Beauty Zir Milling Burs

boboyrobert

boboyrobert

Member
Full Member
Messages
59
Reaction score
0
I've been experimenting with a few different vendors for milling burs. We started with Imagine's which were good but a little pricey so I started buying them from ToolMac. That cut my price down from almost 100 dollars per bur to 30 bucks. Now there's this company called BeautyZir that sells them for 15 and claims they can mill 80-120 crowns with their most basic version (non diamond coated). I wanted to see if any of you guys have used them before and if they do last that long. Every bur I have tried, go dull pretty quick so I've mostly been focusing on price. I dont want to hear crap like you would need to load new milling strategies into hyperdent in order to use them because that is simply not true. Thank you for input! These burs will be used for milling zirconia and I have a coritec 250I.
 
CoolHandLuke

CoolHandLuke

Idiot
Full Member
Messages
10,078
Solutions
1
Reaction score
1,411
for identically sized tools no, you don't need new strategies you are right.

but if all you're getting is 100 units out of a tool, friendo you could probably do with an overhaul of your strategy in the first place.

you should be seeing easily 300 units and be replacing tools more as a force of habit rather than any longevity issue.
 
boboyrobert

boboyrobert

Member
Full Member
Messages
59
Reaction score
0
And thats why this doesn't make sense to me. My tools only last about 6 hours of mill time before margins start chipping...are milling strategies the solution?
 
CoolHandLuke

CoolHandLuke

Idiot
Full Member
Messages
10,078
Solutions
1
Reaction score
1,411
ah, so its chipping that you are trying to fix?

this can be a lot of things but i'll try to jot them all down. if i leave anything off then someone else will point it out no doubt.

1. clean and properly lubricate your machine; in the old DWX50 you had to grease the rails from time to time, consult your machine's handbook as to this maintenance.

2. address any vibration in the machine. example: i worked at a place with 2 mills on the same steel table, this caused both machines to wobble while in use. this wobble translates directly into tool deflection and chipping or breakages.

3. perform a collet cleaning and get your runout checked with a gauge. most collet cleaning kits contain a pin for use in securing the collet while tightening so that the fingers of the collet don't deform or break. use this pin in your runout checks. you absolutely do not want > 0.005mm runout over 10k rpm because with limited engagement tools like the 1mm finishing tool, this makes for a 10% increase in engagement, which means the tool gouges the workpiece and can dig in, insodoing while the tool might not break, it will try to rip a chunk out of the material or cause a chip.

4. calibrate your machine. it is known that some machines have touch-off issues, the machine picks a tool and touches the sensor but due to wear in the sensor, the machine understands a faulty value for the tool length. this leads to breaks all over the place, and while i'm trying to recall the name of the machine this is most problematic in i think its Wieland? other users may be able to pinpoint this for me.

5. this ones the difficult part: if the machine is still chipping after all the maintenances then you should have your CAM provider take a look at the CAM to see if there is a way to revise the speeds, feeds, or engagement for better tool life. if you have a roland, use your vpanel to turn the spindle speed down 2-4k rpm (usually 5-10%) and see if you notice a change. lower rpm means lower tool runout but also means larger cuts, which is why you'd only want to trim off 5-10% of the speed at most.
 
boboyrobert

boboyrobert

Member
Full Member
Messages
59
Reaction score
0
ah, so its chipping that you are trying to fix?

this can be a lot of things but i'll try to jot them all down. if i leave anything off then someone else will point it out no doubt.

1. clean and properly lubricate your machine; in the old DWX50 you had to grease the rails from time to time, consult your machine's handbook as to this maintenance.

2. address any vibration in the machine. example: i worked at a place with 2 mills on the same steel table, this caused both machines to wobble while in use. this wobble translates directly into tool deflection and chipping or breakages.

3. perform a collet cleaning and get your runout checked with a gauge. most collet cleaning kits contain a pin for use in securing the collet while tightening so that the fingers of the collet don't deform or break. use this pin in your runout checks. you absolutely do not want > 0.005mm runout over 10k rpm because with limited engagement tools like the 1mm finishing tool, this makes for a 10% increase in engagement, which means the tool gouges the workpiece and can dig in, insodoing while the tool might not break, it will try to rip a chunk out of the material or cause a chip.

4. calibrate your machine. it is known that some machines have touch-off issues, the machine picks a tool and touches the sensor but due to wear in the sensor, the machine understands a faulty value for the tool length. this leads to breaks all over the place, and while i'm trying to recall the name of the machine this is most problematic in i think its Wieland? other users may be able to pinpoint this for me.

5. this ones the difficult part: if the machine is still chipping after all the maintenances then you should have your CAM provider take a look at the CAM to see if there is a way to revise the speeds, feeds, or engagement for better tool life. if you have a roland, use your vpanel to turn the spindle speed down 2-4k rpm (usually 5-10%) and see if you notice a change. lower rpm means lower tool runout but also means larger cuts, which is why you'd only want to trim off 5-10% of the speed at most.
I'll contact my reseller and do a lubrication this week. The table it sits on is very sturdy with no other mills running around it most of the time. I calibrate regularly and it doesn't make much of a difference.

Addressing the runout: The coritec 250I measures the length of the tool every time it grabs it and puts that into consideration when milling so could that still be a problem? I do collet cleaning regularly as well. Its always generally pretty clean. I think the problem is addressing the milling strategies and spindle speeds. The only reason why I didnt want to go there was because my reseller used it as an excuse for me only to keep buying their burs and it really pissed me off. They said it would take hours to program new milling strategies in for a different vendors burs (not even asking who I was buying them from).
 
CoolHandLuke

CoolHandLuke

Idiot
Full Member
Messages
10,078
Solutions
1
Reaction score
1,411
well, length of the tool does matter. strategies are usually made for specific tools because the tool's deflection has been measured and accounted for. its not a huge deal to get new tools in the same sequence, but it does matter somewhat.

it is highly unlikely that such precision calculations were used in the CAM that even a few mm of extra tool would put so much deflection in the tool that it would create catastrophic chipping.

if anything i'd bet since this an imes machine, the vibration is in the machine itself. the 250 is the one that went AG style and put the spindle on its side. you mentioned imagine and hyperdent? is imagine your machine and cam reseller? if so, they really know their stuff but i've never known them to be that pedantic about tooling.
 
CoolHandLuke

CoolHandLuke

Idiot
Full Member
Messages
10,078
Solutions
1
Reaction score
1,411
important to note that this horizontally mounted spindle is particularly sensitive to length changes, because the tool now isn't hanging vertically, its laying horizontally. gravity has a larger impact on deflection in this instance.

so yeah i'm going to go ahead and agree with imagine (if that's your cam provider) that your tools need new strategies if they measure longer than the "right" ones.
 
boboyrobert

boboyrobert

Member
Full Member
Messages
59
Reaction score
0
Thats just what they told me. Was that it was "hard" to program in new strategies for a different bur manufacturer. But when we come down to basics, a new bur works excellent. There's no doubt about that. The problem is that it gets dull quickly. A calibration with the same bur that eventually causes chipping doesn't help. We mostly use argen ht and stml which seem pretty soft compared to katana or other zircobia, so it can't be the grade of the zirconia causing it. I'll invest in a good bur and see if that helps and lubricate machine. The offset during calibration is never that much when I do calibrate so the integrity of the machine is fine. Does that sound like a good start? Thanks for your help. I really appreciate the input.
 
boboyrobert

boboyrobert

Member
Full Member
Messages
59
Reaction score
0
important to note that this horizontally mounted spindle is particularly sensitive to length changes, because the tool now isn't hanging vertically, its laying horizontally. gravity has a larger impact on deflection in this instance.

so yeah i'm going to go ahead and agree with imagine (if that's your cam provider) that your tools need new strategies if they measure longer than the "right" ones.
Sounds good. I'll contact them and get some new strategies in place.
 
user name

user name

Well-Known Member
Full Member
Messages
6,960
Reaction score
1,633
Dont forget dry air. Sticky Zr dust on burs causes chipping.

All burs arent identical, so strategies may well need to change. I prefer to pay more and use what the mfg uses.

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
 
boboyrobert

boboyrobert

Member
Full Member
Messages
59
Reaction score
0
Dont forget dry air. Sticky Zr dust on burs causes chipping.

All burs arent identical, so strategies may well need to change. I prefer to pay more and use what the mfg uses.
Wow thank you so much. I can't believe I missed this! I'll try programming in a new feed rate and see what happens.
 
JMN

JMN

Christian Member
Full Member
Messages
12,205
Reaction score
1,884
Wow thank you so much. I can't believe I missed this! I'll try programming in a new feed rate and see what happens.
If you want to investigate your air, start by seeing if dust is sticking to the burr or anything else. If so, your air is too moist.

Username is a air guru and has written many detailed informing posts which can be found here on DLN.
 
boboyrobert

boboyrobert

Member
Full Member
Messages
59
Reaction score
0
Someone mentioned that briefly, but we're based in Eastern Washington and the climate is always dust dry. I have never seen dust collect on the burr but that's good to know. I'll still be watching out for it now that I know it might effect the quality.
 
boboyrobert

boboyrobert

Member
Full Member
Messages
59
Reaction score
0
Dont forget dry air. Sticky Zr dust on burs causes chipping.

All burs arent identical, so strategies may well need to change. I prefer to pay more and use what the mfg uses.
Maybe I'll switch back to what I was using in the first place (imagine's burs) if changing the feed rate doesn't help. I'm milling 6 restorations right now and I can already hear the difference.
 
boboyrobert

boboyrobert

Member
Full Member
Messages
59
Reaction score
0
Update! I changed the feed rate which was set at 16000 (seemed a little high). But here's the punchline... We have a Quatro IVac 2.0 and it's supposed to tell me when to "service filters". I never saw that light go on so I never thought anything of it. I thought about what some of you said about air purity so I looked inside. There are two filters. The initial filter is automatically vibrated and tapped to remove dust but the second one it not. The second filter was super dirty so I cleaned it out and put it back in. I turned it on and ran a milling session and I could hear the suction inside the machine and it was much more powerful than before. My margins are great now that the vacuum actually works to it's full potential! It's amazing what just a tiny bit of dust in the air can do to those burs. I guess they are spinning at pretty fast RPM. Problem solved! Thank you all so much for your input.
 
user name

user name

Well-Known Member
Full Member
Messages
6,960
Reaction score
1,633
Update! I changed the feed rate which was set at 16000 (seemed a little high). But here's the punchline... We have a Quatro IVac 2.0 and it's supposed to tell me when to "service filters". I never saw that light go on so I never thought anything of it. I thought about what some of you said about air purity so I looked inside. There are two filters. The initial filter is automatically vibrated and tapped to remove dust but the second one it not. The second filter was super dirty so I cleaned it out and put it back in. I turned it on and ran a milling session and I could hear the suction inside the machine and it was much more powerful than before. My margins are great now that the vacuum actually works to it's full potential! It's amazing what just a tiny bit of dust in the air can do to those burs. I guess they are spinning at pretty fast RPM. Problem solved! Thank you all so much for your input.
Not so fast...the second filter is a HEPA. You dont clean it. Replace it! Both should be replaced every 6 months.
 
boboyrobert

boboyrobert

Member
Full Member
Messages
59
Reaction score
0
Yeah I placed an order for two of them. I just cleaned it for temporary usage.
 
Top Bottom