Create a Point to Point Operation

task target This task shows how to insert a Point to Point operation in the program. 

To create the operation you must define:

  • the tool that will be used
pre-requisites Open the PrismaticMilling02.CATPart document, then select Machining > Prismatic Machining from the Start menu. Make the Manufacturing Program current in the specification tree.  
scenario 1. Select Point to Point .

A Point to Point entity along with a default tool is added to the program.

The Point to Point dialog box appears directly at the Strategy tab page . 
This Motions tab allows you to define the elementary Goto Point, Goto Position and Go Delta motions making up the machining operation. 
2. Click Goto Point , then select a corner point on the underside of the part. 

Just double-click to end point selection. The first tool motion is defined and appears in the list in the Point to Point dialog box.
3. Click Goto Position . A Sequential Motion dialog box appears to help you specify the part, drive and check elements as well as positioning conditions (To / On / Past). 
4. Just click OK when you have specified the desired elements and conditions. The second tool motion is defined and appears in the list in the  Point to Point dialog box.
5. Add other Goto Point, Goto Position and Go Delta motions as shown in the figure below.

In the Point to Point dialog box you can:

  • add PP words to the list by clicking on the PP words icon and specifying the desired syntax.

  • move motions up or down the list by the Arrow icons or remove motions by means of the Remove icon.

  • edit the properties of a motion by clicking the Properties icon.
6. Select the Strategy tab to specify machining parameters. If needed:
  • Click the plane symbol in the sensitive icon to specify an indication plane. Just select a plane or planar face or enter X, Y, Z coordinates in the Indication Plane dialog box that appears.
  • Double click the text in the sensitive icon to specify an offset along the tool axis.
  • Define the tool axis direction by first selecting the axis representation in the sensitive icon then specifying the direction in the Tool Axis dialog box that appears.
7. Select the Tool tab page to replace the default tool by a more suitable one.

Select the Face Mill icon. A 50mm diameter face mill is proposed. You can adjust the parameters as required.

See Edit the Tool of an Operation for more information about selecting tools.
Check the validity of the operation by replaying the tool path.

8. Select the Feeds and Speeds tab page to specify the feedrates and spindle speeds for the operation.
9. If you want to specify approach and retract motion for the operation, select the Macros tab page to specify the desired transition paths. 

The general procedure for this is described in Define Macros of an Operation.
10. Click OK to create the operation.
You can right click the motions displayed in the 3D view to access contextual commands to insert or remove point positions and to assign local feedrates.

By selecting a circle, its center is taken as the point to machine.

Points of an associated sketch can also be selected.

Points can be defined by clicking on a user-defined indication plane.

Points can be defined by entering  X, Y, Z coordinates in the motion editor.
Point coordinates are defined in the machining axis system.

end of task