Use these techniques to simplify dull tool replacement.
Task simplification provides at least three important benefits: it lowers the skill level required of the person performing the task, makes the task less error-prone, and almost always enables the task to be completed in less time.
The task of dull tool replacement varies substantially among machine types, but the general procedure remains essentially the same from machine to machine. For machining centers and turning centers, it goes something like this:
1. Recognize a tool that has become dull.
2. With the machine stopped, select the tool station that holds the dull tool.
3. Remove the cutting tool from the machine, if necessary.
4. Remove and index or replace the cutting portion of the tool.
5. Place the tool back into the machine, if necessary.
6. Measure and enter the offsets required for the tool, if necessary.
7. Consider the wear offset used with the tool and reset, if necessary.
8. Use trial machining techniques, if necessary, to ensure the next workpiece is machined properly.
In every step, there are techniques that can be used to simplify the overall task of replacing dull tools. The following are a few suggestions.
Help operators recognize when cutting tools get dull. Most companies expect their CNC operators to know when tools dull, but without guidance, it is unlikely that any two operators will replace dull tools at exactly the same time. With short production runs, this may not be an issue, but with longer runs, you will want to help them determine when tools are dull. At the very least, specify in the production run documentation the number of workpieces that can be run with a given tool. Better yet, program the machine to stop when tool replacements are required. This program will stop the machine after 150 workpieces are run:
(Machining program goes here)
#500 = #500 + 1
IF [#500 LT 250] GOTO 99
#500 = 0
#3000 = 100 (FINISHING TOOLS DULL)
Help operators get dull tools out of the machine. Selecting the tool station that holds the dull tool often involves executing an MDI command, because many machines don’t allow complete manual control of the turret or automatic toolchanger. You may be able to come up with a universal program that will select the tool to be removed and position the axes to a position that makes it convenient to remove it. For example, G65 P1000 T4.0 can be used with machining centers to place tool number four in the spindle and move the Y axis away from the operator, allowing more access to the spindle.
G91 G28 Z0 M19 (Move to tool-change position)
T#20 M06 (Place dull tool in spindle)
G53 Y-12.0 (Move Y axis for easier access to spindle)
M99 (End of custom macro)
Color code toolholders and hand tools. Operators must remove and replace the cutting portion of the tool, often using hand tools like hex wrenches. These tools all look alike, and you can eliminate trial-and-error by coloring the hand tools to match the toolholders with which they are used.
Help operators with offset measurements and entries. The same cutting-tool-related tasks required during initial setup must be repeated when tools get dull. For machining centers, for example, a tool length and possibly a cutter radius compensation value must be entered into the appropriate offset. Study these tasks and come up with ways to simplify them. Is it easier to measure cutting tools offline or in the machine? Could a custom macro help with tool-length measurement? Knowing tools will get dull during a production run, can duplicates be assembled and measured up front?
Help operators with trial machining. If trial machining was required during the initial setup to help size-in the first workpiece, it will probably be required when dull tools are replaced, and you can program the related commands. (Have the operator turn off the block delete switch to enable trial machining, because if this switch is on, the machine will not execute the commands.) Consider this turning center example for a finish turning tool that is place in station number two:
N180 T0202 M42
N185 G96 S450 M03
/G10 P2 U0.01 (Increase X register of offset 2 by 0.01)
/T0202 (Invoke trial machining offset)
/G00 1.875 Z0.1 M08 (Move to diameter to trial machine)
/G01 Z-0.3 F0.006 (Turn a small amount of diameter)
/X2.0 (Feed away)
/G00 X4.0 Z4.0 (Move to convenient measuring position)
/M00 (Adjust offset to machine 1.875 diameter)
N185T0202 (Re-invoke offset)
N190 G00 X2.075 Z0 M08
N195 G01 X1.05 F0.006
N200 G00 Z0.1
N210 G01 Z0
N215 G03 X1.875 Z-0.0625 R0.0625
N220 G01 Z-1.0
N230 G00 X6.0 Z5.0
While the mistakes listed here will not sound an alarm or cause a program to fail, they will cause confusion, wasted time and scrap parts.
A company’s CNC needs can vary depending on what it produces.
They offer benefits that many CNC users overlook.