SR Documentation Requirements:
[pic]
Engineering Document
757-4002-505
VMX 42 SR
NC Post Processor Guide
Version: 1.2
Table of Contents
1 Revision Log iii
2 General Information 4
2.1 Machine and Workpiece Coordinate Systems 4
2.2 5-axis Part setup 4
2.3 3-axis part setup 6
2.4 Rotary direction convention 6
2.5 Tool Change Sequence 7
2.6 M31 rotary encoder reset 7
3 NC Program Syntax 8
3.1 Transform plane – Vector Input 8
3.2 Transform plane – Angle Input 9
3.2.1 Local vs. Global Rotations for Transform Plane 9
3.3 M126/127 shortest angular traverse 11
3.4 M200 Tilt axis preference 11
3.5 M128 TCPM 12
3.6 Axes Angle Input 13
3.7 Tool Vector Input 13
3.7.1 What is a Vector? 13
3.7.2 Activating and Cancelling Tool Vector Input Mode 15
3.8 3D Tool Geometry Compensation 15
3.8.1 Tool Geometry Specification 18
3.9 G43.4 5-axis linear interpolation 18
3.10 M140 tool vector retract 20
3.11 SR42 Machine Specifications 21
3.12 Inverse Time 21
Revision Log
|Name |Date |Revision Description |Version |
|Paul J. Gray |11/16/07 |Initial Document Release |REV 1.0 |
|Paul J. Gray |07/28/08 |Updated NC Transform Plane and G43.4 linear interpolation |REV 1.1 |
|Paul J. Gray |08/08/08 |Updated M141 Tool Vector Input Mode Cancel |REV 1.2 |
| | | | |
| | | | |
| | | | |
| | | | |
General Information
1 Machine and Workpiece Coordinate Systems
Figure 1 shows the Machine Coordinate System (blue), the Un-rotated “Part” Coordinate System (yellow), and the Workpiece Coordinate System (red).
The Machine Coordinate System is fixed to the machine frame and does not move when the machine axes move. It is located at the spindle nose center when all machine axes are at their zero machine positions.
The Workpiece Coordinate System is fixed to the part loaded on the C-axis table. This coordinate system is typically set in the user’s CAD/CAM system or on the part drawing used for programming the tool paths. The Workpiece Coordinate System moves and rotates when the machine axes move since it is fixed to the physical workpiece loaded on the table.
The Un-rotated “Part” Coordinate System is located at the Workpiece Coordinate System when all machine axes are set to their Part Setup locations. This coordinate system moves with the machine’s linear axes but does not rotate with the rotary axes. It is generally used only by NC Post Processors that do not use Tool Center Point Management.
[pic]
Figure 1 Coordinate Systems
2 5-axis Part setup
Figure 2 shows the values used to setup a 5-axis part on the machine. The Workpiece Coordinate System is shown in red and is fixed to the part that is being cut. The values in the Part Setup Screen (Figure 3) are described below.
Z Table Offset = the directional distance from the C-axis table face to the Workpiece Coordinate System XY-plane. It is a positive number for the setup shown in the figure.
Offset Z = the directional distance from the Z-calibration point on the machine used to calibrate the tools to the Workpiece Coordinate System XY-Plane. It is a positive number for the setup shown in the figure.
Z Calibration = tool calibration height. In the tool setup screen this number is positive but in the NC Tool Offsets table it is negative.
Notes:
• When measuring these values, ensure that the B-axis is at Zero degrees.
• For conversational programs, the B-axis Part Setup Offset must be Zero Degrees
[pic]
Figure 2 5-Axis Part and Tool Setup
[pic]
Figure 3 Part Setup Screen
3 3-axis part setup
For 3-axis operation of the SR machine, the setup procedure is identical to any Hurco 3-axis machine. Calibrate tools to the calibration plane and use the Offset Z field to indicate the Workpiece XY plane relative to the calibration plane.
4 Rotary direction convention
The VMX 42 SR machine follows the ANSI/EIA Standard RS-267-B. This standard states that the user programs the tool moving about the workpiece without regard for which axes of the machine move the spindle or the table. According to the standard, a positive move of +100mm in X, the machine control will move the machine table -100mm in the X-axis relative to the fixed machine coordinate system. Similarly, a positive C-axis command in a program will result in a C-axis rotation that is clockwise when viewing along the negative Z-axis direction (along the spindle pointing towards the table) of the machine coordinate system. This move corresponds to a negative rotation of the C-axis relative to the machine coordinate system, which results in a positive rotation of the cutting tool about the Workpiece Coordinate System Z-axis. Figure 4 shows the machine axes motion for a positive axis input.
Since the B-axis is attached to the spindle, a positive B-axis command will result in a clockwise rotation of the machine B-axis when viewed along the positive Y-axis direction of the Machine Coordinate System. This move corresponds to a positive rotation of the B-axis relative to the Machine Coordinate System, which results in a positive rotation of the cutting tool about the Workpiece Coordinate System Y-axis as shown in Figure 4.
[pic]
Figure 4 Rotational Axes Rotation Direction Convention
5 Tool Change Sequence
For any tool change, whether it is during program run (M06) or a manual tool change, the CNC will perform the following operations automatically in the specified order:
1. Retract along the current tool vector to machine limits.
2. Retract to machine Z-axis limit
3. Move X- and Y-axes to tool change position. The tool change position is specified in the Integrator Support Screens.
4. Rotate B-axis to zero degrees (spindle vertical).
5. Move Z-axis to tool change height.
6. Perform tool change.
6 M31 rotary encoder reset
The M31 command will reset the rotary axis encoder position (C-axis for the VMX 42 SR) if it has wound up or down multiple revolutions to lie between –180 to 180 degrees. If M31 is executed during contouring while running a program, the move prior to the M31 call will come to an exact stop before M31 is executed.
[pic]
NC Program Syntax
1 Transform plane – Vector Input
NC Transform Plane does not execute a rotary move when it is called. It defines a new position and orientation for a Transform Plane Coordinate System. The XYZ location of the Transform Plane is defined with respect to the Workpiece Coordinate System. It uses the X- and Y-direction vectors to define the orientation of the Transform Plane Coordinate system with respect to the Workpiece Coordinate System (vectors are discussed in subsection 3.7). The operator can use any tool orientation in an NC Transform Plane (i.e. the Tool Axis does not have to lie along the Z-axis of the Transform Plane shown in Figure 5).
[pic]
Figure 5 NC Transform Plane
Syntax
G68.2 X_Y_Z_ I_J_K_U_V_W_
G68.2 specifies the {XYZ} location of the Transform Plane with respect to the Workpiece Coordinate System. {IJK} tokens specify the Transform Plane’s X-direction vector with respect to the Workpiece Coordinate System, where the I component is the along the Workpiece X-direction, the J component is along the Workpiece Y-direction and the K component is along the Workpiece Z-direction. Similarly, {UVW} tokens specify the Y-direction of the Transform Plane with respect to the Workpiece Coordinate System.
G69 cancels NC Transform Plane.
Notes
• The CNC will align the Transform Plane to the specified IJK X-direction exactly. If the Y-direction is not exactly perpendicular to the X-direction, the control will automatically recomputed the Y-direction to be perpendicular to the X-direction. The recomputed Y-direction will lie in the plane containing the IJK and UVW direction vectors.
• All subsequent tool positions (XYZ positions, IJK tool vectors, and UVW surface normal vectors) are specified with respect to the Transform Plane except part rotary angles (i.e. B- and C-angles).
• Rotary moves are permitted while NC Transform Plane is active.
• The NC Transform Plane block is not a motion block; it does not execute motion.
• NC Transform Planes can be stacked.
2 Transform plane – Angle Input
Similar to the Vector Input NC Transform Plane, the Angle Input NC Transform Plane also does not execute a rotary move when it is called. It defines a new position and orientation for a Transform Plane Coordinate System. The XYZ location and ABC rotations are defined with respect to the Workpiece Coordinate System. The operator can use any tool orientation in an NC Transform Plane (i.e. the Tool Axis does not have to lie along the Z-axis of the Transform Plane shown in Figure 5).
1 Local vs. Global Rotations for Transform Plane
G68.2 specifies global rotations for the A-, B-, and C-angle in the NC Transform Plane. The rotation sequence will be in the order of A, followed by B, followed by C, where all rotations are about the X-, Y-, Z- axes of the fixed Un-rotated Part Coordinate System (Figure 6).
G68.3 specifies local rotations for the A-, B-, and C-angles in the transform plane. The rotation sequence will be in the order of A, followed by B, followed by C, where all rotations are about the rotated X-, Y-, Z- axes of the rotating Transform Plane Coordinate System. A rotation of the A-angle would rotate about the X-axis. Then a rotation of the B-angle would rotate about the Y-axis of the rotating Transform Plane Coordinate System that has been rotated by the A angle. Then a rotation of the C-angle would rotate about the Z-axis of the rotating Transform Plane Coordinate System that has been rotated by the A and B-angle rotations. This is demonstrated in Figure 6.
Syntax
G68.{2,3} X_Y_Z_ A_B_C_
G68.2 rotations sequence of A, B, C about fixed machine reference frame
G68.3 rotation sequence of A, B, C about the rotating Transform Plane
G69 cancels NC Transform Plane.
[pic]
Figure 6 G68.2 Global vs. G68.3 Local Transform Plane
Notes
• All subsequent tool positions (XYZ positions, IJK tool vectors, and UVW surface normal vectors) are specified with respect to the Transform Plane except machine rotary angles (i.e. B- and C-angles).
• Rotary moves are permitted while NC Transform Plane is active.
• The NC Transform Plane block is not a motion block; it does not execute motion.
• NC Transform Plane has three rotations available.
• NC Transform Planes can be stacked.
3 M126/127 shortest angular traverse
M126 activates Shortest Rotary Angle Path Traverse. The control will move the rotary axis through the shortest angular distance to the commanded position as described in Table 1. The red case is depicted in Figure 7.
Table 1 M126 Shortest Angular Traverse
|Initial position |Commanded position |Angular distance traverse |
|350( |20( |+30( |
|20( |350( |-30( |
M127 cancels Shortest Rotary Angle Path Traverse. This is the standard operating mode, which is described in Table 2. The green case is depicted in Figure 7.
Table 2 M127 Canceling Shortest Angular Traverse
|Initial position |Commanded position |Angular distance traverse |
|350( |20( |-330( |
|20( |350( |+330( |
[pic]
Figure 7 M126 red, M127 Green cases
4 M200 Tilt axis preference
To improve the work volume when the spindle is horizontal, the C-axis table has been located at the corner of the machine’s base table. Although this configuration provides a large work volume for negative B-axis angles, it restricts the work volume for positive B-axis angles. Since parts that require positive B-axis angles can be cut using a negative B-axis angle with a rotation of 180 degrees of the C-axis table, the configuration does not impose limitations on the parts that the user can cut.
Since positive B-axis angles have a restricted work volume, for 3+2-axis machining, the user may request that the post processor set the B-axis limits to –90 to 0 degrees to prevent using positive B-axis angles.
M200 can be used to select the Tilt Axis Preference direction for simultaneous 5-axis contouring in an NC program. A positive Tilt Axis Preference will keep the B-axis between 0 to +90 degrees. A negative Tilt Axis Preference will keep the B-axis between -90 to 0 degrees. A neutral Tilt Axis Preference specifies no preference and the program will execute with the shortest angular traverse if activated. A Neutral, Positive, and Negative preference is specified using P0, P1, or P2 parameter with the M200 command respectively.
The Tilt Axis Preference is only applied in M128 mode and when Tool Bottom Centre with Tool Vector interpolation mode is active (G43.4 {Q0}, described in Subsection 3.9). The machine will then force the B-axis to remain in the Tilt Axis Preference region specified.
The default for NC programs is P2 (negative).
Syntax:
M200 P[0,1,2]
P0 = None (turns tilt axis preference off)
P1 = Positive, B-axis between [0(, +90(]
P2 = Negative, B-axis between [-90(, 0(]
Motion during 5-axis contouring with Tilt Axis Preference:
If the B-axis is requested to move to the opposite side of the Tilt Axis Preference, the CNC will interpolate the tool tip and tool vector up to the machine singularity point (B-axis at 0 degrees), then the machine will rotate about the singularity point (i.e. the CNC will rotate the C-axis and interpolate the X- and Y-axes while keeping the tool tip at a constant location relative to the workpiece), followed by interpolating the B-axis and tool tip to their final positions with the B-axis on the Tilt Axis Preference Side.
5 M128 TCPM
The Tool Centre Point Management (TCPM) feature allows the user to program 5-axis tool positions in the Workpiece Coordinate System independent of the part setup location in the machine.
M128 activates TCPM and M129 deactivates TCPM.
Notes:
• Only G00 and G01 moves and NC canned cycles are supported in M128 mode.
• Both G94 (UPM) and G93 (Inverse Time) modes are supported.
• The CNC will not automatically activate G43.4{Q[0,1]} 5-axis linear interpolation (Subsection 3.9) when M128 TCPM mode is activated. The user must explicitly call G43.4{Q[0,1]} to activate the interpolation mode.
Input Options for M128 Mode
The following three input modes are available with M128 active and are discussed in greater detail in Subsections 3.6, 3.7, and 3.8.
1. Tool tip (X_ Y_ Z_) and axes angle input (B_ C_).
2. Tool tip (X_ Y_ Z_) and tool vector (I_ J_ K_).
3. Surface Contact Point (X_ Y_ Z_) and Tool Vector (I_ J_ K_) and Surface Normal Vector at the Surface Contact Point (U_ V_ W_).
6 Axes Angle Input
The user can specify the tool tip with respect to the Workpiece Coordinate System and the rotary and tilt axes angles relative to the Part Setup offsets:
Syntax:
G[00, 01] X_ Y_ Z_B_ C_ [F_]
Where:
{X_ Y_ Z_} is the bottom centre point of the tool
{B_ C_ } are rotary and tilt angles relative to the Part Setup. Angles are modal
F_ is optional unless it is a G01 move in inverse time mode (G93)
7 Tool Vector Input
1 What is a Vector?
A Vector is a directional line in 3D space that is defined using values for the X, Y, and Z direction components. Since Vectors describe a direction, their base is always at the coordinate system origin from which they point outward. Figure 8 a plot of a Vector with its I, J, K components that correspond to the X, Y, Z directions.
[pic]
Figure 8 Example of a Vector
A Tool Vector is simply the Vector that describes the orientation of the tool axis. The Tool Vector describes the direction from the tool tip pointing up through the spindle and away from the workpiece. If the NC program contains Tool Vectors in the tool positions, the CNC will compute the appropriate Rotary and Tilt axes (B- and C-axes) positions. The Tool Tip location in the part program specifies where on the workpiece that the tool should be positioned. The CNC computes the X, Y, Z machine axes positions to move the rotated tool tip to the specified point on the rotated workpiece. The Tool Tip and Tool Vector are specified with the following syntax:
Syntax
G[00, 01] X_ Y_ Z_I_ J_ K_ [F_]
Where:
{X_ Y_ Z_} is the bottom centre point of the tool. XYZ are modal.
{I_ J_ K_} is the tool vector. IJK are non-modal.
F_ is optional unless it is a G01 move in inverse time mode (G93)
Notes:
• This feature is only available if M128 TCPM mode is active.
• The Tool Vector can be specified with up to 6 decimal places. It is highly recommended that the full precision be used. The field values will normally lie in the range of [-1.000 000 to +1.000 000]. If the magnitude of the vector does not equal 1, the vector will be automatically normalized by the CNC.
• Since Vectors specify direction, they are non-dimensional. {I, J, K} Vector components should not be multiplied by unit conversion factors when converting a program from Inch to metric or vice-versa.
• The Tool Tip and the Tool Vector are specified with respect to the Workpiece Coordinate System defined in the CAM software for the part program. The CNC will automatically compute the machine axes positions using the tool length and part setup information.
• The CNC will not automatically activate G43.4{Q[0,1]} 5-axis linear interpolation (Subsection 3.9) when Tool Vector input is used. The user must explicitly call G43.4{Q[0,1]} to activate the interpolation mode.
2 Activating and Cancelling Tool Vector Input Mode
Tool Vector Input Mode activates automatically when a tool vector is given in a G00 or G01 block. When Tool Vector Input Mode is active, the Tool Vector is non-modal and must be given for each G00 and G01 block.
Tool Vector Input Mode is cancelled by the four commands listed below. When the Tool Vector Input Mode is cancelled, the CNC will hold the current rotary orientations until new orientations are programmed either by a new Tool Vector or new rotary axes positions.
1. M141 (Tool Vector Input Mode Off). This command explicitly cancels Tool Vector Input Mode.
2. M129 (Cancel Workpiece Coordinate System) command.
3. G69 (Cancel rotation or NC Transform Plane), but only if all Transform Planes have been cancelled. If more than one Transform Plane has been stacked, all Transform Planes must be cancelled before Tool Vector Input Mode will be automatically cancelled.
4. G00 or G01 block with a rotary axis angle.
8 3D Tool Geometry Compensation
This function will allow the user to specify the Surface Contact Point, the Surface Normal Vector, and the Tool Vector. The CNC will compute the tool position automatically for ball nose, flat end, and bull nose (corner radius) end mills. The tool will be positioned to tangentially touch the specified Surface Contact Point.
The Surface Contact Point, Surface Normal Vector, and Tool Vector are specified with respect to the Workpiece Coordinate System defined in the CAD/CAM software or part drawing. The CNC will automatically compute the machine axes coordinates using the tool dimensions and Part Setup information.
Syntax
G[00, 01] X_ Y_ Z_ I_ J_ K_ U_ V_ W_ [F_]
Where:
{X, Y, Z} is the part’s surface contact point (modal),
{U, V, W} is the surface normal vector of the part contact point (non-modal),
{I, J, K} is the tool axis vector (non-modal),
F_ is optional unless it is a G01 move in inverse time mode (G93),
where all coordinates are specified in the Workpiece Coordinate System.
Notes:
• Only the XYZ and F parameters are modal. IJK and UVW are non-modal.
• The Tool Vector and Surface Normal Vector can be specified with up to 6 decimal places. It is highly recommended that the full precision be used. The field values will normally lie in the range of [-1.000 000 to +1.000 000]. If the magnitude of the Vector does not equal 1, the vector will be automatically normalized by the CNC.
• Since Vectors specify direction, they are non-dimensional. {I, J, K} and {U, V, W} Vector components should not be multiplied by unit conversion factors when converting a program from Inch to metric or vice-versa.
• G41.2 activates 3D Tool Geometry Compensation Mode.
• G40 cancels 3D Tool Geometry Compensation Mode.
• TCPM (M128) must be active when using 3D Tool Geometry Compensation (G41.2).
• Although 3D Tool Geometry Compensation can position ball, flat, and bull nose endmills interchangeably, there is no guarantee that the selected tool dimensions and geometry will not cause gouging of the part. It is the responsibility of the operator to ensure that the tool path is gouge-free for the selected tool.
• The CNC will not automatically activate G43.4{Q[0,1]} 5-axis linear interpolation (Subsection 3.9) when 3D Tool Geometry Compensation is activated. The user must explicitly call G43.4{Q[0,1]} to activate the interpolation mode.
Infinite Solution Case
For flat and corner radius endmills, when the Tool Vector and Surface Normal Vector point in the same direction there are infinite solutions for the tool position. Under this condition, any point on the bottom face of the tool can touch the Surface Contact Point as shown in #1 and #2 in Figure 9. For this condition, the CNC will place the bottom center of the tool on the surface contact point, shown as #3 in Figure 9.
[pic]
Figure 9 3D Tool Geometry Compensation infinite solution case
1 Tool Geometry Specification
3D tool geometry compensation requires the following tool dimension information to compute tool positions:
1. Radius
2. Corner radius
G41.2 D_ R_ specifies the Tool Radius D_ code and the Corner Radius R_ code. The values in D_ and R_ are indexes for the NC Tool Radius Offset Table and NC Tool Corner Radius Offset Table respectively.
Notes:
• The Tool Radius and Corner Radius offsets can be cancelled when 3D Tool Geometry Compensation Mode is cancelled using G40.
• The tool Z-calibration can be specified using G43 H_ where H_ references the Tool Calibration register number or it can be specified using the Zero Calibration value in the Tool Setup. The Tool Length is computed based on the Z-Calibration, Offset Z, and Z Table Offset in the Part Setup screen.
• G41.2 will not cause movement. The tool geometry is compensated in the next commanded move.
9 G43.4 5-axis linear interpolation
The CNC can interpolate the Tool Tip relative to the Workpiece Coordinate System for 5-axis machining. The CNC offers two modes for rotary interpolation:
1. Linearly interpolate the tool vector with respect to the Workpiece Coordinate System between tool positions (Figure 11).
2. Linearly interpolate the rotary angles between tool positions.
[pic]
Figure 11 G43.4 Q0 Tool Tip and Tool Vector linear interpolation
Important Notes
1. It is extremely important to have a good start point that is relatively close to the C-axis centerline location immediately before activating G43.4 5-axis linear interpolation. Due to the M200 Tilt Axis Preference, the machine may need to rotate the part up to 180 degrees about the machine singularity point when moving to the contouring start point and tool orientation. If the tool start point is too far away from the C-axis centerline, an axis out of limits error will be thrown.
2. Although G43.4 Q0 will interpolate the Tool Tip and Tool Vector relative to the Workpiece Coordinate System, the CAM software must generate properly tolerance tool paths to machine smooth surfaces. Even with G43.4 the surface finish is still highly dependent on the CAM software to generate enough tool positions to properly break up rotary transitions and tolerance the Tool Tip linearization of the surfaces being cut. The concept is similar to using G01 moves to cut 3D surfaces in 3-axis machining but even more critical since the Tool Vector may change orientation.
3. M129 (subsection 3.5) will automatically turn G43.4 off. G69 will turn G43.4 off if it is cancelling the last stacked Transform Plane.
Syntax
G43.4 {Q[0,1]} will turn 5-axis workpiece-relative linear interpolation on. If Q parameter is not specified, the CNC will automatically select Q=0 (linear interpolation of Tool Vector and Tool Tip) when Tool Vector input is used (subsection 3.7) and Q=1 (linear interpolate rotary angles and Tool Tip) when rotary angle input is used (subsection 3.6).
Otherwise, when the user specifies Q=0 the CNC will linearly interpolate the Tool Vector and Tool Tip in a plane between NC points (Figure 11) regardless of the input type. If the user specifies Q=1 the CNC will linearly interpolate the Tool Tip between tool positions with respect to the Workpiece Coordinate System and the rotary angles in the Machine Coordinate System regardless of the input type.
10 M140 tool vector retract
M140 command allows the operator to move the tool along the current Tool Vector for a specified distance or to retract to the machine limits.
Syntax
M140 [L_] [F_]
Notes:
• L_ is the incremental distance the tool will move from its current position along the current Tool Vector direction. A positive value retracts the tool away from the workpiece as shown in Figure 12. A negative value plunges the tool towards the workpiece. Normally a positive value will be programmed, which will move the tool away from the workpiece in most situations. When the L parameter is specified, the CNC will NOT clip the move to machine limits and the CNC may throw an out of machine limits alarm if necessary.
• When M140 is used without the L_ parameter, the tool will retract along the positive direction of the current Tool Vector to the machine limits (i.e. move the tool tip away from the workpiece). The CNC will clip the move to the machine limits and will not throw an out of limits alarm.
• There are 4 possible cases for the F_ token:
1. If in G94 mode (feedrate in UPM, units per minute) and F_ is provided, the CNC will retract at the specified feedrate.
2. If in G94 mode (UPM) but not in Rapid traverse, the retract will use the current modal feedrate.
3. If G00 is called immediately before M140 or during the same block, the CNC will retract at rapid traverse rate.
4. If in G93 Inverse Time mode the CNC will thrown an alarm.
• M140 is non-modal and only active for the current block.
[pic]
Figure 12 Positive tool vector retract direction along arrow
11 SR42 Machine Specifications
Axes Limits:
X 1067mm, attached to table
Y 610mm, attached to table
Z 610mm, attached to spindle
B +/-90 degrees, attached to spindle
C Full 360 degrees rotation, attached to table
Maximum programmable contouring feedrate is 15240 mm/min
Maximum rapid traverse feedrate is 35000 mm/min
12 Inverse Time
Hurco’s inverse time field width has been expanded to 9 digits [######.###]. However, all interpolation modes and tool path inputs can use G94 unit-per-minute feedrate.
-----------------------
Surface Normal Vector
Tool Vector
Surface Contact Point
Figure 8 Vector definition for 3D tool geometry compensation
Figure 10 Tool Geometry
Tool Length
(spindle zero to tip)
Corner Radius
Radius
................
................
In order to avoid copyright disputes, this page is only a partial summary.
To fulfill the demand for quickly locating and searching documents.
It is intelligent file search solution for home and business.