05-08-2018 09:01 AM
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.
Solved! Go to Solution.
05-08-2018 09:19 AM
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.
05-08-2018 09:52 AM
05-08-2018 10:07 AM
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.
05-08-2018 10:08 AM - edited 05-08-2018 10:09 AM
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.
05-08-2018 10:16 AM
05-08-2018 10:29 AM
05-08-2018 12:30 PM - edited 05-08-2018 12:32 PM
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.
05-08-2018 03:35 PM
05-08-2018 03:45 PM
File, Preferences, Modeling, then the Edit tab.
I'd also change it here:
File, Utilities, Customer Defaults, Modeling, General, Edit