UG NX 2.0 WHAT'S NEW

Ball Mill
What is it?
The Ball Mill option allows you to define a ball mill with or without a taper in a manner consistent with industry usage.
  
   
  
APT Method and Tool Method
  
The following explains the above image:
  
1. Diameter
  
2. Corner Radius.  
  
Why should I use it?
With this option, you enter the true ball diameter and taper angle, instead of calculating the theoretical diameter and corner radius.   
  
Where do I find it?
The best way is to go to create tool, and choose BALL_MILL . You can change existing mills to ball mills by changing the type in the tool dialog.   
  
  

Coordinate System Purpose
What is it?
This functionality allows you to designate the purpose of the coordinate system specified in the Orientation Group as either Main or Fixture Offset. Use this option when you have to specify multiple coordinate systems and identify one as Main so the post processor considers the relationship between the coordinate systems correctly.  
  
Why should I use it?
Use the main csys to establish the machine's primary coordinate system. Then you can use other MCS's with fixture offsets to establish local coordinate systems such as G54. The postprocessor can also use the relationship between the main and local coordinate systems to define the fixture offsets.   
  
Where do I find it?
This is a customizable item that may be added to any MCS_MILL object.
  
  

Operation Navigator Tool Enhancements
What is it?
You can now display the tool number in a column in the Program and Tool Views. And in the Tool View, you can display only the tools, without the hierarchy of pockets, faces, carriers, and turrets.
  
Why should I use it?
Use this option to see what tool number the system is going to output to the postprocessor or CLSF. You can also use this option to hide information that is not relevant for your machine tool or postprocessor.  
  
Where do I find it?
The system displays the Tool Number Column in the Operation Navigator by using MB3 --> Columns. The display of the Tool View is changed in the background of the Operation Navigator with MB3 --> Properties --> Condensed Tool View.   
  
   
  
  

Orient WCS to MCS
What is it?
This is a preference that you can set to orient the WCS to the MCS whenever you edit an Orientation group or an operation.  
  
Why should I use it?
Use this option to input coordinate system related data with respect to the MCS.  
  
Where do I find it?
In Manufacturing--> Preferences--> General--> Orient WCS to MCS.
  
  

Spindle Output
What is it?
The SPINDL UDE (post command) has been removed. The system now stores all of the spindle information as parameters in the operation. When you open a part with SPINDL post commands, the system moves the information in the command to the operation feed rates dialog, and removes the post command. CLS Output generates the SPINDL post command based on the new operation parameters.   
  
Why should I use it?
Use this to manually specify spindle parameters, or with the feeds and speeds table to automatically calculate them.
  
Where do I find it?
The system stores the spindle parameters in the feed rates item on the operation dialog.
  
  

Tool Holder
What is it?
This enhancement gives the system a better description of the shape of the tool holder by defining a series of cylinders which are stacked to represent the holder.
  
Why should I use it?
Use this option when you need a more accurate representation of the holder in the Manufacturing processors that use the holder for collision avoidance, such as Area Milling, Flowcut, Zlevel, and Holemaking.  
  
Where do I find it?
When creating a new tool, select the Holder tab. On an existing tool, the tool holder item can be added with customized dialogs.  
  
  

Tool Number Output
What is it?
You can now store the tool number in three places: the pocket, the tool, and the operation. The number inherits from the pocket, in to the tool, and on in to the operation. You can override it in the tool or the operation. The system always displays the output tool number in the operation.  
  
The legacy LOAD and TURRET UDEs (post commands) have been removed from the system, and all the information previously stored there is now stored in parameters in the operation instead. CLS Output generates the LOAD and TURRET post commands based on the new operation parameters. To be sure these are always output, the tool change marker has a preference called “Force LOAD and TURRET” to control this. When you open a legacy part with LOAD or TURRET post commands, the system replaces the LOAD and TURRET commands with a tool change marker. The system moves the information in the commands to the new parameters. The system sets the tool change marker to Force LOAD and TURRET, to assure the same CLS output as previous releases.   
  
Why should I use it?
Use this option to set the tool number to be output, based on your shop practices. For example, if the pockets on the machine are numbered, create pockets with numbers in the Machine Tool View, and load your tools there. If your tool numbers represent the actual tools, and not the position on the machine, assign tool numbers to the tools. If want to override a tool number, change it in the operation.  
  
Where do I find it?
You can create pockets by using create tool. The Pocket ID is on the pocket dialog. You can enter tool numbers by editing a tool or by selecting Operation dialog--> Machine.  
  
For a tool, enter the tool number as always. Some of the parameters previously in the LOAD and TURRET commands have been added.  
  
In an operation, many of the parameters previously in the LOAD and TURRET commands, particularly the tool number, are now on the Machine Control dialog.  
  
   
  
  

Output Tracking Point
What is it?
The Tracking Point feature allows you to define additional tracking points for a cutter in addition to the usual tool end position.
  
Why should I use it?
This option allows you to program a tool path once and then replace the programmed tool with a tool of a different size. Machine controller adjusts the tool path appropriately, saving you programming time.   
  
Where do I find it?
To define the additional tracking points: Define Milling Tool -> Tracking Points. To select a tracking point within an operation: Create/Edit operation -> Machine --> Tracking Points.
  
  

Alternate Processes
What is it?
This option allows you to define several alternate processes for a single feature template. Use this option when you need to minimize the number of feature templates. Several possible processes can be defined for this template.
  
Why should I use it?
Instead of having to create multiple templates for different processes, now you can create one template and define all your processes on that one template.
  
Where do I find it?
Manufacturing -> MB3 on a Feature Group -> Object -> Alternate Groups.
  
   
Classification Range
What is it?
Classification Range allows you to group features by the attribute ranges, as well as by any other rules of grouping that can be applied to the feature groups by creating rules in Knowledge Fusion.  
  
Why should I use it?
You should use this feature when you need to group the features in more ways than by the same attribute values.
  
Where do I find it?
In the file ug_cam_func.dfa modify the function ug_fbm_classifyFeatures() as required.
  
   
  
  Feature Recognition
What is it?
The feature recognition machining process finds the hole shapes by analyzing the part geometry. It recognizes three types of holes: simple hole, counterbore, and countersink.  
  
Why should I use it?
You should use this option to recognize hole shapes in your part and fully utilize the benefits of the Holemaking process.
  
Where do I find it?
Manufacturing -> Tools Menu -> Feature Recognition
  
   
Feature Recognition
What is it?
The feature recognition machining process finds the hole shapes by analyzing the part geometry. It recognizes three types of holes: simple hole, counterbore, and countersink.  
  
Why should I use it?
You should use this option to recognize hole shapes in your part and fully utilize the benefits of the Holemaking process.
  
Where do I find it?
Manufacturing -> Tools Menu -> Feature Recognition
  
   
Feature Status
What is it?
When you use Feature Status the system displays the machined status of features. It is possible that a tool can't machine a feature because the tool may collide with the clamp if it tries to machine the feature. The system now identifies and records such operations so that you can take appropriate action. This option checks all operations within a feature group whether or not the tool path has been fully generated. The system indicates the status by using the following icons: Complete  , Incomplete  , or Regenerate  .
  
   
  
Why should I use it?
You should use this option to make sure that all the operations are fully generated. If any operations is not fully generated because the holes could not be accessed, then the tool may break during the next operation.
  
Where do I find it?
Manufacturing -> MB3 Object -> Feature Status.
  
  Holder Types
What is it?
Holder Types allows you to select a floating or rigid holder for a Tap tool.  
  
Why should I use it?
You should set the holder type of a Tap tool to floating for a floating holder, where the tap can slide in and out of the holder. You should use rigid when the you put the tap in a solid holder and set up the machine for rigid tapping.   
  
Where do I find it?
Manufacturing -> Create Tool -> Hole Making Type -> Tap Tool
  
   
3D In Process Workpiece (IPW)
What is it?
Holemaking allows you to use the previous 3D In Process Workpiece (3D IPW) as the Blank Geometry and create the resultant 3D IPW. Holemaking also allows you to display the previous 3D IPW and the resultant 3D IPW in the operation dialog. In the workpiece and  geometry groups, there are two new options for blank geometry - auto block and offset. Use these to create an automatic, associative blank for use by visualize and Holemaking.
  
Why should I use it?
You should use 3D IPW in a Holemaking operation when you need to cut the regions based on the real workpiece and avoid regions with no material to be machined.
  
Where do I find it?
Manufacturing -> Edit a Holemaking Operation -> Use 3D IPW
  
   
  
   
  
   
  
  

Maximum Cut Depth and Extended Length
What is it?
The Maximum Cut Depth and Extended Length options have two checkboxes: Check Flute Length and Check Tool Length. If you select the Check Flute Length checkbox, the tool query returns the tools from the tool library that satisfy the query and the maximum cut depth condition.  
  
If you select the Check Tool Length checkbox, the tool query returns the tools from the tool library that satisfy the query and the extended length condition.
  
If you only select the Check Tool Length checkbox, the returned tools may go into the holes beyond the flutes.  
  
The following explains the image above:
  
1. Maximum Cut Depth
  
2. Extended Length
  
3. Short Flute Length
  
4. Short Tool Length
  
Why should I use it?
This option allows you to make sure the tools you retrieve from the tool library have long enough flute length and tool length to cut all the holes in the part without gouging the part or breaking the tool.
  
Where do I find it?
Manufacturing -> Holemaking Operation -> Groups