Dear Shop Doc,
In our facility we do a lot of general purpose face milling applications. We’ve got a new job for which we’re using a 40 taper vertical machining center. Our problem is that when we enter into cut the cutter vibrates and we get chatter on the part. The only way we can diminish the problem is to turn the feed rate down. This works but it’s frustrating, can you help?
Dear Bad Vibrations,
By turning down the feed you may be hiding the problem, and you are probably losing productivity. The good news is that you can fix this by using a simple programming solution called the “roll-in” technique.
How you approach the part is very important. The first thing you need to consider is how the chips are being formed. The position of the cutter forms each chip. To ensure immediate cutting action you want a thick chip as you enter into the cut. When exiting cut, you want to generate a thin chip. That will put less stress on the insert.
Your chatter and vibration issues are happening because you are generating a thick chip on the exit. With the roll-in technique you focus on easing the inserts into the cut to ensure a thick chip on entry and a thin chip on exit. It is important that you are always rolling in the correct direction, which is clockwise under normal spindle rotation. If you approach the component in the counterclockwise direction it will take you right back to where you began—generating a thick chip on exit, with vibration, a bad sound and a poor part finish.
I mentioned earlier that the position of the cutter forms the chip, so let’s discuss that in more detail. A common mistake is that too much of the cutter diameter is used to take radial depths of cut. An example of this is using a 4 inch diameter face mill and taking a 3-1/2 inch to 4 inch radial depth of cut (85-100 percent of the cutter diameter). This may seem as though you are “getting as much out of the cutter as possible,” but actually the end result is detrimental to productivity and tool life. This large radial cutting depth distributes radial cutting forces around the cutter diameter, resulting in opposing forces that cause vibration tendencies as well as improper chip formation.
The general rule of thumb regarding radial engagement for face milling applications is to use 70 percent of the cutter diameter. This guideline will ensure a thick to thin chip formation and the radial cutting forces will be focused on one side of the cutter diameter, eliminating vibration tendencies through the spindle.
Programming the roll-in technique is simple. Start as you normally would with a rapid traverse move to your “X,” “Y” and “Z” starting positions. The only change is to ensure you leave enough room in the radial direction to clear the part and position the cutter to allow for a clockwise entry arc into the part (common practice for your entry arc is at least one half the cutter diameters).
The roll-in technique is a very simple programming solution. Simply add one line to your program to allow the cutter to arc into the cut in the clockwise direction. Using the roll-in technique gives you a secure process, good surface finish and part quality, as well as increased tool life and productivity.
Kevin Lorch, Project Manager of Business Strategies and Development at Sandvik Coromant.
Article originally published on Today’s Machining World