Tool Trajectory Parameters: Turning > Contour - Contour Tab

Take a single turning pass along a shape, creating a smooth surface finish.
Used for finishing operations.

The Tool Trajectory parameters for Turning > Contours are displayed in a dialog. The Contour tab is displayed below.

Contour Cut Options

Contour Entry and Exit

Contour Style

Chip Break

Contour Cut Options

These checkboxes indicate the direction the tool will move along the designated cut shape.

Cut Side X+

Cut Side tells you which side (usually X+ or X-) will be cut. To flip the positioning, select or deselect the Cut Other Side checkbox.

Cut Other Side

Forward

This indicates the direction the tool will move along the designated cut shape.
When this option is ON, the tool will move from the Start Point to the End Point of the selected cut shape as designated in the Geometry parameters.
When this option is OFF, the tool will move from the End Point to the Start Point of the selected cut shape.

Square Corners

Determines the external corner moves for a cut shape.
When this option is ON, the system does not add a radius move at the corners of the cut shape. Instead, the tool makes sharp moves only when going around a corner and will leave contact with the finished shape, possibly creating a burr at the corner.
When this option is OFF, the system automatically makes a radius move when rounding a corner, so that the tool always stays in contact with the part.

Cut Off

For use with cut off tools.
When this option is ON, the system creates deep grooves to remove (Cut off) a part from its parent stock. This process is also known as Part Off.

Rapid In

Specify the move speed from the Entry Clearance Plane position to the start point of the toolpath.
When this option is ON, the move will be a rapid move
When this option is OFF, the move will be feed move.
The Rapid In option should be used with caution, as it can create rapid moves directly into the part material. Available only when Use Auto Clearance is not selected. To use Rapid In, a post modification is required.

No Drag

Indicates how the contour will be cut.
When this option is ON, the toolpath is created in such a way that only the positive insert angle of the tool cuts material. The designated cut shape is segmented into pieces to accomplish this.
The tool will finish one side of the groove, rapid up and over, and then go down and finish the other side of the groove, always cutting along the positive direction of the insert angle, so all cutting will be "pushing" the insert, not "pulling" it. This eliminates drag or cutting with the back side of the insert.

Approach/Retract Type

The Approach/Retract Type selection designates the axis along which the tool will approach and retract from the part. These are similar for all Turning procedures, with the exception of Lathe Drill.

On most turning machines, X is radial and Z is axial, as shown below.
Xr indicates a Radius dimension; Xd indicates a Diameter dimension.

The OD (Outside Diameter of the part) and Front ID (Front Inside Diameter of the part) approach type options specify that the tool approaches and retracts radially along the X axis, on most turning machines.
The Front Face and Back Face approach type options specify that the tool approaches and retracts axially along the Z axis, on most turning machines.

Once the Approach Type is selected, the corresponding Clearance diagram appears in the Process dialog. The boxes with the arrows next to them represent the Entry and Exit Clearance Positions that the tool may use when approaching and retracting from the part; both boxes are labeled with arrows going towards and away from the part, respectively. The Entry and Exit Clearance Positions are only required when Auto Clearance is turned OFF.

Entry Clearance Diameter/Radius specifies the location to which the tool will make a rapid move, before it begins to feed radially to the operation's start point.

Exit Clearance Diameter/Radius specifies the location to which the tool will make a rapid move, after it has completed cutting at the operation's end point.

The OD approach type option deploys the toolpath on the Outer Diameter of the part.

For this option, the following Clearance Diagram is displayed:

Entry Clearance

Exit Clearance

Front ID

The Front ID approach type option deploys the toolpath on the Front Inner Diameter of the part.

For this option, the following Clearance Diagram is displayed:

Entry Clearance

Exit Clearance

Front Face

The Front Face approach type option deploys the toolpath onto the Front Face (Z+) of the part.

For this option, the following Clearance Diagram is displayed:

Entry Clearance

Exit Clearance

Back Face

The Back Face approach type option deploys the toolpath onto the Back Face (Z-) of the part.

For this option, the following Clearance Diagram is displayed:

Entry Clearance

Exit Clearance

Auto Clearance

Specify whether the clearance positions are to be calculated automatically by the system or are fixed positions based on a user-defined part clearance position.
When this option is ON, the system will calculate the clearance positions automatically. In this case, the diagram will disable the clearance position values because they are calculated based on the Auto Clearance value.
Auto Clearance Additional Information:Auto Clearance Additional Information:

The Auto Clearance option performs several functions when it is turned on. It will calculate the part clearances in both Z and X that are used to position the tool between each operation. These positioning moves will be dynamically calculated for each operation. This means that as the stock conditions of the part change as material is removed, the clearance positions will adjust accordingly.

When Auto Clearance is ON, the system will also take into account where the tool needs to be to begin the next operations' toolpath when calculating the positioning moves. Additionally, the Auto Clearance function may add entry and/or exit moves to the toolpath in order to safely maneuver around the part. The Auto Clearance function generates the most efficient positioning moves around a part. However, canned cycles cannot be used in conjunction with Auto Clearance. In order to use canned cycles, which are turned on in Process (Tool Trajectory) dialogs by selecting the Prefer Canned option, Fixed Clearance positions must be used.

The Auto Clearance option requires the user to enter an offset amount from the part stock that the system uses to calculate the clearance positioning moves between operations. Because the stock conditions are constantly changing as material is removed from the part, in order to optimize the toolpaths, an offset amount is used for positioning rather than absolute positions. Fixed clearance, which is used when Auto Clearance is turned off, uses absolute positions.

When this option is OFF, fixed clearance positions are used by the system to calculate clearance moves. In this case, you need to enter an overall part clearance in the Clearance & UCS Motion Parameters (in the Xr/Xd and Z text boxes), as well as Entry and Exit Clearance Positions in the Process dialogs for each operation. When using canned cycles, fixed clearance positioning should be used.
Fixed Clearance Additional Information:Fixed Clearance Additional Information:

When the Auto Clearance option is turned OFF, fixed clearance positions are used by the system to calculate clearance moves. The user must enter an overall part clearance in the Clearance & UCS Motion Parameters, as well as Entry and Exit Clearance Positions in the Process dialogs for each operation. When using canned cycles, fixed clearance positioning should be used.

The overall part clearance is entered in the Clearance & UCS parameters in the Xr/Xd and Z text boxes that become active when Auto Clearance is turned off. They designate the position the tool will rapid to and from during a tool change. This position will also be used when moving from one approach type to another between operations that use the same tool. The absolute positions specified in the Xr/Xd and Z text boxes are locations the tool can rapid to when moving around the part. One or both of these fixed positions are used whenever a tool is moving to the start point of the toolpath or exiting from the toolpath. Where the tool moves when approaching and retracting from the part depends on the Approach Type selected and the positions specified in the Clearance Diagrams in the Process dialog.

Contour Entry and Exit

The Entry and Exit options can create additional movements that will be added to the toolpath.

Line

When this option is selected, a 90° arc of the specified radius value will be added to the toolpath. This arc will be tangent to the start feature at the start point. If a value is entered in the Line text box, a line of the specified length will be created tangent to the arc. Also, if this is selected and the radius value is zero, the line will not be perpendicular but instead will be parallel.

90° Line

When this option is selected, a line of the specified length will be added to the cut shape. This line will be perpendicular to the start feature at the start point.

Advanced

Selecting the Advanced option allows you to define custom Entry and Exit Moves using the Entry/Exit tab.

Contour Style

The Contour Style selection affects the toolpaths created for the current operation.

Material Only

When this option is ON, the system keeps track of material that has already been removed. Calculations are performed on the exact shape of material left from the initial stock shape and all prior machining operations. The toolpath will only feed over areas that have not yet been machined in previous operations, providing for "no air cutting."

Because of this, the order of operations directly affects how the part will be cut. If the order of operations is changed or operations are added or removed, all operations should be recalculated in order to account for the change.

Clearance

The Clearance value specifies an offset amount from the material that the system uses to calculate where the tool can safely rapid during an operation. If the tool is within the clearance amount, only feed moves will be allowed.
The Clearance value is available when the Material Only option is selected.

Full

The Full option gives you more control over toolpath creation.
When this option is ON, the toolpath generated will feed over the selected cut shape from the start point to the end point. The X Stock Start Position is displayed in the Clearance Diagram. The X Stock Start Position designates the position from which the first cut will be calculated.

Corner Break

The Corner Break value specifies a radius that will be put on every outside sharp corner of the selected cut shape. A value of zero will not break the corner, but will keep the tool in contact with the part as it moves to the next feature.

Corner Break is only available when Square Corners is not selected.

Fin. Stock ±

The Finished Stock value specifies the minimum amount of material that will be left outside the part geometry (equally on all faces) after a toolpath is completed. The toolpath will be offset from the part geometry in Z and in Xd. This excess material is removed with the finish pass.

Xr Stock

The Xr Stock value allows you to specify any additional stock amount for the X axis. The value entered here specifies the amount of material that will be left on the cut shape along the X axis only.

Z Stock

The Z Stock value allows you to specify a stock amount for the Z axis. The Z Stock value specifies the amount of material that will be left on the cut shape along the Z axis only.

Cutter Radius Compensation On

A checkbox that indicates whether Cutter Radius Compensation (CRC) is turned ON or OFF .

When this checkbox is ON , the selected compensation is as defined in the Cutter Compensation - Turning Output default parameter in the Preferences; Cutter Compensation by Tip Location or by Geometry Location.

Cimatron has a number of rules for when and where it will generate CRC markers. These rules have been chosen so as to be as safe as possible for the widest range of machines. This means that while a specific machine may be able to handle different CRC rules, Cimatron will not generate markers for all cases by default. CRC rules on arcs are the primary example of this.

For new toolpaths, the system will do the following:

CRC will be activated on entry moves, before the entry arc. If there is no move before the entry arc, CRC will be activated on the arc. The system has a warning that will tell you when you are using CRC without a line move. In general, the system considers CRC activation on an arc to be an invalid case, because it does not accurately cut the arc.

CRC will be activated on exit moves, after the exit arc. If there is no move after the exit arc, the CRC deactivation will be made on the Depth move. Again, the system will warn you when you do not have a line move. In general, the system considers CRC deactivation on an arc to be an invalid case, because it does not accurately cut the arc.

Some Operations have the option of deferring CRC activation until later in the toolpath (roughing with a finish pass.) Rules 1 and 2 will be applied to the finish pass only.

For old Toolpaths, the system will only follow rules 1 and 2. No markers will be added for rapids imbedded in the toolpath.

When exiting the Process dialog by clicking the OK button, the cutter compensation mode is displayed, dimmed, in the Enable Cutter Compensation field of the procedure's parameter table grid, under Machine Parameters.

When this option is OFF, the following is displayed in the parameter table:

When this checkbox is ON , the selected compensation is as defined in the Cutter Compensation - Turning Output default parameter in the Preferences; for example:

See Cutter Compensation for additional details.

Cut Direction Axes

The Cut Direction Axes checkboxes allow you to limit motion along the cut axis, thereby regulating the axes and directions of the cut shape.
Deselecting an axis will prevent cut shape moves in that axis direction. The default settings should have all axes selected.
Example:Example:

The X- checkbox has not been checked. This means the tool will not travel in the X- direction.	The X- checkbox has been checked. The tool moves in the X- direction.

Chip Break

The Contour and Rough Turning procedures provide a Chip Break capability which give you the ability to break off chips according to set parameters.

These parameters are useful when machining material that is soft or spongy, where chips can sometimes be quite long, interfering with the machining of the part.

Note: A post change is required if your existing post does not support the output of Dwell in the toolpath. If you are unsure, contact your Provider or Reseller to verify or request a modification.

Pull Off

When this checkbox is ON , you can specify how far the tool will retract from the stock.

Dwell

When this checkbox is ON , you can specify how many revolutions the tool will stay in place before it continues to cut.

Chip Length

Specify the length of chip to tolerate before Pull Off and/or Dwell occur. The length of chips that are removed will remain constant even though the circumference of the stock diminishes (in an OD process).
This option is available if either the Pull Off or Dwell options are selected.