Cutoff Cycle

This is one of the extended style turn cycles and specially designed for cut-off operations. It handles the complete process including the option to create a chamfer on the backside of the part before the final depth moves are generated. The cycle uses regular grooving tools with tool angle set to 90° as would be normally used for outside grooving operations. It also checks for the maximum cutting depth as specified in the tool settings. When selected, the cycle opens a small dialog that displays the cut-off specific settings only. Once finished there, you will normally use the "Work Step Data" button to continue to the regular machining dialogs to define all other parameters like the tool/turret number, speed and feedrates. To edit the cut-off specific settings later, simply double-click the corresponding Work Step in the Selection List Box. To edit settings on the regular "Work Step Data" dialog you can also use the Work Step Data command from the Machining menu or the corresponding button on the extended dialog.

$image\btn_mini.gif$ Graphic: Movement Sequence (Cutoff + Chamfer)

$image\btn_mini.gif$ How to change default liftoff Settings

$image\btn_mini.gif$ Important Post-Processor Information

For more information select the desired area in the graphic below:

X Rapid Diameter (Xr)

This setting specifies the X axis position were the tool will be positioned at rapid feed-rate at begin of the cutoff operation.

Z Cutoff Position (Zc)

The value specified here indicates the cutoff length as absolute position of the right edge of the tool tip in relation to the parts origin. Keep in mind that the tool settings (X/Z Prog. Point, Tip Radius, Width) as defined on the Tool Info dialog still need to refer to the left tool edge as it is standard for grooving tools with 90° Tool Angle.

X Clearance (Xc)

This parameter defines the clearance and retract plane above the part diameter, specified as an unsigned incremental value. When Diameter Input on the Setup dialog is selected, this setting is input as diameter, otherwise as radial value. From this point, all plunge moves are done using regular cutting feedrate.

Part Diameter (Xp)

This is the outside diameter of the part in the area where the cutoff operation will take place.

Cutoff Diameter (Xc)

This setting specifies the final cutoff diameter. When reaching the final depth, the cycle calls "User Cycle -17" from the post-processor to support optional parts catcher retract commands. It then lifts off in positive Z direction using the internal Z Lift Off amount before retracting to the initial X rapid diameter.

Note:

Specify a negative diameter to let the tool cut over the centerline if a flat front surface is required. For a tool with 0.005 inch tip radius you would specify a cutoff diameter of "-0.01" to achieve this result.

X Step (rad)

This parameter specifies the incremental unsigned depth move after which the tool is retracted by the X Lift Off distance for chip breaking.

Backside Chamfer

Activate this checkbox if you need to machine a chamfer on the backside of the part that is cut off.

Chamfer Size

This setting specifies the size of the 45° chamfer along the Z axis as an incremental unsigned value.

Work Step Data Button

This button opens the regular Work Step Data dialog that is used to input tool & offset numbers, cutting speed and feedrates. The Cutoff dialog itself is closed after it's current settings have been checked and stored.

Help Button

This button opens the EZCAM help system and pre-selects the current cutoff cycle as the main topic.

OK Button

When this button is selected, current user inputs are checked and the dialog is closed.

Cancel Button

This button closes the cycle dialog without accepting any inputs or alterations.

Cutoff Movement Sequence (With Chamfer):

The graphic and text below explains the moving sequence generated by the cutoff cycle with the chamfer option selected. You might notice the use of some internal lift-off values for the X and Z axis. These parameters can be accessed by adding/editing related entries in the EZCAM.INI file. Click here for more information.

Step1

Step2

Step3

Step1:
The grooving tool rapids to the position specified by the Xr and Zc settings. The Z position is hereby automatically shifted by the tool width and an additional shift in Z minus direction (Z Lift Off/2) to provide side clearance for the subsequent chamfering pass. Then follows a rapid move to clearance plane Xc above the part diameter Xp . Now the tool plunges down to a depth specified by the chamfer size and tooltip radius to ensure enough clearance for the subsequent chamfering pass. Finally the tool rapids back to X clearance.
Step2:
The tool is positioned for machining the chamfer first in Z, then in the X axis, followed by the 45° cutting pass for the chamfer.
Step3:
Move to final cut-off diameter as specified by Xd. If an X Step has been defined the tool will step down with subsequent retracts for chip breaking. When reaching the final depth, the tool lifts off in positive Z using the internal Z Lift Off amount before retracting to the initial X rapid diameter.

How to change default Liftoff Values

In various places, the cutoff cycle uses internal values as liftoff amounts for the X and Z axis. By default, both are set to 0.2mm or 0.005 inch. If necessary you can customize these values by adding the below listed lines to the EZCAM.INI file located in the windows directory. To edit this file you can use the Notepad editor that comes with the operating system. Use the "Search" function to locate the "[TURN-Automation-Metric]" or "[TURN-Automation-Inch]" sections. If they exist, add the two lines below each of these sections. Otherwise append all six lines as shown below at the end of the EZCAM.INI . Then customize the values or the X and Z axis and save the file.

[TURN-Automation-Metric]

cutoff_xliftoff=0.2

cutoff_zliftoff=0.2

[TURN-Automation-Inch]

cutoff_xliftoff=0.01

cutoff_zliftoff=0.01

Important: Always create backup copies before applying changes to INI files.

Important Post-Processor Information

When creating the NC code, the Cutoff cycle calls "User Cycle-17" section from the post-processor three times. First at begin of the cutoff operation when reaching X clearance plane, second - after machining the optional chamfer/fillet, and third - right after the tool reached the final cutoff diameter. This is done to support optional parts catcher in/out commands. As this cycle was not available in post-processor versions prior to V13, any existing post-processors may need to be updated. Contact EZCAM support and request an update proposal.

In "User Cycle-17" you can determine to call position by checking the string variable p25.

p25="1" 'this is first call

p25="3" 'this is second call - this option was introduced at a later stage so it got "3" assigned

p25="2" 'this is third call

Important: Always create backup copies before applying changes to post-processors.