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Creating a 3D sketch

Creator
Creator

I am trying to create a 3D curve which is composed of a few segments of lines with radii between them (the lines are not lying in one plane). I connected the lines by creating the intersection points. But I couldn't find any fillet option for 3D lines?

I tried creating arcs between the lines. Although this was easy, but then I was stucked by trimming them, which was not easy at all.

Then I realised that there was a fillet line option which was under the sketch lines. But I couldn't find any 3D sketch option in NX. That feature (i.e. 3D sketch)  is easy in Inventor (you can create 2D or 3D sketches).

My question is:

What is the simplest way to create fillets for 3D connected lines (say 3 perpendicular lines not in one plane)?

6 REPLIES

Re: Creating a 3D sketch

Honored Contributor
Honored Contributor

If the lines intersect, I'd use the old curve fillet command (found on the basic curves toolbar). Alternately, you can create an associative tangent arc between the lines and when you create the feature, use the "tangent curves" curve rule or the "follow fillet" selection option (no need to trim the lines).

 

If the lines do not intersect, use "circular blend curve" or "bridge curve".

Re: Creating a 3D sketch

Creator
Creator
The fillet command exists only under the "sketch curve" command. In my case I don't have a sketch. I created "stand alone" curves (connected) - beacuse I didn't find any 3D sketching options. When I use tangent curves, the original curves remains together with the arcs, not trimmed.

Re: Creating a 3D sketch

Phenom
Phenom

Curves don't necessarily have to be trimmed, if you use the "stop at intersection" option, when creating your extrude, tube, revolve, etc.

 

I've done it with an assortment of sketches that were only the arc, before the "Circular Blend Curve" option.  More than one roll cage was done like that.

-Dave
NX 11 | Teamcenter 11 | Windows 8.1

Re: Creating a 3D sketch

Honored Contributor
Honored Contributor

"The fillet command exists only under the "sketch curve" command."

 

The fillet command that I mentioned can be found on the basic curves toolbar (menu -> insert -> curve -> basic curves...). The dialog is "old-school" so it may take some experimentation to see how it works. I like the 2 curve fillet option; pick each curve that you want to fillet/trim then pick the side that the arc center lies on. Note that the result will be unassociative.

Re: Creating a 3D sketch

Genius
Genius
Not sketching any of the curves used in this set of curves will be the simplest way, IMO. Then you will have access to all the tools that are being suggested above.

Before you delete your sketches, exit Sketcher, go out into Modeling and bring up the Basic Curves dialog and draw lines (NOT associative lines) on top of the 3 straight sections then hide or delete the sketches and give the above suggestions a try.

It also might help if we were to know what you're going to be doing with this 3D curve once you get it created - in case you need to deal with bend radii, etc....some "fillet" type curves will result in splines and won't be true bends so to speak.
-Tim

Re: Creating a 3D sketch

Siemens Genius Siemens Genius
Siemens Genius

Try the 'Circular Blend Curve' command to create your fillets.

(view in My Videos)

 

Abe