Speeds.

You can specify spindle speed values, which the system outputs to the NC program at S address (ISO).

Spindle Speed (n), rev/min.

The system shows the spindle rotation speed in revolutions per minute. Adjusting this value manually triggers an automatic recalculation of the cutting speed and any non-selected feed rates.

Cutting Speed (Vc), m/min.

The cutting speed is displayed in meters per minute—it represents the circumferential speed of a point on the cutting edge during the cutting process. This value is calculated from the Spindle Speed and Cutting Diameter (DC). If modified manually, the spindle speed and unselected feed rates are updated automatically.

Cutting Diameter (DC), mm.

In the case of a rotating tool, this is the diameter of the circular path traced by a point on the cutting edge during rotation and cutting. For turning, it represents the initial diameter of the machined surface..

Feeds.

Set the feed rate values, and they will be transferred to the NC program at F address (ISO).

Table feed (Vf), mm/min.

The interface displays the feed rate per minute, which defines the relative movement speed of the tool and workpiece in mm/min. Manual adjustments will cause the system to update the other feed rates automatically.

Feed per revolution (fn), mm/rev.

The interface displays the feed per revolution, which defines the tool’s displacement in the feed direction per one full rotation of the tool or workpiece. This value is derived from the Feed per tooth and the Number of effective teeth (Zc). If modified manually, the system will update the other feed values automatically.

Feed per tooth (fz), mm/tooth.

The system shows the feed per tooth, which defines the displacement of the tool’s center in the feed direction as it rotates by one tooth (Zc). Modifying this value manually will automatically update the other feed values.

Number of effective teeth (Zc).

The count of tool cutting edges (teeth) available for use in the cutting process.

After setting and recalculating the values in the calculator, select the type of speed and feed that should be output to the NC program.

Spindle Speed.

Specify the direct spindle speed in revolutions per minute (RPM) or cutting speed in meters per minute (CSS). In the second case, the CNC system continuously calculates and adjusts the spindle's revolutions per minute based on the current workpiece diameter. Instead of a fixed revolutions per minute, only the maximum allowable value is specified.

Max RPM.

If the spindle speed is set via cutting speed, it is necessary to specify the maximum rotational speed to restrict its increase when the diameter changes.

RPM before CSS.

In turning operations, this parameter enables RPM mode at the tool change position and activates CSS mode following the approach moves.

If the tool is positioned at the tool change point and the spindle is activated in CSS mode, its rotation will be slow since the tool is far from the workpiece’s rotational axis. During the first rapid movement when the tool approaches the workpiece, the spindle accelerates significantly, causing extreme loads on the machine. To prevent this, some machine manufacturers recommend initially running the spindle in constant RPM mode and switching to CSS after the tool approaches the workpiece. When the "RPM before CSS" option is enabled, the spindle first runs in RPM mode at the speed corresponding to the first cutting feed point, then the approach movement is executed, and finally, the mode switches to CSS.

Range.

Specify the range number required to obtain the desired spindle speed on a machine with a mechanical gearbox.

Rotation direction.

Configure the spindle rotation direction.

Forward.

This is a clockwise spindle rotation when viewed from the motor side, represented in the NC program by M3. If a tool is installed, this direction tightens a right-hand screw. In turning operations, the spindle rotates towards the operator.

Reverse.

This is a counterclockwise spindle rotation when viewed from the motor side, represented in the NC program by M4. If a tool is installed in the spindle, this direction corresponds to tightening a left-hand screw. In turning operations, the spindle rotates away from the operator.

Grip RPM . The subspindle performs the part capture at this RPM.

Plunge speed.

In a Roughing Waterline operation, a specific spindle speed can be defined for the cutter's plunge movement into the material when milling enclosed surfaces like pockets. See more.

Flood.

Activating this parameter initiates coolant supply through the nozzle.

Mist.

Compressed air sprays the liquid to produce a mist and transports the air-liquid mixture to the cutting zone.

Tool.

Activating the parameter enables coolant delivery under pressure through the tool channels.

Coolant 4.

Activating the parameter enables coolant delivery to the tool using an alternative method, such as an air blast.

Work feed (in lathe operations Cut Feed).

The primary feed rate value maintained for stable cutting during the process. In roughing operations material removal will be performed at this speed, in finish – detail surface machining.

Calculable.

In the milling operations the feed value can be either permanent or calculated, depending on the slope angle of every elementary toolpath section. When assigning a calculated feed, defining will be feed values and coefficients when moving down, horizontally and up. The real feed values when moving down, horizontally or up will be equal to multiplication of the corresponding correction coefficient to the feed value. With intermediate values of slope angle of an elementary toolpath section, the real feed value will be calculated proportionally to the defined border values. For example, with a feed values equal to up 300, horizontally – 200, down – 100, the real feed value on a section with tool movement up under angle of 45 degrees will be equal to 250. Use of the calculated feed, allows the user to decrease the machining time due to more flexible control over cutting modes.

Up feed value.

Feed rate during vertical upward motion of the tool.

Down feed value.

Feed rate during vertical downward motion of the tool.

Engage feed.

The feed rate value used for engage movement. See more.

Retract feed.

The feed rate value used for retract movement. See more.

First feed (in lathe operations First Cut Feed).

The feed rate applied during working passes at the initial cutting depth. First feed is useful when machining a workpiece with an initial tough exterior (skin).

Finish feed (in lathe operations Finish Cut Feed).

The feed rate value used for finishing passes in operations with separate roughing and finishing stages. It is advised to use when need to obtain a surface of high quality after a roughing operation.

Plunge feed.

Feed applied to tool plunge moves, for example, it ia applied for plunging to a lower machining layer in waterline roughing and pocketing operations. See more.

Chip Breaking Feed.

In lathe operations, this value specifies the speed for retracting from the workpiece and repositioning during chip breaking.See more.

Adaptive feedrate.

The feature automatically adjusts the toolpath feedrate based on the actual tool engagement. So it reduces feedrate in tight corners where the tool engagement approaches 100% and increases feedrate as the tool engagment approaches 0% (the air cutting).

To activate this parameter, the main condition is the width of the overlap.

The tool engagement approaches 100% (Ae~100%). Option is active. The zones are marked in black in CAM system.

Full Cut Feed. Minimum final feed, in percents of the Work Feed.

Fmin - Full Cut Feed

No Cut Feed. Feedrate on return from the zone (without cutting), in percents of the Work Feed.

Fnot - No Cut Feed

Feed Increment. Step to change feed.

Mark overloads. Allows you to mark the segments where the tool engagement is maximal in the Simulation tab. In the parameter you can specify the value from the work feed that needs to be marked.

Override Feeds.

This parameter becomes available in lathe operations, and its activation allows defining separate feed rate settings—Cutting, Engage, Retract, Finish Cutting, and Traversal feeds—for designated cycles in the Job Assignment.

Rapid feed.

The feed at which all rapid tool transitions (positioning) are performed. Its value is the rapid motion velocity for the current machine. Movements at this speed are output to the NC program under the G00 address. This figure is used to calculate accurate machining process time. Toolpath sections, performed at rapid feed are displayed in red. When switched to rapid feed, the system creates the RAPID command in the CLDATA program.

Short link feed.

The feed rate applied to transition movements executed according to the Short Links rule. See more.

Long link feed.

The feed rate applied to transition movements executed according to the Long Links rule. See more.

Approach feed.

The feed rate applied for the approach movement, covering the distance from Feed Distance to the start of the Plunge or Engage. See more.

Approach from safe surface feed.

The movement speed value from the Safe Surface to the Feed Distance. See more.

Return to safe surface feed.

The movement speed value from the Feed Distance to the Safe Surface level. See more.

Transition on safe surface feed.

The movement speed value during the links over the Safe Surface. See more.

Traversal Feed.

In lathe operations, this speed defines the transition rate from one work pass to the next.

Return feed.

In milling operations, this is the movement speed from the end of the Retract motion to the Feed Distance level. In hole machining operations, this is the retraction speed in some drilling cycles. e.g. deep drilling cycles with chip removal or breaking. See more.

Rapid idle moves (Rapid non-work moves).

When this parameter is activated, all the tool retraction movements from the machining areaб intended to be performed at Return feed rate are instead executed at Rapid feed.