UG NX 2.0 WHAT'S NEW

Highest Reference Point tapers – Used to taper faces, using the highest reference point on the face.

To create a body taper follow these general steps:
  
From the Body Taper dialog choose either the Edge or Face creation method.
  
Specify the objects for the various selection steps.  
  
In the case of undercut tapers, you don’t need to specify a parting entity.  
  
To create tapers using highest reference point select the Highest Reference Point option.  
  
For double-sided tapers, based on the method of taper creation, specify two sets of edges (one on either side of the parting) or faces to be tapered. If you specify edges, they should satisfy the following constraints: they should not cross the parting; they should either be connected end to end or they should be such that the taper surfaces created from the edges can be trimmed by the body.
  
The same Body Taper dialog is used for both creation and edit. However, when you are making modifications, you can only change the angle of draw or the match option, or switch between double-sided taper and highest reference point taper. To modify the selected objects use the Redefine Feature in the Model Navigator.
  
Why should I use it?
Use body taper features to prepare the concept part for molding and casting. These types of tapers have significance from the manufacturing process perspective and as such are best used after the concept part has been prepared.
  
Where do I find it?
Creation: Modeling-> Insert-> Feature Operation-> Body Taper
  
Edit: Modeling-> Edit-> Feature-> Parameters
  
The edit dialog is also accessible through MB3 on the feature in the Model Navigator. This feature also supports redefine (rollback edit), accessed through MB3 on the feature in the Model navigator.

Selection Intent and Section Building
What is it?
Selection Intent has been added to most Modeling features that select multiple curves, edges and faces. In addition, a new Section Builder tool can be used in parallel with Selection Intent for features that require a profile. (Selection Intent was formerly known as Smart Collectors, and was first introduced in V18 for the Taper function.)  
  
You use these tools when creating and editing features. First set an appropriate collection method in the Selection Intent Toolbar during object selection of an enabled feature. Then select the base object or objects to define the collection.
  
Why should I use it?
These tools let you define your intent at a high level. Not only is selection more efficient, you also increase the robustness of updates during edits by relying on higher level entities that capture your intent instead of low level curves and topology.
  
Where do I find it?
Most Modeling features that previously selected multiple curves, edges and faces now use Selection Intent and/or Section Building.
  
For example:
  
Modeling-> Insert-> Form Feature-> Extrude
  
Modeling-> Insert-> Feature Operation-> Edge Blend
  
Modeling-> Insert-> Free Form Feature-> Styled Blend
  
  

Refit Face
What is it?
Refit Face is a new editing tool that lets you modify an aesthetically displeasing face to produce acceptable results while maintaining close tolerance with the original geometry. You can modify the data size of the resulting geometry by specifying new values of degree, patch count and tolerance.
  
To operate:
  
Select the face to refit.
  
Select the refit direction or accept the default.
  
Select the refit method or accept the default.
  
Specify new values for the degree, patch count or the tolerance or accept the default.
  
Check for any fitting errors. If acceptable, use Apply to refit the face.
  
Exit the dialog or continue to refit another face.
  
Why should I use it?
Refit can be very useful wherever you have a need to modify existing geometry for any of the following reasons.  
  
The existing geometry is aesthetically unacceptable.
  
The existing geometry has too much data generated as a result of previous operations.
  
The existing geometry is reverse engineered data to be used for detail work.
  
The existing geometry is data translated from another CAD system.
  
Where do I find it?
Free Form Shape toolbar
  
Edit Curve toolbar
  
Edit-> Free Form-> Refit Face
  
Edit-> Curve-> Parameters-> Edit Spline-> Fit

Sketcher Enhancements - Redefine Positioning Dimensions  
What is it?
You can now redefine sketch positioning dimensions.
  
Just select existing positioning dimensions and then follow the prompts given by the system to select new reference objects.
  
Why should I use it?
Use this new capability when you want to change the positioning of a sketch that was already positioned using outside references.
  
Where do I find it?
Modeling-> Sketcher-> Reattach.
  
   
  
  

Sketcher Enhancements - Working in a 3D Context
What is it?
Sketcher has a new procedure to let you project curves into a sketch. This replaces the old Add Extracted Curve to Sketch function.
  
The process is the same as that used by the Add Extracted Curve to Sketch function, except that you can now project a curve non-associatively into a sketch. You can also remove the associativity of a projected curve in the sketch.  
  
Why should I use it?
Use this function to project entities onto the sketch plane and to solve and define a sketch.
  
Where do I find it?
Modeling-> Sketcher->Insert-> Project
  
  

Sketcher Enhancements - Spline by Points and Poles
What is it?
Sketcher now has two new methods for creating splines:
  
Spline by Points.
  
Spline by Poles.
  
Simply select screen locations to indicate the defining point or pole locations. Before exiting the dialog you can make adjustments to the spline shape by dragging the point or pole handles.
  
Why should I use it?
Spline creation within Sketcher now provides immediate visual feedback, and is more interactive and easier to use than the traditional spline creation methods.
  
Where do I find it?
Modeling-> Sketcher-> Insert-> Spline by Points or Spline by Poles
  
  

Sketcher Enhancements - Rectangle
What is it?
Two new methods for creating rectangles in the Sketcher are now available.
  
Use these new creation methods to indicate an angle at which you would like to create a rectangle. After selecting one point to start the rectangle creation, indicate the angle by specifying where the second point is located.
  
Why should I use it?
This function lets you create rectangles that are not parallel to XC and YC. This relieves you of having to use the Profile or Line function to create such rectangles.
  
Where do I find it?
Modeling-> Sketcher-> Insert-> Rectangle
  
   
  
  

Sketcher Enhancements - Dimension
What is it?
The process of creating and editing dimensions in the Sketcher is now done without using dialogs. And, you can perform both of the operations at the same time.
  
To create dimensions choose the Sketch Dimension icon option and then select the geometry on which you want to create dimensions. To edit dimensions, select the dimension.  
  
Why should I use it?
These enhancements let you create dimensional constraints to fully define a sketch. You can easily edit the dimensions to modify a sketch.
  
Where do I find it?
Modeling-> Sketcher-> Insert-> Dimensions.   
  
Note that both Dimensions and Create Constraints have been moved from the Tools-> Create Constraints menu to the Insert menu. In addition, Create Constraints has been renamed Constraints.  
  
  

Sketcher Enhancements - Filleting of Splines, Conics, and Projected Curves
What is it?
All supported curves in the Sketcher that include Splines, Conics, as well as Projected (Extracted) Curves can now be filleted.
  
Why should I use it?
This enhancement lets you fillet all curves in the Sketch.
  
Where do I find it?
Found in the Sketch Task Environment under Insert-> Fillet.