Seems there isn't a way to associatively extract curves anymore. They left it out of the Extract Geometry command when they revamped the dialog for NX5. I'm guessing it's because you can select Face Edges with Selection Intent for various commands.
Neat. Essentially, we now have 2 Join Curve commands and nothing that will extract a curve associatively and leave it as-is without joining it into a spline.
You can also perform an Instance Geometry, choose the Translate type, select the desired edge(s), select some vector direction, set distance to 0 and copies to 1.
John R. Baker, P.E.
Product 'Evangelist'
NX Product Line
SIEMENS PLM Software Inc.
Cypress, CA
Seriously though, don't you feel that is a bit misleading in terms of keeping things simple and easy to use? Extractions shouldn't have to be made with an Instance command (or vice versa for that matter).
I'd rather see the old method put back on the Extract command or have an option for the Composite Curve command to not join the curves, but just extract them associatively.
Yes, the workaround you mentioned is fine, but do you really feel a brand new user and modeler will figure that out? I've been using UG for a long time and even that workflow escaped me at the time. Just think what might run through a rookie's mind.
It will be a while before we get to use NX-5 in anger and these sorts of changes that take away current functions really scare us.
Can we please turn the associativity off! I don't generally care for associativity of any extraction as a default option. If I want to have to think about whether I'm going to have to maintain an associative entity in my model then while I do appreciate the ability to do so I want to have a choice and would use it infrequently, with the option turned off by default.
I can't say how annoying it is using NX-3 and NX-4 when we extract or enlarge faces that we generally have to mess about making three of four extra steps to blow away the parameters. I don't even care if you do think that I want them. I'm telling you that most of the time I just don't and that's that.
A couple of things. To start with, a 'Composite Curve' is not necessaily a Spline. If you extract a single straight edge, while it will be designated as a Composite Curve feature, it will still behave exactly like a Line in all places where you are expected to reference a Line.
Also, a Composite Curve is not just another Join Curve. In the case of Join Curve, the result actually is a single approximated curve (i.e. Spline) while in the case of a Composite Curve, what we have done is sort of 'group' extracted copies of the original curves/edges into a single feature where each individual segment still 'behaves' as if it were the original curve/edge, that is there is NO approximation, just a sort of collective or 'Composite' Curve.
Now as for for the old Extract Curve, it's still there under Insert -> Curves from Bodies -> Extract...
The only change made for NX 5 was that we removed the Curve/Edge option from the Insert -> Associative Copy -> Extract... function.
John R. Baker, P.E.
Product 'Evangelist'
NX Product Line
SIEMENS PLM Software Inc.
Cypress, CA
So, assuming the edges are splines, if you extract these composite curves off a face and then remove the trim from the face what are you left with?
See what we often need to do with surfaces, (sheet bodies if you like) is to effectively extend the boundaries of a face, sometimes several faces and then trim back to the original edges on a couple of sides, while adding new trim edges of our own to the areas that we're changing.
Note that unless you've turned Dialog Memory off, if a function offers you an 'Associative' option, such as the new Composite Curve does, and you toggle it OFF, it will remain OFF, even for new sessions, until you toggle it back ON.
John R. Baker, P.E.
Product 'Evangelist'
NX Product Line
SIEMENS PLM Software Inc.
Cypress, CA
