Cutter radius compensation for machining centers (also called cutter diameter compensation) has at least three major benefits. It lets a manual programmer ignore cutter size when calculating coordinates for the program, it allows the setup person to choose from a range of cutter sizes, and it allows for easy trial machining and workpiece sizing during setup and the subsequent production run.
Cutter radius compensation for machining centers (also called cutter diameter compensation) has at least three major benefits. It lets a manual programmer ignore cutter size when calculating coordinates for the program, it allows the setup person to choose from a range of cutter sizes, and it allows for easy trial machining and workpiece sizing during setup and the subsequent production run. Programmers must fully understand and master this important CNC feature.
There are actually two methods of applying cutter radius compensation. First, let's describe the two methods. Then we'll make a few comments about which method is best for a given company.
Method 1: programmed path is work surface and offset is the cutter's size. With Method 1, the programmed path is a series of coordinates that are right on the workpiece. These coordinates are quite easy to determine, many times coming right from the blueprint. The setup person will specify the size of the cutter (its radius or diameter, depending upon the control manufacturer) in the cutter radius compensation offset. When the program is run, the control will keep the cutter away from the programmed path (the work surface) based upon what it sees in the offset, effectively machining the contour to its desired size.
For example, if the setup person uses a 1-inch cutter, and if the control manufacturer requires that the offset be specified in radius, the cutter radius compensation offset will be set to 0.5 inch.
Method 2: programmed path is cutter centerline path and offset is the deviation from planned cutter size. With Method 2, the programmed path is based upon a planned cutter size. The programmed coordinates will be the centerline path of this cutter as it machines the contour. In the offset, the setup person will specify the deviation from the planned cutter size to the size of the cutter actually being used. Again, control manufacturers vary when it comes to whether the offset must be specified as radius or diameter deviation.
For example, if the programmer plans for a 1-inch cutter, all programmed coordinates will be kept 0.5 inch from the work surface. If the setup person uses a 1-inch cutter, the cutter radius compensation offset will be 0 (the planned cutter size is being used). If the setup person uses a 0.75-diameter cutter, the actual cutter size is smaller than the planned cutter size, and the offset value will be set to -0.125 (assuming the control requires the deviation to be specified in radius). If the setup person uses a 1.25-diameter cutter, the offset will be set to 0.125 (the actual cutter size is larger than the planned cutter size).
Which method is better? Because programmed coordinates are so much easier to calculate, most manual programmers prefer Method 1. The more complicated the contour to be programmed, the more manual programmers cling to Method 1. A CAM system can calculate centerline path coordinates just as easily as it can calculate work surface path coordinates. This means CAM system programmers tend to have more of a choice to make.
Your choice should be based upon simplifying the use of the CNC machine for setup people and operators. Remember, they're the people who actually make your company's money. Keep it as simple as possible for them. So the question becomes, "Which method minimizes the potential for mistakes at the machine?" Just choose the method that best answers this question for your own company.
Though this may open the door to a great deal of debate, here comes my opinion. People tend to be too quick to jump to the conclusion that Method 1 is best. Admittedly, the cutter's initial radius (or diameter) should be quite easy to determine. For new cutters, just look at the cutter. It's size is etched on the shank. For re-sharpened cutters, measure it with a micrometer. If your control requires a radius value, divide the cutter diameter by 2.
With Method 2, the setup person must know the intended cutter size. It should be included in the setup documentation, and a message should be placed at the beginning of the CNC program. If your company uses many new cutters, the related offset values will be zero, meaning the setup person may have nothing to do, eliminating the need for any kind of action.
Again, this choice must be based upon simplifying things for setup people and operators. Judge the wisdom of your current choice by how many scrap-causing mistakes are currently being made.blog comments powered by Disqus