Series of tool motions programmed after the last element of the contour had been machined is called tool retract or lead-out motion. In many ways, the methods and suggestions for the lead-out motions are similar to the lead-in methods. The major considerations are - as before - the cutter radius offset and sufficient clearances.

Retract from a Face

If the last element of the contour is a face (also called a shoulder, if it is in the middle of a contour), the retract is very simple, and there are no special considerations required. All that is needed is to continue the face cutting 'into the air' - into a X-axis clear position (clearance diameter).

The following program illustrates the method.

Note the retract diameter - although the part diameter is only 32 mm, another 2.5 mm per side has been added as a standard procedure.

Retract from a Diameter

When the last element of a contour is a diameter (specified by the X-axis only), program any tool retraction along the X-axis first, before moving away from the part. This X-motion should always be minimum of 2.5 mm (or 0.1 inches) per side (5 mm or 0.2" on diameter). As mentioned several times before, this clearance is necessary to accommodate the three standard tool nose radius sizes - 0.4, 0.8, and 1.2 mm (0.0156, 0.0313, and 0.0469 inches).

Retract from a Chamfer

A chamfer (or a taper) should always be extended, if it is the last element of the contour. This extension is necessary to guarantee completion of the contour. Typically, the part programmer selects the clearance above the diameter and calculates the final X-axis position, based on the clearance amount and the chamfer (or taper) angle. There are two common methods of programming a tool retract from a chamfer, both correct, if used properly. In both examples, the chamfer is extended above the final diameter by 0.75 mm (0.03 in inches).

Retract from a Radius

Retracting from a radius is similar to the lead-in motions, there are two common methods. If the last element of the contour is a radius, it should be followed by a lead-out radius and a linear or rapid motion, where the cutter radius offset will be canceled. This is the most common method and also one that will always work, providing the lead-out radius is greater than the tool nose radius. Programming this radius as 1.5 mm or even 2 mm will satisfy that condition.

Retracts to Avoid

Certain retract motions from the last chamfer or a radius are not recommended and, when used in the program, they can cause problems. The illustration shows some of the most common lead-out methods to avoid.

In a typical CNC lathe work, it is not unusual - in fact, it is quite common - to fully complete machining of the required part by clamping it more than once. CNC machine shops are used to a certain terminology when it comes to this type of machining. The main objective is to focus on the difference between reversing the part in the same setup and having two separate setups . For the purposes of this chapter, two terms will be used, with the following meaning:

• First chucking / Second chucking                  ... one setup - part is reversed in the middle of program
• First operation / Second operation    ... two setups - only a portion of the program is completed

These are by no means firmly established terms, but they are used in CNC machine shops quite frequently, even if the local meaning may be a bit unclear. Using these terms in this chapter with a specific definition should make it easier to distinguish between the two different types of machining.

About Jaws

On the basic level, there are two types of jaws for CNC lathes - hard jaws and soft jaws . As thematerial they are made of indicates, hard jaws are generally used for roughing and semifinishing toolpaths, whereby soft jaws are used for semifinishing and finishing toolpaths. Because of their hard material, hard jaws will 'bite' into the material and, in many cases, leave a physical mark on the part diameter, as they are mainly used with maximum chucking pressure. That is the main reason why hard jaws are not suitable for clamping of finished surfaces. Another reason is that hard jaws do no guarantee concentricity of the part as well as soft jaws do.

Soft jaws are made from mild steel, usually 1018 or 1020, with only a small percentage of carbon difference between them. The main benefit of soft jaws is that they can be bored to the exact diameter required with excellent concentricity of the clamped part. Since boring soft jaws has to be done between the stroke limits of the jaws travel, either an external or an internal ring should be used to provide the required clamping diameter.

Boring soft jaws is one of the most important skills a CNC lathe operator should have. Jaws can be bored manually, or with the help of a simple subprogram or a macro. An undercut between the jaws diameter and the locating face may be a necessary addition.

The illustration at right shows the correct bore of soft jaws (top), where the bored diameter matches the part diameter. The bottom figures show how the part will be clamped if the jaws bore is smaller than the part (left) or greater than the part (right). In both cases, the physical contact between the jaws and the part will be only at one or two points. Concentricity will also be hard to maintain.

Another very important information relating to soft jaws is the minimum depth of grip . Apart from time consuming study of the program, the CNC operator has no way of knowing how far along the Z-axis the tool is programmed. Many a toolpath is programmed very close to the front face of the jaws, and the programmer should provide all information relating to safe setup.

Single Setup - Two Chuckings

Two chuckings usually mean machining one end of the part, implementing a program stop M00 function in a suitable place within the program, reverse the part and continue with the machining using the same program. In this type of setup, each part will be completely finished when it leaves the CNC lathe.

There is no need for a complete example - the program structure should illustrate the concept quite clearly. Note the comment following the M00 function. Anytime the Program Stop (M00) is used in the program, the CNC operator should be aware of its purpose. The best place to convey this information is the comment section, programmed in the same block as the M00 function.

The example shown will show a program structure for three tools - after the first tool, there will be a part reversal, followed by two other tools:

N1 G21

N2 T0100

N3 G96 S.. M03

N4 G00 X.. Z.. T0101 M08

N5 …

N6 <... actual machining - tool 01 ...>

...

N16 G00 X.. Z.. T0100           (CLEAR POSITION FOR TOOL CHANGE AND PART REVERSAL)

N17 M00 (*** REVERSE PART FOR SECOND CHUCKING ***)

(================================================)

N18 T0200

N19 G96 S.. M03

N20 G00 X.. Z.. T0202 M08

N21 …

N22 <... actual machining - tool 02 ...>

...

N33 G00 X.. Z.. T0200           (CLEAR POSITION FOR TOOL CHANGE)

N34 M01                                (OPTIONAL STOP)

N35 T0300

N36 G96 S.. M03

N37 G00 X.. Z.. T0303 M08

N38 …

N39 <... actual machining - tool 03 ...>

...

N50 G00 X.. Z.. T0300           (CLEAR POSITION FOR TOOL CHANGE AND PART REMOVAL)

N51 M30                                (PROGRAM END)

%

Make sure to understand what exactly happens when the Program Stop function is activated:

• All axis motions will stop
• Spindle will stop
• Coolant will be turned off

These three activities are equally vital to successful program processing. Do not forget to reinstate them in the tool that follows the part reversal. Although the last feedrate, spindle speed itself, motion mode, and several other functions will still be active (in the computer memory), it is always advisable to program them anyway. Consider the likely possibility that the program will start after the reversal, for example, when the machining was interrupted or at the beginning of another shift. It is always the best approach not to count on various defaults and current settings - just in case.

Two Setups - Two Operations

Two operations usually mean machining one end of the part first, for all parts in the batch , then changing the setup and completing the same part machined at the other end. In this type of setup, each part will be completely finished only after the second operation is completed. Programming for two operations rather than two chuckings requires additional setup, but generally produces a part that is more accurate, particularly if concentricity is an issue. This method also requires two (or more) part programs that are stored separately, loaded separately, and processed separately. CNC operator should be aware of any job that is split over two or more programs.