Introduction to 2½ Axis Machining in MecSoft CAM


Blog Categories

This tutorial assumes that you are familiar with how to load the MILL module from your MecSoft CAM plugin and that you have previously completed the MILL Quick Start Guide. You can find this guide by selecting Learn from the MecSoft CAM Main Menu (in VisualCAD/CAM, RhinoCAM, VisualCAM for SOLIDWORKS or AlibreCAM).  You should also first refer to the blog tutorial: How to Define a Setup for 2½ / 3 Axis Milling in MecSoft CAM to learn how to create your Machine, Post, Setup, Stock, Alignment, Material and Work Zero. These steps are typical for all 2½ & 3 Axis machining jobs. In this post we will discuss 2½ Axis machining and then show you how to create the toolpaths needed to machine the 2½ Axis part shown below.

What is 2½ Machining

2½ Axis machining is the 2nd most common application (behind 3 Axis machining) for MecSoft CAM users. The reason for this is because a large number of parts found in the real world lend themselves to 2½ Axis machining. That is to say, that the majority of 2½ Axis components are simple prismatic shapes composed of drilled holes, flat horizontal faces and straight or drafted vertical walls. In 2½ Axis machining the cutter moves in a plane both in the X and Y direction while maintaining a fixed Z height. The ½ axis is appended to 2 Axis, to denote the fact that cutting is done in successive fixed Z height planes starting at the highest Z level and stopping at a lowest Z level, thereby machining a complete 3D prismatic part. 

The Example Part

In this tutorial 2½ Axis toolpaths are used to program a simple prismatic part from 2024 Aluminum. The part measures 14.28″ long, 3.46″ wide and 0.748″ high and will be machined from 3/4″ plate stock measuring 15″ x 3.5″ x 0.75″ using the Fanuc0m controller. The part features include blind pockets, through hole pockets and a perimeter profile. The part is also engraved with a part number. The Machining Jog tree for the part is shown above. The machinable features are shown in the illustration below.

The Machining Job & Setup

The Machining Job tree for this project is shown below. The Machine definition is set to 3 Axis, The Post definition is set to Fanuc0m, and the Stock is set to Box Stock measuring 15”x3.5”x0.75”. The stock is aligned flush with the bottom of the part and Stock Material is set to ALUMINUM-6061. Setup1 is at its default location which is coincident with the WCS World Origin. A Work Zero is defined and is located the top south west corner of the stock. Fixtures are set to None. See: How to Define a Setup for 2½ / 3 Axis Milling in MecSoft CAM for the basic steps to complete the Machining Job tree and Setup1 as described here. The Machining Job tree and part now looks like this.

Create the 2½ Facing Operation

The first machining operation is the setup is a 2½ Axis Facing toolpath. This will ensure the top of the stock is flat with the top of the part. The top face of the part is at Z0.748 and is flat parallel to the XY plane. With this operation a 2.50″ diameter x 0.50″ face mill is used. Parameters include a Tolerance of 0.01 and Stock value of zero, a mixed cut direction, linear cut pattern, and 50% stepover. The Location of Cut Geometry is set to At Top with a cut depth of zero (one pass). Facing Entry/Exit is set to Lines & Arcs, a Tangent Approach Motion Length of 0.25 and zero radius and the same for the Departure Motion. Clearance is set to Automatic. You refer to the illustration below.

2½ Axis Facing Procedure

Here are the basic steps to create the 2½ Axis Facing toolpath strategy shown above. The dialog images show the parameters used. In most cases the default values are used. Pay close attention to the parameters on the Control Geometry, Roughing and Cut Level tabs.

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.

From the blog

The latest industry news, interviews, technologies, and resources.
Don LaCourse

Don LaCourse

Don LaCourse is an Application Engineer with MecSoft Corporation. Don brings over 20 years of experience in CAD/CAM operations in both automotive and mold design applications. Don also has extensive experience in documenting CAD/CAM products and is actively involved with writing the on-line help as well as creating training tutorials for MecSoft's products.

Try us out,

no strings attached!

Download Demo Form

Product of Interest(Required)
This field is for validation purposes and should be left unchanged.

Product of Interest(Required)
This field is for validation purposes and should be left unchanged.