5.pdf

Probing Cycles for Conversational Programming

P/N 70000570

Introduction

This document describes operation and an overview of the tool and part

probe canned cycles in conversational format. Probing is an option in

3000M and 5000M CNC products, and is standard in 6000M. The cycles

provided perform the most common tool and part probing functions. If

Probing has been added post-sale, besides Setup Utility changes, there

may be Integral Programmable Intelligence (IPI) program modifications

required.

The tool probe cycles are only supported on machines with automatic

spindle forward/reverse and spindle speed, and homing with a permanent

X, Y, and Z machine position. The method described assumes the use of

negative tool-length offsets. In this method, the Tool-Length Offset (TLO)

in the length column for each tool represents the distance from the tool tip

at machine home to top of work piece and is a negative number. This

method does not require the use of any Z work coordinate offset to be

active. This procedure will find the effective tool diameter by turning the

spindle on in reverse and touching two sides of the probe stylus, then

storing the tool’s diameter in the tool’s diameter offset table.

The part probing cycles are designed to assist in part setup. Using these

cycles, one or more features (edges) of a part can be measured. Using

the data obtained with these measurements, calculations are made that

can be used to set a given fixture offset. It is also possible to find the

orientation angle of a part so as to not always have to align the part

exactly.

Tool and part probing do not allow rotation, scaling, and mirroring. If they

are active before calling the canned cycles, they will be deactivated.

Plane will be set to XY when these cycles are complete.

Tool Probe Cycles

Before using your tool probe and tool probe cycles, you must setup the

probe following the manufacture’s specifications.

The tool probe will update the tool registers only. If you are going to use

the tool being measured after the probing cycle, you must recall that tool

for the new offsets to be active.

This section covers the following topics:

Tool Probe cycle designations

System Variable settings

Detailed description of all tool probe cycles

15-August-03

Probing Cycles for Conversational Programming

P/N 70000570

Tool Probe Cycle Designations

The following summarizes the cycles available:

Probe Calibration

(CalibTlPrb)

Tool Probe Calibration Cycle

This is used to set the Z datum for length preset, the effective

probe stylus diameter for setting tool diameter registers, and

establishes the center of the probe stylus.

NOTE: Calibration must be done at least once before using the

tool probe. Once the probe has been calibrated,

calibration does not need to be done unless the probe

is moved or a new part is being setup.

Length and Diameter

(LenDiamMea)

Tool Length and Diameter Offset Preset

Updates length and diameter tool registers.

NOTE: If the tool has a hole on the bottom so that the probe

would fall between the tool teeth, do not use this cycle.

Damage to the probe could result. In this case, use

Length Special for manual length preset or Diameter

Special for manual diameter preset.

Length Special

(LenSpecMea)

Manual Tool-Length Offset Preset

Updates tool-length register. To be used for large face mill style

tools or shell mill tools that has a hole in the center of the

bottom of the tool.

Diameter Special

(DiaSpecMea)

Manual Tool Diameter Preset

Updates tool diameter register for irregular shaped tools or tools

with a hole in the center of the bottom.

Break and Wear

(BrkWearDet)

Tool Breakage, Length and Diameter Wear Detection

Breakage

Checks the tool and gives an alarm if not within tolerance.

Length and Diameter Wear – Check the Length and/or Diameter

and updates the Length and/or Diameter wear registers up to a

user-defined limit. Once the user-defined limit has been

reached, the cycle will give an alarm.

System Variable Settings

Before you set the parameters for the tool probe you must:

Know the diameter of the calibration standard.

Know that the calibration standard is a standard that is specifically

designed for calibrating the probe. The DiamOfStd parameter is the

diameter of the part of the calibration standard that comes in contact

with the probe stylus during calibration and should be an exact

measurement.

15-August-03

Probing Cycles for Conversational Programming

P/N 70000570

Ensure when entering the values in the parameters that you are in

the same units (inch/metric) as when you are running the tool preset

canned cycle. Set the units in parameters to the units in which you

are going to run the cycles. See “Units” in 3000M Setup Utility. If

you run programs in Inch, then the unit parameter must be set to

Inch, and all probe system variables must be entered in Inch. If you

want to switch to millimeter programs and use these tool-preset

cycles, you must go back and change the unit parameter to metric

then reset the values in these variables and recalibrate the probe

stylus.

See the 3000M CNC Setup Utility Manual, P/N 70000499, “Section 2 -

Builder Setup ” for a detailed description of the setup parameters.

NOTE: 3000M contains a “Probing” section within “Section 2 - Builder

Setup” where the probing parameters are described.

1. Set 3-D probe, this should be set to Corded, Cordless, or Cordless

SG for a strain gauge type probe.

2. Set Nominal probe stylus diameter , the overall nominal probe stylus

diameter. For example, to 0.5” (12.7 mm) for the Renishaw probe, or

for the Heidenhain probe use 1.575” (40 mm). This is dependent on

the probe style and specifications (refer to your probe documentation).

3. Set Maximum stroke from home for first pick , represents the

distance from machine Z home with the shortest tool or the spindle

face to just below the probe stylus top as the maximum stroke for the

initial probe pick.

4. Set RPM for calibration and tool measurement , the spindle spin

RPM for tool touch. (For example, set to 800.)

5. Set Probe orientation , the proper probe orientation. For example, if

set to –1, the probe should be installed on the right side of the table

pointing toward the left in the –X direction. See Table 1 .

Table 1, Probe Orientation Settings

Direction

1 Probe is pointing to the right as you are facing

the machine in +X direction

-1 Probe is pointing to the left of the machine in the

-X direction.

2 Probe is pointing away from you, toward the

back of the machine in the +Y direction

-2 Probe is pointing toward you, toward the front of

the machine in the -Y direction

6. Set Z first pick, FAST feedrate , the Z fast feedrate. [For example,

set to 50.0 inches per minute (in/min) (2540 mm per minute

(mm/min).]

15-August-03

Probe Orientation

Setting

Probing Cycles for Conversational Programming

P/N 70000570

Warning: When using Length and Diameter , the tool will travel

down beyond the top of the probe after the probe is tripped. For this

reason, make sure that the fast feedrate is not so high as to cause the

tool to travel past the probe travel causing damage to the probe. The

maximum feedrate that can be used is specific to the machine and

may need to be set much lower to prevent damage to the probe.

7. Set the Z first pick, Z first pick, MEDIUM feedrate , the Z medium

feedrate. [For example, set to 5.0 in/min (127 mm/min).]

8. Set Z first pick, SLOW feedrate , the Z slow feedrate. [For example,

set to 1.0 in/min (25.4 mm/min).]

9. Set Z retract amount . [For example, set to 0.2” (5.08 mm).]

10. Set XY retract amount . [For example, set to 0.2” (5.08 mm).]

11. Set Z rapid to start position from home . Install the longest tool in

the spindle and bring the Z-axis to machine home. With a tape

measure, measure the distance from the tool tip to within 0.5” (12.7

mm) above the top of the probe stylus and enter that number into

Z start position . When using Length and Diameter , this will cause

the tool to rapid to this position in the Z-axis before starting the initial

probe touch in the Z-axis. This will save time especially if the Z-feed

must be set relatively slow to prevent probe over travel after the probe

has been tripped.

12. Set Diameter of tool probe gauge . The default gauge diameter of

the tool calibration standard. Diameter of tool probe gauge can be

overwritten by the DiamOfStd address word in the Probe Calibration

cycle. Diameter of tool probe gauge is used in the Probe

Calibration calibration only. [For example, set to 2.0” (50.8 mm).]

For tool probing or tool length presetting, Tool-Length Offset

(TLO) is the distance from machine home to top of work piece or

wherever you set your part “ Z ” zero.

Before starting to set your tools, you must calibrate the probe.

Once the probe has been calibrated, calibration does not have to

be done again unless you remove the probe or replace the stylus.

Recalibration may also be required if the Z location of the top of

the part changes, and is not compensated for by a Z work offset.

Description of Tool Probe Cycles

This section contains detailed descriptions of the tool probe cycles:

• Tool Probe Calibration Cycle (CalibTlPrb)

• Tool Length and Diameter Offset Preset (LenDiamMea)

• Manual Tool Length Measure for Special Tools (LenSpecMea)

• Manual Tool Diameter Measure for Special Tools (DiaSpecMea)

• Tool Breakage, Length, and Diameter Wear Detection (BrkWearDet)

15-August-03

Probing Cycles for Conversational Programming

P/N 70000570

Tool Probe Calibration Cycle (CalibTlPrb)

Format: CalibTlPrb DiamOfStd(n) DistDown(n)

This cycle is used to calibrate the probe. This is used to set the Z datum

for length preset, establishing the center of the probe stylus, and the

effective probe stylus diameter for setting tool diameter registers. Refer

to Table 2 .

Table 2, CalibTlPrb Entry Fields

Entry Fields

Description

DiamOfStd

The diameter of the part of the calibration standard that

comes in contact with the probe stylus during calibration.

This should be an exact measurement. (Optional override

for Diameter of tool probe gauge )

DistDown

The distance to go down along the side of the probe stylus

with the probe calibration standard when touching the side

of the stylus for diameter calibration. The maximum

DistDown value is 0.55” (13.97 mm). Without any

DistDown value, the cycle will bring the calibration standard

down past the top of the probe stylus the default 0.1”

(2.54mm). If you put a number higher than 0.55” (13.97

mm), the control displays an error. (Optional) [Default: .1”]

To calibrate the tool probe:

1. Jog the calibration standard (the calibration standard should be in the

spindle) to the top of your work piece, and set its tool-length offset to

the top of the work piece or to wherever you would like your Z zero to

be. To calibrate the tool number:

a) Jog the tip of the calibration standard to the proper spot

b) Press the Calib Z function key.

2. Manually jog the calibration standard over the probe stylus center and

less then 0.2” (5.08 mm) above the probe stylus. It should be no

more then 0.062” (2.0 mm) from the center of the stylus.

3. From the MDI mode, pick

F5 ( Mill ) → F10 ( Probe ) → F1 ( ToolPro ) → Probe Calibration

For example: CalibTlPrb exit by pressing F9 twice and F10 to exit.

4. The Z-axis will initially go down and touch the top of the probe stylus

at the feedrate specified in Z first pick, MEDIUM feedrate . Then

retouch at the slow feedrate, Z first pick, SLOW feedrate ,

establishing the zero probe stylus top.

5. Then incrementally rapid up whatever value that is in Z retract

amount .

15-August-03

Plik z chomika:

Inne pliki z tego folderu:

Inne foldery tego chomika: