Trim a sketch line at a datum plane

[lonesome-joe]

Hi, All!  I'm new to both Siemens NX and to the community.  Please bear with me as I refer to all features, procedures and objects by the wrong names, ask interminal dumb questions and generally cause eye-rolling to the point of headaches.  I've got a demo copy of NX11 (until the bean counters get off their ***** and write a check)... and my boss has entrusted my green self with the task of creating 4 fairly complex models and 2 REALLY complex models in a month.  Lucky me.  What I've learned so far is, NX is really hard.

I have a sketch in which I need to trim a line at a datum plane.  I can't find a way to project the plane to the sketch, and the trim command doesn't recognize the plane.  I can't dimension the endpoint to the plane, either.  Is is possible to project a plane in a sketch?  Thanx.

[TimF]

@lonesome-joe,

A few ways to do this:

1. Use Quick Extend.
2. Use a Geometric Constraint - Point On Curve, endpoint of the line on the plane.
3. Use a Perpendicular Dimension to the Datum Plane.

4. Double click the line, at the bottom of the dialog (make sure it's fully expanded) you should see the curve limits - start and end - change the appropriate limit to Until Selected and then select the Datum Plane.

All of the above work in NX11.0.1.

[lonesome-joe]

Tried all of 'em, the problem is, when editing the sketch, NX doesn't recognize the datum plane, i.e., I can't select it.

[cowski1 · Accepted solution]

The datum plane will need to come before the sketch in the feature tree. A feature that comes after the sketch doesn't exist when you are editing the sketch and therefore cannot affect the sketch.

[TimF]

@lonesome-joe,

In addition to the above, make sure your Selection Scope is not set to Within Active Sketch Only.  You should be able to select almost any geometry outside of a Sketch just like in the attached movie.  If you can't then you have something set such that it's preventing it from behaving the way you wish.

[mike_fdo]

Check the attachment. Edit the Sketch(1) (=Boundary curve) and observe Sketch(2) is trimming up to  its projection.

Is this what you are looking for?

[lonesome-joe]

All:
cowski1 wins the prize, indeed, I had made the datum plane after I made the sketch. I would's run into this same problem in Inventor of SolidWorks, too, I just lost focus. Thanx for your help!

[TimF]

@lonesome-joe,

If you set your Modeling Preferences under the Edit tab, Double-click Action (Sketches) to Edit With Rollback you won't see features that come after the Sketch when you're in Edit mode.  That might present to you a bit more of a clue when you run into timestamp related conundrums like this one.

I've always preferred the Edit with Rollback option when editing things because it can remove potential problem makers.

[lonesome-joe]

I don't have an "Edit" tab...

[DaveK · Accepted solution]

File, Preferences, Modeling, then the Edit tab.

I'd also change it here:

File, Utilities, Customer Defaults, Modeling, General, Edit