In the 
CAM
Tree, right-click 
CAM Defaults, and click Cutting Conditions.
The Cutting Condition Parameters allow you to adjust various cutting parameters for drilling operations. This dialog box contains parameters for the Center Drill, Drill, Ream, Chamfer, Counterbore, Tap, and Bore operations. Some of the parameters have a finish allowance small and a finish allowance large. The reference for small and large tools is 3 mm. or 0.118 inches. Any tool greater than this value is considered a large tool, and any tool less than or equal to this value is considered a small tool.
There are two versions of this dialog box. One is used for the CAM Defaults, and the other is used to change the settings for the current job only as explained next.
To access the Cutting Condition Parameters, do one of the following:
In the CAM
Tree, right-click
CAM Defaults, and click Cutting Conditions.
These settings are the system defaults for all new files/jobs.
In the CAM
Tree, right-click the job folder (for example, Milling
Job), and click Cutting
Conditions.
These settings are applied to the current job only.
View the Cutting Conditions Parameters dialog box
Dwell Seconds - sets the dwell value to a specific measure of time (in seconds). Type the value to set how long the tool dwells for center drill operations.
Dwell Revolutions - sets the dwell value to the number of complete spindle revolutions the tool must complete during the dwell.
Peck Increment (%) - determines the peck depth that the drill plunges into the hole to start the next peck rather than retracting to the clearance plane. This is a percentage of the tool diameter.
Length Through Cut - defines the amount, or distance, that the tool travels through the material after it has reached the bottom of the stock in through-hole machining. This distance does not include the tool point. This value is only used for hole operations that have been set to Through Hole in the feature wizard.
Peck Retract Amount - determines the distance that the drill retracts in the hole to start the next peck rather then retracting to the clearance plane.
Add To Drill Depth Blind Tap - adds an extra constant amount to all drill depths when blind-hole tapping. This generally used for machines that do not have rigid tapping, or when some older machines, in the process of reversing the tap direction, make extra revolutions before stopping. This value acts as a safety to avoid breaking taps.
Hole Rapid Clearance - defines the distance above the workpiece at which the tool movement switches from rapid feedrate to cutting feedrate. This value is used for all hole operations.
Dwell Seconds - sets the dwell value to a specific measure of time (in seconds). Type the value to set how long the tool dwells for drill operations.
Dwell Revolutions - sets the dwell value to the number of complete spindle revolutions the tool must complete during the dwell.
Pre-drill Depth Extension Multiplier - automatically calculates the drilling depth in reaming jobs with blind holes when the drilling depth is less than or equal to the reaming depth. This value is used in place of the Ineffective Length box in the assigned reamer tool if this tool parameter is set to 0.0. The additional drilling amount is equal to the reamer diameter multiplied by this value.
Reamer Finish Allowance 1 Large - is the value used for the first step of a two step finishing process if the reamer outside diameter is greater than 0.118. The system allows you to use one or two finishing steps between the drill and reamer operations of the reaming job. These are normally performed with end mills. The end mill that is automatically selected has a diameter equal to the reamer diameter minus the Reamer Finish Allowance 1 Large.
Reamer Finish Allowance 2 Large - is the value used for the second step of a two step finishing process if the reamer outside diameter is greater than 0.118. The system allows you to use one or two finishing steps between the drill and reamer operations of the reaming job. These are normally performed with end mills. The end mill that is automatically selected has a diameter equal to the reamer diameter minus the Reamer Finish Allowance 2 Large.
Reamer Finish Allowance 1 Small - is the value used for the first step of a two step finishing process if the reamer outside diameter is less than or equal to 0.118. The system allows you to use one or two finishing steps between the drill and reamer operations of the reaming job. These are normally performed with end mills. The end mill that is automatically selected has a diameter equal to the reamer diameter minus the Reamer Finish Allowance 1 Small.
Reamer Finish Allowance 2 Small - is the value used for the second step of a two step finishing process if the reamer outside diameter is less than or equal to 0.118. The system allows you to use one or two finishing steps between the drill and reamer operations of the reaming job. These are normally performed with end mills. The end mill that is automatically selected has a diameter equal to the reamer diameter minus the Reamer Finish Allowance 2 Small.
Dwell Seconds - sets the dwell value to a specific measure of time (in seconds). Type the value to set how long the tool dwells for ream operations.
Dwell Revolutions - sets the dwell value to the number of complete spindle revolutions the tool must complete during the dwell.
Chamfer Cutting Position - defines the default tool position for chamfer milling operations. The distance is used to determine which part of the angular cutting edge of the chamfer milling tool is cutting the chamfer. The distance from the bottom of the chamfer to the bottom of the tool is the value that is needed.
Dwell Seconds - sets the dwell value to a specific measure of time (in seconds). Type the value to set how long the tool dwells for chamfer operations.
Dwell Revolutions - sets the dwell value to the number of complete spindle revolutions the tool must complete during the dwell.
Counterbore Mill Finish Allowance Small - is used to help the system select an end mill that is used for counterbore milling operations. If the counterbore diameter is less than or equal to 0.5 inches, then the selected end mill is less than or equal to the counterbore diameter minus this value.
Counterbore Mill Finish Allowance Large - is used to help the system select an end mill that is used for counterbore milling operations. If the counterbore diameter is greater than 0.5 inches, then the selected end mill is less than or equal to the counterbore diameter minus this value.
Dwell Seconds - sets the dwell value to a specific measure of time (in seconds). Type the value to set how long the tool dwells for counterbore operations.
Dwell Revolutions - sets the dwell value to the number of complete spindle revolutions the tool must complete during the dwell.
Feed per revolution - sets the tap feedrate value to use feed per revolution.
Feed per minute - sets the tap feedrate value to feed per minute.
Dwell Seconds - sets the dwell value to a specific measure of time (in seconds). Type the value to set how long the tool dwells for bore operations.
Dwell Revolutions - sets the dwell value to the number of complete spindle revolutions the tool must complete during the dwell.
