A reader recently used the “Ask an Expert” feature of our Micromachining Zone to ask about a challenge in milling with a relatively small tool on one of his existing machines.
I have a rebuilt vertical machining center with a 10,000-rpm spindle. I'm cutting 1018 cold rolled with a 0.016-inch diameter 4-flute coated carbide end mill. I need to go 0.030 inch deep. I'm running at 9,800 rpm, feeding at 5 ipm at 0.002 inch deep. The tool gets 0.010 inch deep and breaks. Any suggestions?
Response from John Bradford, micromachining R&D team leader for Makino
Here are a few points to consider:
● Coolant—Use water soluble coolant mixed to 8 percent or less
● Dynamics—Is your tool breaking consistently at a corner or geometry transition? This could indicate issues with machine tool dynamics, servo axis stability or general machine rigidity.
● Static runout—Is there runout at the cutting tool edge relative to the shank of the cutter?
● Dynamic tool runout—Do you know with certainty what your actual tool tip runout is at full rpm? At these smaller tool diameters, tool life will be substantially reduced if the tool tip runout exceeds just 10 microns (0.0004 inch). This error amount is pretty common with standard spindles and standard collet systems. If possible, confirm your actual tool tip runout at rpm with a laser or optical measuring device. Or, at least confirm shank runout with a high-precision indicator with the spindle in static position. Try to get this to 0.0002 inch or better. (Remember, at full rpm, you will be adding in spindle vibration and spindle runout on top of this tool runout.)
In our facility, we use toolholders (both shrink-fit and collet-style) that provide us with tool runout of 0.001 mm (0.00004 inch) and less. This is critical for tool life, even with cutters in the larger size range up to 0.020 inch diameter. If you have any tool runout, you will have one flute that is performing the bulk of the cutting, and the other flutes will not be doing much work. This will lead to premature tool failure, without a question.
With the items above considered, and assuming that everything in your tool setup is ideal, I think that your feeds and speeds are not necessarily out of bounds. I would recommend that you use 8 percent of diameter or less for both step-down and step-over per pass. Also, without seeing your tool path, I am assuming that your ramp angle is ideal (1.5 degrees or less). If you have issues with any of the items mentioned above, your feeds and speeds would need to be modified.
Keep in mind: When cutting with tools less than 0.020 inch in diameter, every single issue you have with tool runout, flute runout, tool path, lead-in, machine tool stability or spindle stability becomes magnified.