Wireframe Fillet in NX7.5

[Kenevil]

This should be an easy one but for the life of me, I can't figure it out. How to I crate a wireframe fillet (without basic curves)? I've been using Arc Tan-Tan-Radius, then going back to trim the lines. There's got to be a one step operation for this... right?

 

[kapmnit123]

Hi,
Will Insert/curve from curves/Circular blend will do for you?
Best Regards
Kapil Sharma

 

[JohnRBaker]

Why are you not using the Sketch tools?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
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[Kenevil]

Thanks but Insert/Curve didn't trim the lines.

I love using sketch but I'm the only one I know using it. When other users modify my sections, they remove the sketch and replace it with dead data. I'm thinking if I can't get them to use sketch, maybe I can at least get them to use parametric wireframe.

 

[JohnRBaker]

And I can think of several 'popular' systems where 'sketching' is virtually the ONLY option.

I beg you, please do not allow your co-workers to start stringing together individual associative curves segments to form profiles that they then Extruded or Revolved into solid bodies. That is blatant 'software abuse'.

And while we're on this subject, haven't you been complaining in another thread that NX has too many ways to do the same thing? If you really believe that, why would you even consider telling your co-workers to misuse Associative Curves to create Extrude/Revolve profiles when that is EXACTLY what the Sketcher was designed to do? That would seem to violate your own personal views that you've been expounding on in that other thread.

But getting back to your original issue, even if the curves which were referenced when creating a so-called 'fillet' (outside the sketcher) were NOT trimmed, we've provided selection schemes which will treat that set of untrimmed curves as IF they were trimmed, that is by following tangencies or even to move from intersection to intersection. Sometimes there is a need to NOT trim any of the curves and so we must provide multiple tools and options so that ALL of our users are able to use the software in a manner with suits THEIR particular needs or situation.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Kenevil]

LOL, John, you almost got me except but we are not extruding these curves. We are creating criteria sections for the studio. The section is the deliverable so I don't think there is any abuse going on.

 

[JohnRBaker]

All of the various surface functions accept Sketches as "sections" as well as providing the Selection Rules for 'Stop at Intersection' and 'Follow Fillet' if you're using any of those 'untrimmed' sets of curves.

Don't you just love using a system which offers flexibility when it comes too doing different tasks?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Kenevil]

I think you're trying to say NX can't do what I'm asking it to do which was... Apply an associative 2D fillet at the intersection of two curves or lines that also trims the lines (like fillet in basic curves). We are not using these curves for surface dev or extrusions. They are more like drawings.

 

[Xwheelguy]

Sounds like you're both partially correct.

NX's curve functions were never intended to support the type of work you're doing Kenevil; however, it's also true that there is not a specific command outside of Sketcher which will associatively trim lines and apply the fillet. Hard to tell how your productivity is impacted with non-associative 2D geometry that's not being used for solid modeling. 10 to 20 years ago, people would just manually edit the 2D and not worry so much about giving it associativity since offset, length edits, edit fillet were all present in most softwares in some form.

My suggestion is to sit down with the other designers and explain the situation - if the 2D associativity is an absolute must, then THEY MUST get used to Sketcher. Try having them create the 2D outside of Sketcher without the fillets then adding the curves to a sketch and apply the fillets there. You may find that having more than one way to skin a cat in NX turns into being a salvation rather than a headache.

Tim Flater
NX Designer
NX 7.5.4.4 MP8
WinXP Pro x64 SP2
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[JohnRBaker]

I've given you a perfectly workable solution. It's just a matter of you taking advantage of it.

BTW, the Sketcher is fully supported while working in the context of a Drawing. In fact, and you should appreciate this, with the last couple of releases of NX, if while working in a Drawing you wish to add some explicit curves, to either the Drawing sheet itself or to one of the Views, the ONLY curve creation tool available to you will be the Sketcher. See, we do try and make the system easier to use by removing redundant and/or duplicate functions thus offering the user a single familiar approach (perhaps there's hope for us yet).

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[cowski]

Assuming your geometry is planar, there is an option for you...

Draw your outline with unassociative geometry, use sharp corners (don't add fillets). Extrude the outline some convenient distance and add blends of the desired sizes on the desired edges. Create a datum plane and create an associative intersect curve feature between the solid and the datum plane. You can now edit the unassociative geometry and/or the blend sizes and the resulting curves will update.

Shades of Rube Goldberg, but it will work...

www.nxjournaling.com

 

[kapmnit123]

Hi Kenevil,
Sorry for a late reply.Although i only second John's suggestions (usage of sketches) but if you desire to go by your current methodology ...then here is something that might be of some interest to you...Please find a video attached (it may seem to be one step more than what you expected but may give you the desired result).
Best Regards
Kapil Sharma

 

[Kenevil]

Thanks Kapil. That's similar to what I was doing but with trim curve instead of composite curve. I'm not familiar with composite curve but will play with it today.

Thanks Cowski, I had the same idea but thought other designers using my sections wouldn't be able to figure it out. (My design team is on the other side of the world)

Thanks John, yes you gave me great alternatives and I appreciate your depth of knowledge. In this case, I just needed a "yes" or "no" if I was missing an operator. I questioned myself every time I created a blend and no I wont.

Thanks Tim, you are right. Productivity isn't really affected if I don't use parametric curves. The goal was to use expressions to control the section. I was using expressions to control my offsets (material thickness) and I was trying to expand that to our min rads.

 

[kapmnit123]

Hi Kenevil,
I feel composite curve will suit better as you just need to do the selection once (trim curve will be certainly time consuming if the number of curves is large).Moreover i guess it will be more stable too.But i will leave that decision to you .Let us know if you find it suitable.
Best Regards
Kapil Sharma

 

[cowski]

I think we've established that a sketch is really the right tool for what you want to do, but if you are forced to use unassociative geometry, you can create the fillet with the basic curves tools and edit the fillet with the appropriately named "edit fillet" command. The edit fillet command will recreate the fillet and trim the corner geometry as necessary.

Video attached in 7zip format.

http://files.engineering.com/downlo...bf-fb41-4222-ac1e-e1df9ff8da6f&file=fillet.7z

www.nxjournaling.com