# Point to Point Operations

The information in this section will help you create and edit Point to Point operations in your manufacturing program.

Select Point to Point then set the strategy parameters for defining:

• a sequence of elementary Goto Point, Goto Position and Go Delta tool motions

Specify the tool to be used, NC macros , and feeds and speeds as needed.

## Point to Point Strategy Parameters

### Point to Point Tool Motions

 Goto Point A tool motion defined by the point the tool tip has to reach. Geometry can be selected as follows: Direct selection on the part (points, vertices, and so on) Direct  indication in a pre-selected surface.  Only selection done within the topological limits of the surface are taken into account. Indication of points to be projected onto a user-defined indication plane. This indication plane is considered as infinite (it has no topological limits). This allows point indication outside the part boundaries.  It is a temporary element used as an aid for selection. It is not saved after operation edition. Goto Position A tool motion defined by positioning the tool in contact with a part element, a drive element and possibly a check element, while taking To / On / Past conditions into account. Go Delta A tool motion defined by a displacement relative to a previous Point, Position or GoDelta motion location. Types of Go Delta motion are as follows. Components: relative motion defined by DX, DY, DZ displacements from previous motion location. Along Y axis: relative motion along Y axis (current axis system) on a user specified Distance, from previous motion location. Along X axis: relative motion along X axis (current axis system) on a user specified Distance, from previous motion location. Parallel to Line: relative motion on a user specified Distance, parallel to a user selected Line, from previous motion location. Normal to Line: relative motion on a user specified Distance, normal to a user selected Line, from previous motion location. The tool motion is done in a plane perpendicular to the tool axis. Angle to Line: relative motion on a user specified Distance, along a line computed from user defined Angle and Line. The tool motion is done in a plane perpendicular to the tool axis.

### Point to Point Machining Parameters

 Machining tolerance Specifies the maximum allowed distance between the theoretical and computed tool path. Offset along tool axis Defines an offset along the tool axis for all positions of the tool path (it is taken into account for all the positions of the operation). First compensation Specifies the tool corrector identifier to be used in the operation. The corrector type (P1, P2, P3, for example), corrector identifier and corrector number are defined on the tool. When the NC data source is generated, the corrector number can be generated using specific parameters.

## Point to Point Tool

All Milling and Drilling tools can be used in this type of operation.

## Point to Point Feeds and Speeds

In the Feeds and Speeds tab page, you can specify feedrates for approach, retract and machining as well as a machining spindle speed.

Feedrates and spindle speed can be defined in linear or angular units.

A Spindle output checkbox is available for managing output of the SPINDL instruction in the generated NC data  file. If the checkbox is selected, the instruction is generated. Otherwise, it is not generated.

Feeds and speeds of the operation can be updated automatically according to tooling data and the Rough or Finish quality of the operation. This is described in Update of Feeds and Speeds on Machining Operation.

In Point to Point operations, a local feedrate can be defined for all tool motions (except the first motion, which must be either RAPID or a specific feedrate). The local feedrate is applied instead of the machining feedrate during the tool motion to reach the tool position. For the operation start point, machining feedrate is taken into account.

## Point to Point NC Macros

You can define transition paths in your machining operations by means of NC Macros. These transition paths are built from elementary motions and are useful for providing approach and retract motion in the tool path.

• An Approach macro is used to approach the operation start point.
• A Retract macro is used to retract from the operation end point.

You can use the following commands to define the elementary motions of macros in a Point to Point operation:

 | | | | | | | | | | | -> distance along a given direction | | -> axial motion to a plane | -> PP word -> axial motion

The general procedure is described in Define Macros on a Milling Operation.