Divide a curve using another curve (Sketching in NX) 3

[5H4D0W]

Hello.
I have tried to google this rather trivial request, but couldnt find anything. All related scenarios tend to relate to curves outside of sketches.

What I wish to do is cut the green line in two, exactly at the intersection with the reference line (Red Horizontal line). [I made this simplified scenario, but in reality I have a sketch with multiple lines and curves needing to be split at various intersections] Keep in mind this is in a sketch environment, and therefore I cannot use the Divide Curve function.
I know there is a Quick Extend and a Quick Trim, but where is the "Quick Divide"?

 

[PSI-CAD]

Hi,
Unfortunatly, Quick Divide doesn't exist in sketch even in NX12.
You can contact GTAC for an enhancement Request.


Regards
Didier Psaltopoulos

http://www.psi-cad.fr

 

[NutAce]

First Question.
The defining line, which is defining the cut position, Is this in or outside the sketch?
When Outside you need to "project" this into the sketch.

A quick divide is not provided indeed. I think you are stuck with drawing 2 separate lines.

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2

Building new PLM environment from Scratch using NX12 / TC11

 

[5H4D0W]

Thank you, DidierPSICAD and NutAce.

Yes, both lines are in the same sketch. NX12

As mentioned, I only made this picture as a simplification of my actual work, wich has a multitude of lines and curves overlapping in the same sketch.

I can not fathom why this feature doesnt exist.

 

[Xwheelguy]

Works somewhat fine for me in NX11, unless something has changed in NX12. Try adding it to the Sketch Task Environment via the Customize command.

You need to be aware that Divide Curve will delete existing dimensional constraints and some geometric constraints and this will need to be repaired more than likely. If you have Continuous Auto Dimension turned on, you will see about 5 dimensions appear and as you properly apply the needed geometric constraints, the extra auto dimensions will disappear.

Tim Flater
NX Designer
NX 11.0.1.11 MP8
GM GPDL 11-A.3.3
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M

 

[5H4D0W]

UPDATE:

I was able to achieve approximately what I asked about by using Divide Curve

However, as soon as I have selected the defining curve, I must press enter within ≈0,1 seconds, or it will deselect automaticaly. (I assume NX is trying to prevent use of in-sketch curves as definitions in order to hide other disadvantages). So I have to click+enter as quickly as possible. Feels like Im not supposed to be doing this...

Now, Xwheelguy, (and thanks for the assistance, by the way), but do you think this has something to do with me using NX12?

As mentioned by Xwheelguy, geometric constraints and dimensions are destroyed when using this feature. Having to repair this dimensional spaghetti makes me question if this is the most advantageous method of doing things, or if I should just drop down some points at existing intersections and forget about Divide Curve alltogether.

 

[Xwheelguy]

It's anyone's guess as to why it's behaving this way in NX12 without calling GTAC. The documentation in both NX11 & NX12 state the exact same thing - and it DOES state that Divide Curve is NOT applicable for Sketch curves. If I were to guess, I'd say they attempted to correct it to match the Help docs in NX12.

I could see complicated Sketches quickly becoming a complete mess if Divide Curve were to be allowed - just look at your image above - you have 6 dimensional constraints that match (32.7, 35.7, 100) and now you have to figure out which geometric constraints need to be applied to get rid of some of the duplicate dimensional constraints. Seems to me it would be a bit easier, with less to figure out, to just make colinear lines where needed. I wouldn't want my sketch left with 3 matching dimensional constraints like the above.

If you still feel differently, call GTAC and submit an ER but I would be sure to include text for the Divide Curve to correctly solve the Sketch.

Tim Flater
NX Designer
NX 11.0.1.11 MP8
GM GPDL 11-A.3.3
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M

 

[Xwheelguy]

5H4D0W,

You don't even need to do the points, depending upon your Sketch. See the attached - about as quick as you can do it, IMO. Note that all of my dimensions are manual and of the Perpendicular type.

Tim Flater
NX Designer
NX 11.0.1.11 MP8
GM GPDL 11-A.3.3
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M

 

[cowski]

What do you hope to accomplish by dividing curves in a sketch, what is your end goal?

If you want to use part of an existing sketch curve for a later operation (such as an extrude), perhaps the "stop at intersection" option will get what you want? Depending on your needs, there might be another way to get what you want.

www.nxjournaling.com

 

[5H4D0W]

Xwheelguy

Thank you!
Could also use Quick Trim in that first step.
The weird part is that Quick Trim sometimes leaves a point where the end of the former line was.

Cowski

In this case I do not intend to extrude, but to create a thin surface for latter use in a 2D mesh (FEM).
The indea of dividing a line with use of another could also be used in other scenarios, and I have asked myself several times how to accomplish this more efficiently.
Than you for the tip on selecting with regard to intersections. Very useful!

 

[Xwheelguy]

5H4D0W,

The point is probably due to a dimensional constraint - that's why I didn't use Quick Trim - been there, done that years ago already. Is also why I don't use Auto Dimensions - you don't know what kind of dimensions NX has used and you don't know to what they're attached (intersections will often cause the points to appear when geometry is modified).

Tim Flater
NX Designer
NX 11.0.1.11 MP8
GM GPDL 11-A.3.3
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M