nicely. However, when trying to add geometric or dimensional constraints, I cannot. It appears that these curves are stilly splines, even though they have DOFEE's on them.


Any suggestions to get these selectable or to convert these splines into usable sketch curves?

Thanks again....


Jason M.
Unigraphics NX Designer

 

[JPM73]

Hi John & Others,

I am able to convert Section Curves (from the Section Curve feature) easily, then remove the parametrics to make them "dumb".

For the most part, these "dumb" curves are being added to my sketch & for those that aren't, I can easily recreate those. However, it appears that these"dumb" curves are still considered splines, instead of true sketch curves, meaning, I am limited to the geometric & dimensional constraints I can put on them. The problem is that not everything is selectable, even though it's an added sketch curve.

Any suggestions to get everything selectable?

As stated above, my design intent is to take a dumb solid & make it 100% parametric as possible. Even though this can't be fully done, I think if I can get the main freeform types of features, I can create the rest.

Thanks for the assistance again.....


Jason M.
Unigraphics NX Designer

 

[cowski]

You can try the 'simplify curve' command, which will split the spline into a number of arc segments. Depending on the spline it may split into hundreds of arcs, making this option less preferred. If you can tolerate some deviation from the input you may be able to recreate the spline (or the output from simplify curve) into a smaller number of arcs.

If your goal is to recreate freeform type features, you may want to keep the spline as is or recreate it with a 'studio spline'. Your curves do not have to be in a sketch for them to be parametric, your features will still follow changes to the input curves. Depending on the goal and the shape you are creating, a sketch may actually make things more difficult for you.

 

[JohnRBaker]

After removing the Parametrics of your 'section' go to...

Insert -> Curves from Curves -> Simplify...

...and select the curves after choosing the 'Hide' option. Now you will have a series of Lines and Arcs only, but don't surprised if you discover that there are a lot of these new segments. You can increase the Modeling tolerance if you would like (under Preferences -> Modeling...) but then results will not match as close to the original 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.

 

[JPM73]

Hi Everyone,

Thanks for the feedback again.... I'll have to try these suggestions when I get into work tomorrow


Jason M.
Unigraphics NX Designer

 

[JPM73]

Hi Guys,

Thanks for the info. It appears that converting splines to lines & arcs is doable, but it's more hassle than it's worth.




Jason M.
Unigraphics NX Designer

 

[Xwheelguy]

We used to "fit" splines into lines/arcs by putting non-associative points along 100% of the spline length. About 1 point every 2.5 mm or so...you decide the density of the points based on how close you need to match the original spline. Once the points are along the spline, create 3 point arcs and 2 point lines(non-associative) using the points along the spline. Feel free to skip over points and/or adjust the radius values as needed. Again, it will depend on how closely you need to match the original spline. Finally, use the Edit Curve command to re-blend the arcs and make them tangent to adjacent curves.

Check the resulting lines and arcs to make sure they are all planar. Correct any non-planar curves. Finally, you should be able to add them to your sketches as needed and delete the original splines.

I kept the original splines until the end so I could make sure I was able to use them to gage how close of a fit I was making with the lines and arcs.

Hope this helps.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[capnhook]

Hmmm...spline fitting.

Where's that old french curve I used to use....?

Proud Member of the Reality-Based Community..

 

[JPM73]

Hi Tim,

Where's the fit spline feature? At a glance, this approach seems better, rather than simplifying curves to have a bunch of segments.

I'll try this approach.


Jason M.
Unigraphics NX Designer

 

[cowski]

There is no 'fit spline' feature, he is describing a manual process that starts with a point set (there is a point set command).