Offset Specification with Cutter Compensation
Whether it’s based on the cutter’s radius or diameter, compensation means a range of cutter sizes can be used, and it allows for sizing adjustments.
Machining center cutter compensation allows a CNC programmer to ignore the size of milling cutters used for side milling operations as they create CNC programs. The programmer will specify a programmed path—either with center line coordinates based on a planned cutter size or with work surface coordinates—and the machine operator will specify a compensation value in a cutter compensation offset. When the program is run, the machining center will modify the programmed path by the amount of the offset.
This feature provides several advantages, including:
• A range of cutter sizes can be used.
• Trial machining can be done for surfaces that have small tolerances.
• Sizing adjustments can be made as the milling cutter wears.
Although programming remains remarkably similar among CNCs, over the years, control manufacturers have varied how the cutter compensation offset value is specified. With some CNC controls, the offset value is specified as the cutter’s radius. With others, the offset value is specified as the cutter’s diameter. This can be a source of great confusion among operators if a company has several machines and both offsetting methods must be used.
If a given machine requires offset specification in diameter and if work surface coordinates are specified for the programmed path, the operator will initially enter the milling cutter’s diameter into the cutter compensation offset. Many CNC users prefer this method, since it is very easy to determine the milling cutter’s diameter (by measuring it).
If a machine requires specification of the cutter’s radius, the operator must first perform a calculation, dividing the cutter’s diameter by two, prior to entering the initial offset value.
Admittedly, the initial offset value is relatively easy to determine regardless of which method is used. But with surfaces having small tolerances, it is likely that trial machining must be performed on the first workpiece, and that sizing adjustments will be required during the milling cutter’s life. Offset adjustments made for trial machining and sizing adjustments are also affected by which offset specification method is used.
Say, for instance, that a programmer has programmed work surface coordinates and an operator will be trial machining a critical surface with a 1.0-inch end mill. Let’s first address a machine that requires the cutter compensation offsets to be specified in diameter. If the operator wants to leave 0.01 inch in additional stock on the surface, he must double the trial machining stock amount and enter a value of 1.02 inch in the offset register. When the milling cutter trial machines the surface, it will leave about 0.01 inch of stock.
If, on the other hand, the operator is performing the same milling operation on a machine that requires radius specification, he will increase the cutter’s radial value by 0.01 inch, the exact amount of stock to be left, and set the offset register to 0.51 inch.
The same applies when making sizing adjustments. Operators running machines requiring diameter offset entry will be doubling values, while operators running machines requiring radial offset entry will not. Again, this can make it difficult for operators who move from one machine to another.
Older CNC controls typically allow only one of the two methods, forcing operators to adapt to the control manufacturer’s required method. It is important to know, however, that most current-model controls let you specify the preferred method with a parameter setting. This, of course, means that you may be able to standardize on one offsetting method, possibly on a company-wide basis. The parameter number should be specified in the programming manual during the explanation of cutter compensation.
Which method is best?
This may be a difficult question to answer. Your people will likely argue for whichever method they have learned and are comfortable with.
My recommendation would be based on your tolerance bands. With large tolerances, there will be no need for trial machining, since the initial offset setting will be good enough to machine the surface within its tolerance band. Additionally, the milling cutter will not wear enough during a production run to require sizing adjustments. For this scenario, since it is easier to determine the cutter’s diameter than its radius, I recommend setting the parameter in such a way that cutter compensation offsets are specified in diameter.
On the other hand, if the tolerances are small enough to require trial machining for the first workpiece and sizing adjustments during the milling cutter’s life, I think it is easier to calculate adjustment values when the machine requires radial offset entry. (There won’t be a need to double the calculated adjustment amount.) In this case, I recommend setting the control’s parameter so that cutter compensation offsets are specified in radius.
They offer benefits that many CNC users overlook.
A company’s CNC needs can vary depending on what it produces.
Which command is better to get your machine axes to the reference position?