3D sketch

[dgberry]

In NX3 I was able to create a path to extrude a wire or cable to follow. I remember placing a wire component that had stubs on one side for the individual wires and the other was the jacketed cable size. I would then create a center line left of right, forward or back and up or down. I could create a line between two line segments and then I would place curves at the intersections of the lines to smooth things out. I could then use the center line to measure the cable length and then extrude the cable. My question is what is the command for doing the 3d sketch. I think there was a key stroke to change yz to xz to xy.

 

[JohnRBaker]

NX has never had a so-called '3D Sketcher'. By definition, the curves of a sketch most lay on the plane of the sketch itself. Granted, you can create regular curves, lines, arcs conics, splines in 3D space connecting them together to form a 3D network of curves. This has been possible since the very beginnings of UG/NX and is still supported today. And with the advent of the so-called Smart or 'Associative Basic Curves' they can even be created so that they will remain connected and can be edited, but they are still NOT a sketch.

BTW, what version of NX are you currently running? I suspect that you were using the old 'Basic Curve' functions which while they are still available in NX, have been removed from the normal out-of-the-box configuration since it now preferred that you use either 2D sketches or use the newer Associative Basic Curves to create wireframe objects.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
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To an Engineer, the glass is twice as big as it needs to be.

 

[dgberry]

I'm currently using nx8.5

 

[JohnRBaker]

OK, you can create these '3D curves' by using the either the explicit...

Insert -> Curve -> Line...

or

Insert -> Curve -> Arc/Circle...

...functions which will provide you a dialog and option for simple point-to-point line/arc/circle creation. Note that in the 'Settings' section of the dialog there's the 'Associative' option that you want to toggle ON so that these networks of curves hang together as intended.

Now if you wish to access to all of the various line/arc/circle options available which creating Associative Basic Curves, then I would suggest that you toggle ON the 'Lines and Arcs' toolbar which will give many different approaches to creating 3D lines and arcs/circles including one that might be of particular interest since you mention that you're looking for something which would line up with the three basic directions of X,Y and Z. When you open this 'Lines and Arcs' toolbar, the 3rd icon (note that the 1st icon is a toggle which indicates whether curves are to be created 'Associative' or not) is labeled 'Line-Point XYZ' which will drawing lines oriented to be parallel to one of the three axis in space from a point, which could be the end of a previous line. Using just this one function to would easy to create a '3D network' of lines connecting two points in space by defining what could very well be considered a 'path' for a cable to tube run (see attached example). All that you would need to do is to add the necessary 'corner' fillets, which are also on this toolbar (14th icon if you have not edited the contents of the 'Lines and Arcs' toolbar).

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.

 

[dgberry]

When putting in fillets, the corners will not trim.

Sorry to be a pain

 

[vja]

hello john

can you upload the model in nx 7.5 version if possible
thanks

 

[JohnRBaker]

But that's not important since the you can automaticaly go around the corners by using the Curve Selection rule 'Tangent Curves' with the 'Follow Fillet' toggled ON as shown below...

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]

They don't necessarily have to. You can use the follow fillet option (as John has done in his example).

If you really want them trimmed, you can use the "basic curves" fillet command (with trim options set) or use the "trim curve" command as necessary.

www.nxjournaling.com

 

[dgberry]

Okay, I see. It has been awhile and I'm very rusty with NX.

 

[JohnRBaker]

Attached is basically the same model except that it was created in NX 7.5.

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.

 

[vja]

thank you john