What is 2½ Machining
The Example Part
The Machining Job & Setup
Create the 2½ Facing Operation
2½ Axis Facing Procedure
1. New operations are generated BELOW the selected operation in the Machining Job tree so first make sure the Work Zero is selected.
2. From the Program tab select the 2 Axis menu and then pick Facing.
3. The 2½ Axis Facing operation dialog will display with the Control Geometry tab selected by default. In Facing if you do not select Part Regions, the entire part is calculated for the XY extents of the facing operation. Check the box to Include stock model silhouette and then select the Tool tab.
4. From the Tool tab select the Edit/Create/Select Tool … button to display the Create/Select Tool dialog.
5. Use the parameters shown in the dialog below to define a Face mill cutting tool. Here are the basic steps:
A: Select Face Mill from the top toolbar.
B: Enter “FACEMILL-2.5 INCH” for the Name.
C: Enter the Tool dimensions shown in the dialog below paying attention to the tool preview window.
D: Complete the Properties sections as shown.
E: Select the Feeds & Speeds tab and enter the desired values.
F: Then select Save as New Tool and you will see that the tool is added to the Tools in Session list on the left side of the dialog.
6. Now pick OK from the Create/Select Tool dialog and you will see that your tool is added to the Tools list of the Tools tab in the 2 Axis Facing dialog.
7. Since it is the only tool, it will be selected by default for this operation. Now select the Feeds & Speeds tab of the dialog.
8. The feeds & Speeds allows you to set you feeds and speeds for this operation only. To load the feeds & Speeds that you set for the tool, pick the Load from Tool button. To calculate new Feeds & Speeds values you can pick the Load from File button and use the built in Feeds & Speeds Calculator.
9. Now select the Clearance Plane tab of the Facing operation dialog. We will use the default values for clearance. The Clearance Plane Definition is set to Automatic and the Cut Transfer Method is set to Clearance Plane. At any time you can select the Help button from the dialog to display the online help for this dialog.
10. Now select the Roughing tab from the dialog. Here you can set global parameters, the cut pattern, cut direction and stepover parameters.
11. We are using a Linear Cut pattern, Mixed cut direction, a Stepover distance of 50% of the tool diameter and we are starting at the bottom of the cut (i.e., negative Y direction).
12. Now select the Cut Levels tab of the dialog. Here we have the Location of Cut Geometry set to At Top and the Total Cut Depth, Rough Depth, Finish Depth, Rough Depth/Cut and Finish Depth/Cut all set to zero. This means that there will be only one cut level located at the top of the part.
13. Now select the Facing Entry/Exit tab of the dialog. Here you can determine how the cutter will approach and engage the cut pattern as well as how it will depart and retract. We have the Entry Motions set to Lines & Arcs, Approach Motion set to Tangent and Length (L) set to 0.5. The Engage Motion is set to Radial and Radius (R) set to zero. These parameters will extend the entry motion tangent to the cut start point of the cut pattern by 0.5”.
14. We also have the Exit Motions set to Lines & Arcs, Departure Motion set to Tangent and Length (L) set to 0.5. The Retract Motion is set to Radial and Radius (R) set to zero. These parameters will extend the exit motion tangent to the last cut point in the cut pattern by 0.5”.
15. For the Advanced Cut Parameters tab we use the default values.
16. Now pick Generate and the 2½ Axis Facing toolpath is calculated and displayed on the part. It is also listed in the Machining Job under the Work Zero.