Firstly, I am surprised you were told NOT to adjust spindle speed. I would be curious as to the reason.
Chatter is the likely cause of chipping and poor tool life. Reducing chatter is what needs to be done to eliminate or reduce these effects.
I did a sort of whitepaper on chatter a while back and posted it somewhere in the forum. Since I cannot remember the topic, here is the link to that paper which is on our blog blog.axsysdental.com:
https://blog.axsysdental.com/cnc-machine-vibrations-and-effect-on-restoration-quality/ As a machinist, I have learned that the first thing that can be done in troubleshooting chatter IS adjusting spindle speed. Just about any experienced machinist will do this.
You can do this while machining the restoration, just listen closely while the tool is engaged. You are likely hearing the chatter. While machining, slowly reduce the spindle rpm in small increments- the chatter (noise) will either get worse or get reduced.- keep going until you get the chatter (noise) down to the lowest possible. Now go back to the original rpm and increase the spindle rpm, again slowly and in small increments to see if the chatter (noise) gets reduced even more than by increasing the rpm. You may find increasing the rpm worsens the chatter or lessens it.
Either way once you have found the rpm that reduces or hopefully eliminates the chatter, you have found the optimum spindle rpm for YOUR:
- · machine and fixture rigidity
- · spindle construction (bearings, run-out, etc.)
- · tooling (sharpness, diameter, number of flutes, coating, clearance angles, helix angle, etc.)
- · restoration material
- · cutting parameters (depth of cut, width of cut, chip load, etc.)
You may find that you cannot completely eliminate the chatter using this method as the chatter may be a result of your machine and fixture rigidity, spindle/collet (bearings, runout, etc.) and/or the chip load determined by the machining templates that are being used. Chip load is a measurement of the thickness of material removed by each cutting edge during a cut.
To begin with, effective zirconia machining is characterized by slow speeds and heavy feeds.
Also, optimum surface finish and tool life are obtained when the tool is ground with a positive 12 to 15 degrees radial rake along with cutting corner. A high spiral flute should also be used.
Now, this I know will be controversial, but studies have proven that the work should be flooded or sprayed with a coolant to completely wash away all chips from the tool.
The chip load can range from 0.005 to 0.020 inch per tooth at 150 to 250 SFPM. The work absorbs about 10 percent of the cutting energy with sharp cutters. Zirconium requires only about 75 percent of the horsepower required for SAE 1020 CR steel.
So the important parameters are: chip load or the amount of material removed by each flute of the cutter and SFPM (or the cutting speed of the end mill - the distance per minute that a given point on the circumference of a cutter travels per minute).
Studies have shown that the optimum velocity (in terms of tool wear) for machining zirconia is between 100-300 m/min, so approximately 200 m/min is a good target.
There are of course, formulas and websites available for determining feeds and speeds based on chip load and tool diameter, SFPM. Tool manufacturers also recommend optimal cutting parameters for THEIR tooling for given materials. It is best to follow these recommendations.
For example, here is a sample of a basic parameter recommendation from a tool manufacturer for machining graphite and copper alloys. This chart does not include zirconia however it will give you the basic idea.
View attachment 30113 View attachment 30114 The metric formula for spindle speed is:
RPM = {CUTTING SPEED *1000}/ PI X {DIAMETER}
Therefore the appropriate spindle speed for a 1.0 mm ball end mill at the target 200 min/min cutting velocity would be:
200*100/3.14*1 =63,662 rpm
To maintain 200 m/min velocity the programmed feed rate (mm/m) for a two flute end mill and a recommended .02mm depth of cut for zirconia would be:
FEED RATE = {FEED/TOOTH) * {NUMBER OF FLUTES} * {RPM}
.02 X 2 X 63,662 = 2,546.48 mm/min
Looking at these optimum calculations, I am fairly certain you machine/fixture set-up is not rigid enough to support these parameters- so let’s slow it down.
Remember in machining zirconia we want lower spindle speeds and faster feeds. Keeping this in mind lets do the calculations based upon a surface feed of say 150 m/min.
The spindle speed would be: 150 * 1000 / 3.14 * 1= 47,770.7 rpm
The new associated feed rate would be: .02 * 2 * 4 7,770.7 = 1,910.82 mm/min.
I’m thinking this too is likely too fast for your set-up so let’s go with a velocity of 100 m/min (still within the optimum rage of zirconia machining to achieve most favorable tool life).
The spindle speed would be 100 * 1000 / 3.14 * 1= 31,847.133
The new associated feed rate would be: .02 * 2 * 31,847.133 = 1,273.89 mm/min
This is likely best for your machine configuration however you will see longer cycle times. I should suspect you would not see a significant increase since the machine will likely never actually reach the programmed federate due to size of restoration, length of cut machine adjustments for acceleration/deceleration and other factors.
This brings about another important question for buyers of milling machines: Do you really need a machine with 80,000 or 100,000 rpm when the machine/fixture configuration cannot support the cutting feed rates necessary to support the high rpm to maintain the highest quality finish, smooth margins with minimum reinforcement and optimum tool wear? My guess is maybe, but probably not. In this case you may find, to achieve the aforementioned benefits you would never operate the spindle above say 40,000-50,000 rpm.
The above calculations are fairly close but do not take into account radial chip thinning. These calculations assume 50% cutter engagement which is not what happens in milling zirconia restorations.
View attachment 30115 I posted some information on this a while back and it is something that must be taken into account with high-speed machining of dental materials.
Calculator can be found here
: https://www.metalcuttingvision.com/__trashed-31/ Here is a good site that explains this phenomenon:
https://www.tormach.com/blog/chip-thinning-cut-aggressively/ There are many on-line feeds, speeds and chip thinning calculators that can be utilized in optimizing your cutting conditions for best quality and longer tool life. I urge everyone to look into this and optimize your machining templates.
Ask your distributor to enable you to make your own changes to meet your needs. Remember not all zirconia discs are created equal. Each has its own composition and methods of production which absolutely do affect machinability (i.e. subjectivity to chipping and tool wear, etc.).
End of report. I hope this is helpful.
Steve