Key concept number four: You must Understand the forms of compensation
All types of CNC machine tools require some form/s of compensation. Though
applied for different reasons on different machine types, all forms of
compensation allow the CNC user to allow for unpredictable conditions related
to tooling as the program is developed. Before discussing how compensation
applies to CNC usage, let's look at compensation in general terms.
Compensation is used in many facets of everyday life. The airplane pilot
must compensate for wind velocity and direction as a heading is set. The race
car driver must compensate for weather and track conditions as a turn is
negotiated. A bowler must compensate for the spin of the bowling ball as the
ball rolls down the alley. A marksman firing a rifle must compensate for the
distance to the target. The marksman analogy is amazingly similar to what
happens with many forms of compensation on CNC equipment, so let's discuss it
further.
Say a marksman is standing 50 yards from a target. By one means or another,
the marksman would adjust the sight on the rifle to allow for the 50 yard
distance. The marksman would make the necessary adjustment, but until the first
shot is fired, the marksman will not know for sure whether the initial sight
adjustment was perfectly correct. Once the first shot is fired and the marksman
can see the resulting hole location, the sight may have to be fine tuned to
adjust for minor imperfections with the initial adjustment.
In similar fashion, the CNC user will be faced with several situations when
it will be impossible to predict the result of certain tooling related
problems. So one form or another of compensation will have to be used to handle
the problem. But just as the marksman may have to fine tune after the initial
shot, so may the CNC user have to fine tune the initial compensation entry.
More on how and why in a little while.
What are offsets?
All forms of compensation work with offsets. You can think of CNC offsets as
like memories on an electronic calculator. If your calculator has memories, you
know you can store a constant value into each memory for use during a
calculation. This keeps you from having to enter the number over and over again
with redundant calculations.
Like the memories of an electronic calculator, offsets in the CNC control
are storage locations into which numerical values can be placed. Just as the
value within the memory of a calculator has no meaning until referenced by its
user within a calculation, neither does the value within an offset of the CNC
control have any meaning until it is referenced by a CNC program.
From the marksman analogy, you can think of the values stored in CNC offsets
as like the amount of adjustment required on the sight of the rifle necessary
to compensate for the distance to the target. Keep in mind that the rifle only
needed adjustment for one purpose, to adjust for the distance to the target.
With most CNC machine tools, there is a need for at least one offset per tool.
Reasons for tool offsets
Offsets can be used for several purposes depending on the style of machine
tool and type of compensation being used. Here are some of the more common
applications for offsets.
To specify tool each tool's length
For machining center applications, it would be very difficult for the
programmer to predict the precise length of each tool used in the program. For
this reason, the feature tool length compensation allows the programmer to
ignore each tool's length as the program is written. At the time of setup, the
setup person measures the length of each tool and inputs the tool length value
into the corresponding offset.
To specify the radius of the cutting tool
When milling on the periphery of the cutter (contour milling), it can be
cumbersome and difficult for the programmer to program the cutter's path based
on the size of the milling cutter being used. Also, if the cutter size must
change (possibly due to re-sharpening), it would be infeasible to change the
program based on the new cutter size. For this reason, the feature cutter
radius compensation allows the programmer to ignore the cutter size as the
program is written. The setup person inputs the size of each milling cutter
into its corresponding tool offset. In similar fashion, turning centers have a
feature called tool nose radius compensation. With this feature, an offset is
used to specify the radius of the very tip of the turning or boring tool.
To assign program zero
Machining centers that have fixture offsets (also called coordinate system
shifting) allow the user to specify the position of the program zero point
within offsets, keeping the assignment of program zero separate from the
program. In similar fashion many turning centers allow the assignment of
program zero with offsets (this feature is commonly called geometry offsets).
To allow sizing on turning centers
Tool offsets are used on all turning centers to allow the operator to hold
size with tools used within their programs. This allows the operator to adjust
for imperfections with tool placement during setup. It also allows the operator
to adjust the tool's movements to allow for tool wear during each tool's life.
Organizing offsets
With some CNC controls, the organization of offsets is very obvious. Some
machining center controls, for example, automatically make the offset number
correspond to the tool station number. With this kind of machine, when tool
station number one is commanded, the control will automatically invoke offset
number one. Within offset number one, the operator can store a tool length
value as well as a tool radius value.
Unfortunately, not all controls make it this simple. In many controls, each
offset contains only one value and the offset number has no real relationship
to the tool station number. In this case, the programmer must cautiously
organize which offset/s are used with each tool.
For example, the tool length compensation offset numbers can be made the
same as tool station numbers. Cutter radius compensation offset numbers can be
made equal to the tool station number PLUS a constant value larger than the
number of tools the machine can hold. If the machine can hold 25 tools, tool
station number one could be made to use offset number one to store its length
compensation value and offset number thirty-one could be used to store its
cutter radius compensation value. With this method of offset organization, the
programmer and operator are constantly in sync.
The offset table on most turning centers incorporate at least two values per
offset. Generally speaking, the programmer will instate the offset number
corresponding to the tool station number for each tool offset used. That is,
tool number one will use (only) offset number one, tool two will use offset
two, and so on. Additionally, most turning center offset tables allow the user
to enter data related to the tool's radius (for tool nose radius compensation).
Typically the radius (R column of the offset table) and the tool type (the T
column of the offset table) can be specified within the turning center's offset
table.
Types of compensation
Now let's discuss the compensation types for the two most popular forms of
CNC machine tools, machining centers and turning centers. Keep in mind that
while the actual use of these functions vary dramatically from one machine to
the next, the basic reasoning behind each compensation type remains remarkably
similar. With an understanding of why the compensation type is required, and
with an elementary understanding of how it is applied to one specific control,
you should be able to adapt to any variations that you come across.
Tool length compensation
This machining center compensation type allows the programmer to forget
about each tool's length as the program is written. Instead of having to know
the exact length of each tool and tediously calculating Z axis positions based
on the tool's length, the programmer simply instates tool length compensation
on each tool's first Z axis approach movement to the workpiece.
At the machine during setup, the operator will input the tool length
compensation value for each tool in the corresponding offset. This, of course,
means the tool length compensation value must first be measured.
If tool length compensation is used wisely, the tool length compensation
value can be measured off line (in a tool length measurement gage) to minimize
setup time. With this method, the tool length compensation value is simply the
length of the tool.
Many CNC controls allow the length of the tool to be used as the offset
value. One popular command to instate tool length compensation is G43. Within
the G43 command, the programmer includes an H word that specifies the number of
the offset containing the tool's length value. Here is an example program that
utilizes tool length compensation with two tools. The program simply drills two
holes (one with each tool). Notice that tool length compensation is being
instated in lines N015 and N055.
Program
O0001 (Program number)
N005 T01 M06 (Place tool number one in the spindle)
N010 G54 G90 S400 M03 T02 (Select coordinate system, absolute mode, start
spindle CW at 400 RPM, get tool number two ready)
N013 G00 X1.0 Y1.0 (Rapid to first XY position)
N015 G43 H01 Z.1 M08 (Instate tool length compensation on first Z move,
turn on coolant)
N020 G01 Z-1.5 F4. (Drill hole)
N025 G00 Z.1 M09 (Rapid out of hole, turn off coolant)
As stated, this feature varies dramatically in use from one control model to
the next. You must reference your control manufacturer's programming manual to
learn more about how tool length compensation applies to your particular
machining center. Sizing with tool length compensation
In the marksman analogy, we said that the marksman would not know for sure
whether the initial sight adjustment is perfectly correct until the first shot
is fired. In similar fashion, the CNC operator will not know for certain
whether the tool length compensation value is perfectly correct until the first
workpiece is machined. Say for example, the tool length measurement was made
incorrectly. During the measurement, the operator finds the tool to be 6.5372
in long. But the actual tool length is 6.5355 in. In this case, the tool would
machine slightly shallower in Z that it is supposed to. After machining, the
minor depth change can be made by adjusting the offset, NOT THE PROGRAM.
In some cases, even if the tool length value is measured perfectly, other
problems may cause the tool not to machine to the proper depth. If, for
example, the workpiece or setup is quite weak, tool pressure may cause the
workpiece to tend to push away from the tool doing the machining.
For critical surfaces or when tool pressure is unpredictable, the operator
can even trial cut the workpiece under the influence of an offset slightly
LARGER than the measured value to ensure that some excess stock will be left.
After machining, the operator can measure the surface to determine precisely
how much offset change is necessary to machine the workpiece to size.
Cutter radius compensation
Just as tool length compensation allows the machining center programmer to
forget about the tool's length, so does cutter radius compensation allow the
programmer to forget about the cutter's radius as contours are programmed.
While it may be obvious, let us point out that cutter radius compensation is
ONLY used for milling cutters and only when milling on the periphery of the
cutter. You would NEVER consider using cutter radius compensation for a drill,
tap, reamer, or other hole machining tool.
Reasons for cutter radius compensation
Let's begin by discussing four reasons why cutter radius compensation is not
only required, but also very helpful to the CNC user.
Program coordinates are easier to calculate
Without cutter radius compensation, machining center programmers must
program the centerline path of all milling cutters. An example program using
this technique was shown during our discussion of motion types (key concept
number three). When programming centerline path, the programmer must know the
precise diameter of the milling cutter and calculate program movements based on
the tool's centerline path.
With cutter radius compensation, the programmer can program the coordinates
of the work surface, NOT the tool's centerline path. This eliminates the need
for many calculations.
Keep in mind that we are now talking about manual programming. If you have a
CAM (computer aided manufacturing) system, your CAM system can probably
generate centerline path just as easily as work surface path.
Range of cutter sizes
Say you do program centerline path for a given workpiece contour and do not
use cutter radius compensation. Say you have programmed based on a one inch
diameter tool. But when the job is to be run, you find that your company does
not have any one inch end mills. Say the closest you have is a 0.875 in cutter.
In this case, the entire cutter path would have to be changed in the program to
match the new cutter size. With cutter radius compensation, handling this
problem is as simple as changing an offset value.
Easy sizing
As with tool length compensation, the operator can use the cutter radius
compensation offset to help with sizing. If the contour is not coming out to
size (possibly due to tool pressure), an offset can be changed to allow for the
imperfection.
Roughing and finishing
This is also a manual programming related reason for using cutter radius
compensation. If contours must be rough and finish milled, cutter radius
compensation allows the programmer to used the same programmed coordinates
needed to finish mill the workpiece to rough mill the workpiece. This keeps the
programmer from having to calculate to sets of milling coordinates (one for
roughing and one for finishing). To leave stock for finishing during the rough
milling, the operator will simply make the cutter radius compensation offset
value slightly larger than the cutter's actual size. This will keep the cutter
away from the surface being milled and leave the desired finishing stock.
How to program cutter radius compensation
The usage of cutter radius compensation does vary from one control to the
next. Additionally, each control will have a set of strict rules that specify
how cutter radius compensation is instated, used, and cancelled. Here we just
show the basics of how it is programmed and give an example for how it is used
on one popular control model. You must refer to your CNC control manufacturer's
manual for more on your particular control.
Most controls use three G codes with cutter radius compensation. G41 is used
to instate a cutter left condition (climb milling with a right hand cutter).
G42 is used to instate a cutter right condition (conventional milling). G40 is
used to cancel cutter radius compensation. Additionally, many controls use a D
word to specify the offset number used with cutter radius compensation.
To determine whether to use G41 or G42, simply look in the direction the
cutter is moving during machining and ask yourself if the cutter is on the left
or right side of the surface being machined. If on the left, use G41. If on the
right, use G42. Figure 4.6 shows some examples that should help you understand
how to determine whether to use G41 or G42 to instate. Figure 4.6 - Drawings
show how to determine whether to use G41 or G42 to instate cutter radius
compensation.
Once cutter radius compensation is properly instated, it the cutter will be
kept on the left side or right side (depending on whether G41 or G42 is used to
instate) of all surfaces until the G40 command to cancel compensation.
Dimensional tool (wear) offsets
This compensation type applies only to turning centers. When setting up
tools, it is infeasible to expect the setup person to perfectly set each tool
into position. It is likely that some minor positioning problem will exist. And
even if all tools could be perfectly positioned, as any single point turning or
boring tool begins cutting, it will begin to wear. As a turning or boring tool
wears, the tool wear will affect the size of the workpiece being machined.
For these reasons, and to allow easy sizing of turned workpieces,
dimensional tool offsets are required (also called simply tool offsets). Tool
offsets are instated as part of a four digit T word. The first two digits
command the tool station number and the second two digits command the offset
number to be instated. The command T0101, for example, rotates the turret to
station number one and instates offset number one. It is wise to always make
the number of the primary offset used with a tool the same as the tool station
number.
When a tool offset is instated, the control actually shifts the entire
coordinate system by the amount of the offset. It will be as if the operator
could actually move the tool in the turret by the amount of the offset.
Each dimensional offset has two values, one for X and one for Z. The
operator will have control of what the tool does in both axes as the workpiece
is being machined. Here's an example that should help you understand how
dimensional tool offsets work. Say you have written a program to use tool
number one (with offset number one) to turn a three inch diameter. After
machining the three inch diameter, it is measured and found to be 3.005 in.
That is, the workpiece is 0.005 in oversize. In this case, the X value of
offset number one will be reduced by 0.005 in. When the program is run again,
tool number one will machine the workpiece 0.005 smaller.
How to guarantee your first workpiece comes out on size
If working on an engine lathe, manually turning a precise diameter, you
would first allow the tool to skim cut to find out exactly where the tool is
located. After skim cutting, you can determine precisely how much to turn the
crank or handle to make the tool turn the desired diameter.
In the same way, you can use dimensional tool offsets to ensure that any
tool will not violate the workpiece on its first cut. Outside diameter turning
tools, for example, could be offset slightly plus in X to ensure that some
excess stock is left. Inside diameter bored holes could be offset slightly
minus in X for the same purpose. In either case, the first time the tool is
run, the operator can rest assured that the workpiece will come out with some
excess finishing stock (it will NOT be scrapped). After machining the first
time, the surface can be measured. The operator will then adjust the
corresponding offset accordingly and re-machine with the tool This time the
surface will be machined perfectly to size. Using this technique on each tool
in the program will almost guarantee that the first workpiece will not be
scrapped.
Tool nose radius compensation
This turning center compensation type is very similar to cutter radius
compensation. In fact the same three G codes are used. G41 instates tool nose
radius compensation in a tool left condition. G42 instates with a tool right
condition. G40 cancels tool nose radius compensation. For this reason, minimize
our discussion of tool nose radius compensation to avoid repeating information.
Just as cutter radius compensation allows the programmer to program work
surface coordinates (not allowing for tool radius), so does tool nose radius
compensation.
To determine G41 or G42, simply look in the direction the tool is moving
during the cut and ask yourself which side of the workpiece the tool is on. If
the tool is on the left, use G41 (this would be the case when boring toward the
chuck). If the tool is on the right, use G42 (turning toward the chuck). Once
you determine which to use, include the proper G code in the tool's first
approach to the workpiece. Once tool nose radius compensation is instated, it
remains in effect until cancelled.
Keep in mind that the tool nose radius is quite small (usually 1/64, 1/32,
3/64, or 1/16 in), meaning the deviation from the work surface will also be
quite small. It is possible that if you are only chamfering corners to break
sharp edges, you may not need tool nose radius compensation. However, if the
surfaces being machined are critical (Morse taper, for example), you must
compensate for the radius of the tool. Also, you should only need tool nose
radius compensation when finishing. You should not use it for roughing
operations.
Other types of compensation
The compensation types shown have been for machining centers and turning
centers. But all forms of CNC equipment have some form of compensation to allow
for unpredictable situations. Here are some other brief examples.
CNC Wire EDM machines have two kinds of compensation. One, called wire
offset works in a very similar way to cutter radius compensation to keep the
wire centerline away from the work surface by the wire radius plus the overburn
amount. It is also used to help make trim (finishing) passes using the same
series of motion coordinates.
The second form of compensation for wire EDM machines is taper cutting. For
machining the clearance angle needed with dies and form tools, the programmer
can easily specify the direction of the taper (left or right) and the angle
desired. The operator fills in some offsets to tell the control the position of
the upper guide relative to the workpiece and the control does the rest.
Laser cutting machines also have a feature like cutter radius compensation
to keep the laser the radius of the laser beam away from the surface being
machined. CNC press breaks have a form of compensation to allow for bend
allowances based on the workpiece material and thickness. Generally speaking,
if the CNC user is faced with any unpredictable situations during programming,
it is likely that the CNC control manufacturer has come up with a form of
compensation to deal with the problem.
