2.5 to 5-axis Drilling Operations

The overall plunge distance is determined as follows:
       Approach clearance + (Plunge depth - Plunge offset)
where Plunge depth is determined by a tool tip or tool diameter value.

The manufacturing attribute is MFG_PLUNGE_MODE.

• Revolutions: Specifies the number of revolutions for the dwell
• Time: Specifies the time duration of the dwell.

• By linear coordinates
  Shift along X: Specifies the shift along X
  Shift along Y: Specifies the shift along Y
  Shift along Z: Specifies the shift along Z

• By polar coordinates
  Shift distance: Specifies the shift distance
  Shift angle: Specifies the shift angle

• None.

The values entered for the selected shift mode determine the angle at which the active part of the boring bar stops and the amount of the tool displacement.

For a shift defined by polar coordinates (90deg, 1.5mm), the tool is displaced 1.5mm as indicated by the arrow in the figure below.

The same shift motion could be obtained by the linear coordinates (0mm, 1.5mm, 0mm).

• each peck in a Drilling Deephole operation

• each break chips pass in a Drilling Break Chips operation.

The manufacturing attribute is MFG_AXIAL_DEPTH.

The manufacturing attribute is MFG_RETRACT_CLEAR_TIP.

• the back motion used to break chips after each drilling pass in a Drilling Break Chips operation

• the offset where machining feedrate starts before each new peck in a Drilling Deephole operation.

The manufacturing attribute is MFG_OFFSET_RET.

Depth of peck 1 = Max depth of cut (Dc)
Depth of peck 2 = Dc * (1-Decrement rate)
Depth of peck 3 = Dc * (1-2*Decrement rate)
and so on.

If Decrement rate is equal to zero, the Maximum depth of cut is applied at each new peck as a constant step.
The manufacturing attribute is MFG_DEPTH_DEC.

Decrement limit
Coefficient used to determine the maximum allowed depth of cut for a peck in a Drilling Deephole operation.

The depth of a new peck never becomes smaller than the Maximum depth of cut multiplied by the Decrement limit.

That is:
Depth of current peck > Maximum depth of cut * Decrement limit.

When:
Depth of current peck = Maximum depth of cut * Decrement limit
this depth is kept for all remaining pecks until the total depth is reached.

The value of Decrement limit must be greater than zero.
The manufacturing attribute is MFG_DEPTH_LIM.

Example of Decrement rate and Decrement limit:

A Drilling Deephole operation uses the following parameters:
Maximum depth of cut = 10mm
Decrement rate = 0.1
Decrement limit = 0.8

Therefore, depth of current peck will always be greater than 8mm (that is, 10mm*0.8).

Depth of peck 1 = 10mm
Depth of peck 2 = 9mm
Depth of peck 3 = 8mm
Depth of remaining pecks = 8mm.

Rotary motions are displayed during Replay.
ROTABL/ instructions are generated in the output file.
Facilitates environment setup by minimizing the requirement on post processors (avoids having to deal with X, Y, Z, I, J, K outputs for rotary tables).
Provides the NC programmer with a more accurate tool path simulation for machine tools with rotary table.

Note: No rotary motion is performed if a linking macro motion is defined (and activated) on the drilling operation. If activated, the linking macro is always performed between the points to machine.

If you want to generate CYCLE statements, you must select the Output CYCLE syntax checkbox in the Strategy tab page and set the Syntax Used option to Yes in the NC Output generation dialog box.
Otherwise, GOTO statements will be generated.

Note that when several axis orientations are present in a machining pattern, output of the components of the tool axis orientation is possible whenever the NC data format is set to Axis (X, Y, Z, I, J, K) in the Part Operation's Machine Editor.

• Output point: the tool compensation point is generated in the output file. The toolpath computation is done according to the tool tip.
• Guiding point: the tool motion is computed according to the tool compensation point and the tool compensation point is generated in the output file.

Note that the tool compensation point is defined on the tool and used on the operation.
The Compensation application mode defines the tool position to reach.

Toolpath computation and Output Point

If Compensation Application Mode is set to Output point then Depth mode option (Tip/Shoulder or Distance/Diameter) is taken into account for tool path computation.

Examples:
P2 compensation is defined on the tool and used on the drilling operation.
Compensation application mode = Output point.

Depth mode = Tip	Depth mode = Shoulder
The active compensation point (blue dot in figures above) is only used as output point in the generated file (APT source).

Toolpath computation and Guiding Point

When Compensation application mode is set to Guiding point, the tool compensation point selected on the operation is taken into account to respect the depth to machined on the operation.

All the points to reach with the tool are computed with respect to the activated compensation point. In this case Depth mode (Tip/Shoulder or Distance/Diameter) is no longer taken into account.
Only the tool compensation point is used to compute the different tool positions to reach during the cycle.

Example:
P2 compensation is defined on the tool and used on the drilling operation.
Compensation application mode = Guiding point.

The active compensation point is represented by the blue dot in figures above.

If Compensation application mode is set to Output point then tool path computation is done without modification: Depth mode option (Tip/Shoulder or Distance/Diameter) is applied, if it exists on the operation.

Tool Path Output

• GOTO statements output:
  The tool compensation point is always generated in the output file.
  There is no influence of the Output point or Guiding point option.
• CYCLE statement output
  Coordinates of points between CYCLE/ and CYCLE/OFF statements are always the coordinates of the points to machine.

Output File Generation

Cycle parameters (%MFG_TOTAL_DEPTH, %MFG_TOTAL_DEPTH_COMP) valuation depends on the Compensation application mode defined on the operation.

%MFG_TOTAL_DEPTH and %MFG_TOTAL_DEPTH_COMP are computed parameters.

• MFG_TOTAL_DEPTH: Total depth machined by the operation. This includes the hole depth, breakthrough, and tool tip length.
• MFG_TOTAL_DEPTH_COMP: Total depth machined by the operation up to the tool compensation point selected for the operation. This includes hole depth, breakthrough and tool tip length up to the compensation point.

Then the value depends on the tool compensation used on the operation (if Compensation application mode is set to Guiding point).

The parameter %MFG_COMPENSATION_MODE (1: output point / 2: guiding point) can be defined on the NC instruction of the axial machining operation.

Climb or  Conventional

Climb: the front of the advancing tool (in the machining direction) cuts into the material first
Conventional: the rear of the advancing tool (in the machining direction) cuts into the material first.

• Top to bottom: tool motion is from the top to the bottom of the thread. This involves conventional cutting.
• Bottom to top: tool motion is from the bottom to the top of the thread. This involves climb cutting, and results in a better quality thread.

Machining strategy
Specifies how the tool path is to be computed.

• Mono-pass (default value)
  Machining motion is done in one pass. Tool is considered as a mono-cutting level tool.
• Optimized passes
  This strategy is useful for thread mill tool (more than one cutting level exists on the tool). It is not available when a boring bar is used.
  Toolpath depends on the tool characteristics and thread depth.
  One or more helical (height = pitch) toolpaths can be generated: the number of helical toolpaths depends on the effective thread length of the tool and the thread depth of the hole.

Note about thread mills and effective thread length:

Length1 depends on Cutting length (Lc) and Taper angle (Ach). See Thread Mill for geometry parameters.

Cutting levels on the tool is the number of thread pitches that can be machined during one helical motion.
The number of cutting levels is defined as follows:
Number of effective cutting levels = int (Length 1 / tool pitch)
Effective thread length = number of cutting levels * pitch.

Note that between helical toolpaths:

• approach macro motion is done before each helical motion
• retract macro motion is done after each helical motion.

The following figure illustrates the motion involved for 2 helical toolpaths.

Distance is defined from start of one helix motion to next start of next helix motion.
Distance = effective thread length of the tool + pitch.

Maximum depth of cut (Mdc)
Defines the maximum depth of cut in an axial strategy.
Number of levels (Nl)
Defines the number of levels to be machined in an axial strategy.

Axial: axial machining is done first then radial
Radial: radial machining is done first then axial.

Pitch (P): Specifies the helix pitch
Angle (Ang): Specifies the helix angle.

The following options are proposed:

• If 2D Radial profile is selected, both the tool tip and cutter profile will be visualized during tool path replay. Cutter compensation instructions are automatically generated in the NC data output. An approach macro must be defined to allow the compensation to be applied.
• If 2D Radial tip is selected, the tool tip will be visualized during tool path replay. Cutter compensation instructions are automatically generated in the NC data output. An approach macro must be defined to allow the compensation to be applied.
• If None is selected, cutter compensation instructions are not generated in the NC data output. In this case, please refer to How to generate CUTCOM syntaxes.

Helical Interpolation for Circular Milling and Thread Milling

A helical interpolation instruction can be generated in the output file (APT source or Clfile) for helical tool motions. The machine specified on the Part Operation must support Helical interpolation and the corresponding checkbox must be selected in the Machine Editor.
The Helical Interpolation option must be set to From machine in the Generate NC Output dialog box. If this option is set to None, then GOTO instructions are generated for the helical motion. For more information, see Generate APT Source or Generate Clfile.

Axial Machining Geometry Considerations

Geometry parameters are managed in the Geometry tab page .

Machining Patterns

A machining pattern comprises two sets of data:

• Pattern geometry: hole positions/axes, top element
• Pattern usage or technology data: Ordering mode, Jump distance, local entry/exit distances, local depth, activate/deactivate status.

When you create a new axial machining operation, the New Pattern command in the list prompts you to create a machining pattern for the operation.

You can add positions to this new machining pattern by clicking the sensitive text (No Point or x Points). This opens the Pattern Selection dialog box that lists all available machining and design patterns. Just select one of the existing patterns and/or select geometry in the 3D view to define the hole positions.

The new machining pattern is created when you create the machining operation. The pattern geometry and technology data is stored and the new pattern is assigned an identifier Machining Pattern.x.

If there are already machining patterns on previous operations, the list allows a quick selection of an existing pattern. If selected, the existing pattern is shared between the operations.

You can also use the following commands in the list for assigning a machining pattern to the operation.

Copy from Current: The machining pattern (geometry and technology data) is duplicated. The pattern cannot be shared. It is possible to modify the machining data in the current machining operation without impacting other operations.

New from Current (share geometry): The machining pattern (geometry and technology data) is duplicated. The pattern can be shared. If the pattern is modified, all operations using it will be impacted.

New Pattern: A new machining pattern is created with the geometry and technology data that you specify.

Modification of a machining pattern is possible using the Machining Pattern editor only. This editor can be opened by double-clicking the machining pattern in the manufacturing view. Please refer to Machining Patterns for more information.

Note that it is possible to reference in a machining pattern one or more 3D Wireframe features (that is, Projection, Symmetry, Rotation and Translation operators) containing at least one point.

Tool Axis Initialization from Pattern Selection

When you select pattern points by means of design holes or circular edges, the orientation of tool axis is automatically initialized using semantic information related to the selected geometry.

If a geometrical point is selected there is no semantic information to determine the tool axis. In this case, the tool axis is initialized from the z-axis of the absolute axis system.

You can modify the tool axis by right-clicking a pattern point and selecting Edit Local Axis (see Contextual Menu on Pattern Points for more information).

Pattern Ordering Modes

Holes that are selected for a machining pattern can be ordered according to the following modes:

• Closest: to obtain the shortest possible tool path
• Manual: to obtain a user-defined numbered sequence
• By Band: to obtain a Zig Zag or One Way configuration according to a set of bands that have a user-defined width.
  • Zig Zag ordering of a pattern of 40 points for a band width of 18mm is illustrated below:
    
  • One Way ordering of the same points and same band width is illustrated below:
• Reverse Ordering: Reverses the numbered sequence of pattern points (for example, points numbered 1 thru 10 will become numbered 10 thru 1).

Managing Pattern Points

Contextual Menu on 'No Points / x Points' Sensitive Text

A number of contextual commands are available for managing hole positions when you right click the 'No Points / x Points' sensitive text in the Geometry tab page.

• Remove All Positions: Removes all positions from the pattern.
• Remove: Displays a dialog box for removing selected positions from the pattern.
• Deactivate: Displays a dialog box for deactivating selected points of the pattern.
  
• Move After: Displays a dialog box for moving one or more positions after a specified position in the pattern. Only available when Pattern Ordering mode is set to Manual.
• Analyze: Displays the Geometry Analyser for consulting the status of the referenced geometry.
• Find Features Through Faces: Allows you to quickly locate circular edges in a selected face. Please refer to Select Hole Design Features for Machining.

Contextual Menu on Pattern Points

A number of contextual commands are available when you right-click a pattern point.

• Deactivate the Point: Deactivates the selected point in the pattern. An O symbol indicates that the point is omitted from the pattern. A deactivated point can be activated in the pattern again.
• Invert Selection: All omitted points are retained in the pattern again; pattern points become omitted points.
• Select All: Allows you to include all omitted points in the pattern again.
• Set as Start Point: Allows you to choose the start point for the pattern.
• Renumber: Allows you to renumber points in the pattern. Only available when Pattern Ordering mode is set to Manual.
• Edit Entry Distance and Edit Exit Distance:
  Allows you to locally edit Entry and Exit distances at individual points in a hole pattern. This can be useful for locally specifying a clearance that is greater than the one defined by the jump distance/approach clearance discussed below.
• Edit Depth: Allows you to edit the depth of a pattern point.
• Restore Associativity: Restores the original values taken from the selected design feature if these were modified by the user, and so restore associativity with the feature.
• Edit Local Axis: Allows you to locally modify the tool axis at a point. The Tool Axis dialog box appears.

  Choose one of the proposed methods for defining tool axis orientation: Manual. Choose one of the following: Components to define the tool axis orientation by means of I, J and K components. Angles to define the orientation by means of a rotation specified by means of one or two angles. Selection. If you select a line or linear edge, the tool axis will have the same orientation as that element. If you select a planar element, the tool axis will be normal to that element. Points in the View. Just select two points to define the orientation. Feature defined. Select a machining feature in the 3D viewer. For example, if you select an axial machining feature then the axis of the feature is taken as the tool axis. The tool axis is visualized by means of an arrow. The direction can be reversed by clicking Reverse Direction in the dialog box. Just click OK to accept the specified tool axis orientation. You can also choose to display the tool at the Default position or at a User-defined position. For a user-defined position, click the [...] button and select the desired position in the 3D viewer. For more information about this dialog box please refer to Define the Tool Axis.

• Insert after Current Position: Allows you to insert one or more positions (or patterns) after the current point in the pattern. Only available when Pattern Ordering mode is set to Manual.
• Remove Current Position: Deletes the current point from the pattern.
• Remove Linked Positions: Deletes the current point and all linked positions from the pattern. Linked positions are points from the same design pattern, for example.

Inversing Pattern Ordering

An Inverse pattern ordering checkbox is available in the Geometry tab page to allow an operation to locally override the ordering of the Machining Pattern by inversing it.

• If not selected, the Machining Pattern will be machined as defined (and as shown in the 3D view).
• If selected, the tool path computation will begin at the last point and finish at the first point.
  This will not modify the ordering on the Machining Pattern: the pattern numbers shown in the 3D View are not modified.

This option is useful in the following cases.

• When machining symmetrical parts. Please refer to Opposite hand machining.
• To save machining time when managing two operations sharing the same Machining Pattern on a large part. The first operation can be set to machine from the first position to the last one, and the second operation can be set machine from the last position to the first one.

Overall Tool Axis Orientation

Right click the Tool axis strategy sensitive text in the Geometry tab page and select one of the following options to specify the general tool axis orientation:

• Fixed Axis: the tool axis orientation is the same for all the selected points

• Variable Axis: the tool axis orientation can vary from one point to another

• Normal to PS Axis: the tool axis orientation is determined by the normal to the selected part surface.

Note that the tool axis orientation can be inverted by clicking the tool axis symbol in the Geometry tab page.

Projection and Top Element Modes

In the Geometry tab page you can choose between Projection and Top Element modes by clicking on the sensitive text.

The following figure illustrates Projection mode. The reference pattern points are projected onto the selected part surface. The projected points and the axes normal to the surface define the hole positions to be drilled.

The following figure illustrates Top Element mode. The reference pattern points define the hole positions to be drilled. The machining depth takes into account the normal distance between the reference points and the selected part surface.

Bottom Plane

If a bottom plane is selected, the machining depth is the distance between the hole origin and its projection on the bottom plane. This machining depth is computed for each hole in the machining pattern.

The depth shown in the geometry panel is the machining depth computed for the first hole. The Machine different depths setting is ignored when a bottom plane is selected.

Origin Offset

You can specify an Origin Offset in order to shift the entire tool path by the specified amount.

Jump Distance

The jump distance allows an extra clearance for moving in Rapid motion between the holes to be drilled whenever this distance is greater than the approach clearance.
For example, for an approach clearance of 2.5mm and a jump distance of 10mm, the extra clearance is 7.5mm.

Holes at Different Levels

For 2.5-axis operations, the program automatically manages holes at different levels using horizontal transition paths.

Machining Different Depths

When dealing with design feature holes in design patterns, both the result and specification mode are taken into account (except Spot Drilling, Counterboring, and Countersinking operations).

Select the Machine different depths checkbox in the Geometry tab page when you want the program to automatically manage different depths of holes in a pattern (result mode).

If the checkbox is not selected, the program uses the values specified in the Geometry tab page for the pattern holes (specification mode).

For Threading operations, select the Machine different thread depths checkbox when you want the program to take the real thread depth of each selected pattern hole into account.
Note: Different thread depths can be applied only when information exists on the geometry linked to the machined position. For example, thread information exists on a threaded design hole but none exists for a circular edge.
When no thread information exists on the geometry linked to the machined position, the depth defined on the operation is used.

Relimiting Hole Origins

The Relimit hole origin and Machine different depths checkboxes in the Geometry tab page can be used together to manage the machining strategy of different design hole configurations.

In the following figures the red star () represents the origin of the selected design hole, and the green star () represents the start of the tool path.

Machining Different Diameters

It is possible to machine different hole diameters in a Circular Milling operation thanks to the Machine different diameters checkbox on the Geometry tab page.

If selected, the diameter specified for each position of the machining pattern is machined.
Otherwise, the diameter of the first position of the machining pattern is used for all the pattern holes.

Managing Blind and Through Holes

A Machine Blind/Through checkbox is provided in the Geometry tab page.

If selected, the blind/through characteristic of the hole is determined for each position of the machining pattern.
If not selected, the blind/through characteristic of the first position of the machining pattern is used for all the pattern holes.

Note that the Machine Blind/Through capability is not available for user features.

Macros in Axial Machining Operations

The Macro tab page in the operation definition dialog box allows customized transitions paths for:

• approach
• retract
• linking linking between machining holes of the same pattern
• clearance, which can be used to define the feedrate on the horizontal path between two machining positions.

All types of macros used in Drilling Operations are collision checked. If a check element is specified between two machined positions, a linking macro is applied to avoid collisions. Check (or fixture) elements as well as an associated Offset on Check can be specified in the Geometry tab page.

Note that some specific axial machining operations support additional macro types:

• global approach and global retract (Circular Milling and Thread Milling)
• return between levels (Circular Milling and Thread Milling)
• return in a level (Circular Milling only).

Please refer to Define Macros on an Axial Machining Operation for more information.

Editing CYCLE Syntaxes in Axial Machining Operations

For all axial operations Edit Cycle in the Axial Machining Operation dialog box allows you to:

• display the unresolved syntax of the NC Instruction of the operation. This is the syntax as specified in the PP table referenced by the current Part Operation.

• display and, if needed, modify the syntax that is resolved either by geometric selection and user entries.

For example, the Cycle Syntax Edition dialog box appears when you select Edit Cycle in the Boring operation dialog box. It displays the default cycle syntax for the Boring operation.

You can access all the cycle syntaxes contained in the current PP table for a Boring operation by means of PP instruction .

For example, if your PP Table contains the following NC Instructions for Boring operations:

/
*START_NC_INSTRUCTION NC_BORING_1
*START_SEQUENCE
CYCLE/BORE,%MFG_TOTAL_DEPTH,%MFG_CLEAR_TIP
*END
*END
/
*START_NC_INSTRUCTION NC_BORING_2
*START_SEQUENCE
CYCLE/BORE,%MFG_TOTAL_DEPTH,%MFG_CLEAR_TIP,%MFG_BREAKTHROUGH
*END
*END
/
*START_NC_INSTRUCTION NC_BORING_3
*START_SEQUENCE
CYCLE/BORE,%MFG_TOTAL_DEPTH,%MFG_PLUNGE_OFFST,%MFG_CLEAR_TIP
,%MFG_FEED_MACH,%MFG_FEED_RETRACT
*END
*END
/
*START_NC_INSTRUCTION NC_BORING_4
*START_SEQUENCE
CYCLE/BORE,%MFG_TOTAL_DEPTH,%MFG_PLUNGE_OFFST,0,%MFG_CMP_DWL_TIME,%MFG_CLEAR_TIP
,%MFG_FEED_MACH,%MFG_SPNDL_MACH,ON,0,0,%MFG_FEED_RETRACT
*END
*END

Then these syntaxes will be displayed in the PP Words Selection dialog box that appears:

You can then select the desired syntax and click Apply to display it in the Cycle Syntax Edition dialog box. Just click OK to use the cycle syntax in the Boring operation being edited.

Note that in the example above, the PP Table contained several PP Instructions for the same operation type: NC_BORING_1 to NC_BORING_4.

Note that only one cycle syntax (delimited by *START_SEQUENCE / *END keywords) is allowed for each PP Instruction.

In this way, a multiple choice of syntaxes is proposed at programming time.

For more information please refer to Insert PP Instruction.