# High speed machining?



## Jake2465 (Apr 27, 2018)

I have been watching some of these guys on YouTube using their high dollar mills to machine things. I commonly see where they like to turn a real high RPM and then take the width of cut down considerably while having a full depth of cut. I am not sure if this is what people refer to as "High Efficiency Machining" or not. Part of me wonders if there is really that much of an advantage to machining that way or not. The mill has to perform tons of movements to complete it's too path. I thought "Hey, why not just drop the RPM down to something reasonable and just increase the width of cut instead of trying to make the mill run like a CNC router with a 20,000 rpm spindle?".


----------



## footpetaljones (Apr 27, 2018)

It is "High Efficiency Machining". 

When cutting you generally have to make a choice between having a high WOC with a low DOC or a high DOC with a low WOC. End mills don't really like to have both a high DOC and WOC. One issue is that with a high WOC and low DOC all of the heat from cutting is put into a very small area of the tool, which will quickly dull and get ruined. You'll have to throw that tool out while 90% of it has never been used. With high DOC/low WOC you are using much more of the flutes and your heat gets spread much more evenly.


----------



## Jake2465 (Apr 27, 2018)

Right, so the advantage would be longer tool life. 

So, in having a high DOC and WOC, would the end mill get too much deflection issues? I guess I am viewing it in terms of metal removal rates. If I have a mill that turns 10,000 rpm and runs a .050 WOC and manages to clear, let's say, 6ci/min, and then I take that same mill and drop it's rpm down to 5000rpm, cut the feed speed in half and increase the WOC to .100, then wouldn't the end result be pretty close to the 10,000 rpm setup?


----------



## pdentrem (Apr 27, 2018)

Just remember that flood coolant is usually used at these high rates. 
I run some high speed mills at 60k rpm. The bits are tiny at 0.012 and 0.020”. Moves are at 30-40 ipm. For cooling I use air blast for that and chip removal. The other machines all use flood coolant and they do cut fast!


----------



## MINICNC (Apr 28, 2018)

Jake2465 said:


> I have been watching some of these guys on YouTube using their high dollar mills to machine things. I commonly see where they like to turn a real high RPM and then take the width of cut down considerably while having a full depth of cut. I am not sure if this is what people refer to as "High Efficiency Machining" or not. Part of me wonders if there is really that much of an advantage to machining that way or not. The mill has to perform tons of movements to complete it's too path. I thought "Hey, why not just drop the RPM down to something reasonable and just increase the width of cut instead of trying to make the mill run like a CNC router with a 20,000 rpm spindle?".


As Footpetaljones states it is high efficiency machining, commonly known as trochoidal or adaptive clearance machining. There are very significant advantages to this machining strategy as opposed to more traditional methods. Higher metal removal rates can be achieved. Lower cutting forces on the tool, spindle and machine. Far better tool life, less vibration etc. It is something worth exploring on lighter weight hobby CNC's where rigidity and stability is an issue, though on a small Chinese router anything more than a couple of mm's DOC on aluminium will have the machine bouncing and vibrating too much. A small width of cut in aluminium, about 12% of cutter width on 1/8" did (4mm) could work with up to 2 mm DOC on a 4mm cutter. Feed rates up to 300mm+ may be possible.


----------



## Jake2465 (Apr 28, 2018)

I just recently started experimenting with near full depth of cut moves with my mill. I am interested to see how much longer the tools will last.


----------



## Suzuki4evr (Apr 28, 2018)

I have done it just this week, high DOC and LWC works much better. Less vibration occurred as well.


----------



## Suzuki4evr (Apr 28, 2018)

Flood cooling it I might add


----------



## spumco (Apr 28, 2018)

Jake - remember that regardless of your toolpath strategy, the tool RPM is generally set by tool diameter, tool material, coating, and material.  Full slotting or 10% WOC adaptive - pretty much the same RPM.  What changes is the WOC and DOC and feed rate based on appropriate chip thickness.

I love using HEM/HSM/Adaptive (whatever it's called).  Tool life goes up, no squealing in corners, and the chip load is predictable given the right CAM software.  I can clear faster this way with smaller tools as my mill is not rigid enough to take advantage of bigger (3/4") end mills due to tool side pressure.  The only reason I use end mills larger then 1/2" now is for rigidity.  3/8"& 1/4" are my go-to sizes.

You can also get away with slightly less secure workholding and not fling the part since the tool will never get 'buried'.  Example - I (adaptive) profiled a 4140 block using 3/8" & 1/4" roughers at 1/2" DOC and .0375"/0.025" WOC using nothing but painters tape and superglue to hold it down.  Running about .0025" IPT and 400SFM + flood coolant.  No way I could have pulled this off without the constant tool pressure adaptive clearing provides.




However - it is not a finishing strategy. It will leave tool marks on sidewalls and odd patterns on the floor that need a cleanup pass.

And I just tried Fusion 360's new 'both-ways' adaptive clearing today.  This cuts in both directions (climb & conventional) while still keeping a constant chip load.  Think back and forth arcs instead of a climb arc with a straight move back to the other side for another cut.  This shaved a ton of time off a narrow pocket clearing Op and worked like magic.  And the parameters for the conventional moves are editable independently from the climb passes.

Don't know how well it works for materials that don't respond well to conventional milling, but it was the bee's knees for Delrin.


----------



## JimDawson (Apr 28, 2018)

Jake2465 said:


> I have been watching some of these guys on YouTube using their high dollar mills to machine things. I commonly see where they like to turn a real high RPM and then take the width of cut down considerably while having a full depth of cut. I am not sure if this is what people refer to as "High Efficiency Machining" or not. Part of me wonders if there is really that much of an advantage to machining that way or not. The mill has to perform tons of movements to complete it's too path. I thought "Hey, why not just drop the RPM down to something reasonable and just increase the width of cut instead of trying to make the mill run like a CNC router with a 20,000 rpm spindle?".



Jake, my son is trying to figure this out.  In 6061, his target is 200 IPM using 3/8 cutters, 1 to 1.5 D DOC.  Right now he's running up to 2 D DOC at around 90 IPM and 15% to 40% stepover it's doing quite well.  Maxing out the spindle at 6K RPM  The goal is to maximize the material removal rate, and still leave an acceptable finish. He will be doing comparisons between different cutting strategies and tooling to try to determine the most efficient method.  He'll be working with the Fusion 360 development team and tooling vendors to incorporate his findings.  Oh, and doing this while making money with the machine 

Going to be an interesting ride.


----------



## spumco (Apr 28, 2018)

JimDawson said:


> In 6061, his target is 200 IPM using 3/8 cutters



HSM Advisor gives me some interesting numbers with that target.  If you could get 8kRPM, then the following parameters gets the MRR north of 6cu/in:
2hp spindle; 3/8" 3FL ZrN coated, .750 flute length; .625" DOC & 15% WOC, 8kRPM, .005" IPT (.0075IPT w/chip thinning) at 180IPM feed.

That's at 95% spindle load (reported).  Limited to 6kRPM means giant IPT setting (like 0.008") that - I suspect - would leave a less than awesome surface finish.

Mucho interested in results!


----------



## JimDawson (Apr 28, 2018)

We're about to find out what that new Haas will really do.


----------



## Jake2465 (Apr 28, 2018)

This week I plan to order some Alu-Power three flute end mills in the 3/8" and 1/2" diameters. I am finding that my nice rigid 4 flute end mills don't really like to do helical ramps over 3 deg in aluminum or anywhere there could be chip evacuation issues. Despite what people have told me about those 4 flute end mills, I have good success with clearing aluminum using them as long as I use plenty of water with my spray mist.

Lake Shore Carbide sells their TAS "The Aluminum Shredder" three flute end mills. I saw NYC-CNC take a 24deg helical ramp angle with that end mill and survive. They are a fair bit pricey though.  http://www.lakeshorecarbide.com/tasrougher.aspx. 

The way I currently run my end mills, I am only taking a .002' chip load at 24ipm and 3000rpm. But, with the planned spindle motor upgrade I imagine I could triple that chip load in aluminum and the 30 taper tooling should be able to keep up. So, I could keep the rpm the same and dial the feed up to 72IPM (for aluminum use). That would be pretty smoking fast for a 1980's knee mill .

That HAAS is on a completely different level. You should be able to get that thing to scary fast removal rates. Like, where the shop lights dim somewhat during the passes .


----------



## Jake2465 (Apr 28, 2018)

spumco said:


> Jake - remember that regardless of your toolpath strategy, the tool RPM is generally set by tool diameter, tool material, coating, and material.  Full slotting or 10% WOC adaptive - pretty much the same RPM.  What changes is the WOC and DOC and feed rate based on appropriate chip thickness.
> 
> I love using HEM/HSM/Adaptive (whatever it's called).  Tool life goes up, no squealing in corners, and the chip load is predictable given the right CAM software.  I can clear faster this way with smaller tools as my mill is not rigid enough to take advantage of bigger (3/4") end mills due to tool side pressure.  The only reason I use end mills larger then 1/2" now is for rigidity.  3/8"& 1/4" are my go-to sizes.
> 
> ...



I also just finished trying out that both ways feature. I think they preset it to something like 80% feed rate of the climbing passes as a default for the conventional milling return pass. I had just a normal rectangular clearing pocket adaptive path and It went from 7:02 to 5:33! That was really cool to watch.

My biggest issue with my mill is that the spindle is HP limited. So, whenever I have become impatient and wanted ramp up the feed rates, I can near my spindle speed start to complain. It's a shame because the iron can handle the loads, but the spindle motor does not like it.


----------



## JimDawson (Apr 29, 2018)

Jake2465 said:


> I also just finished trying out that both ways feature.


My son was playing with that yesterday also.  Pretty cool.


----------



## spumco (Apr 29, 2018)

Jake2465 said:


> My biggest issue with my mill is that the spindle is HP limited



How many amps do you have available in your shop?  'Cause the brain trust here can probably set you up with an upgraded spindle motor...

The other thing to consider is if you're after max MRR, look at the spindle motor torque curve and figure out what the max RPM at max torque is.  Use that speed in your F&S calculator as a target and you can take bigger chunks per tooth.  As I've mentioned elsewhere on the forum, My motor & spindle can do about 7400RPM without blowing up.  However, I need to keep it to around 5500RPM if I'm hogging as the torque drops off after that.

Now that you mention spindle motors, I'm considering switching my 2hp Blackmax + VFD for a big servo - mostly to cut down on the weight the Z-axis has to lift.  A 35lb diet would help my ballscrew live a happier life, and I could increase the acceleration.  Peck drilling would look like a sewing machine at full boogie.


----------



## Jake2465 (Apr 29, 2018)

spumco said:


> How many amps do you have available in your shop?  'Cause the brain trust here can probably set you up with an upgraded spindle motor...
> 
> The other thing to consider is if you're after max MRR, look at the spindle motor torque curve and figure out what the max RPM at max torque is.  Use that speed in your F&S calculator as a target and you can take bigger chunks per tooth.  As I've mentioned elsewhere on the forum, My motor & spindle can do about 7400RPM without blowing up.  However, I need to keep it to around 5500RPM if I'm hogging as the torque drops off after that.
> 
> Now that you mention spindle motors, I'm considering switching my 2hp Blackmax + VFD for a big servo - mostly to cut down on the weight the Z-axis has to lift.  A 35lb diet would help my ballscrew live a happier life, and I could increase the acceleration.  Peck drilling would look like a sewing machine at full boogie.



I can probably run 5hp without a problem in my shop. So, probably around 17 amps at 220V. I have one of those R2E3 mills that has the odd motor configuration where the spindle motor is between the Varispeed belt compartment and the solid ram. I took measurements the other day and it would basically need a short, fat motor to replace what's already in there. I thought it would actually be cheaper to make a motor relocation bracket and a idler shaft to put a more common Baldor Super-E motor in it's place.

I checked the voltage and amperage figures off of the data plate of my mill spindle motor, and it's really not 2hp but more like 1.6hp. So, by the time the power gets to the end mill, I imagine I have something like 1.4hp at the tool and perhaps 1.2hp useable without bogging down the motor to the point where it wants to stall.

Here is my mill. I hear it's a fairly common machine, but I have not really seen any of them around my town. Everyone else just had the regular J head Bridgeport's.

I do plan to run a VFD, so I would need a inverter friendly motor for it. That way I can ditch the Varispeed so I can run a little higher RPM's for the small tools.


----------



## stioc (Apr 29, 2018)

You guys and your fancy high speed VMCs  Funny I was just thinking about the high speed cutting rates because by comparison I'm going so slow that it's kinda crazy to think how fast some of the big machines really go. I run 1800rpm (2500 capable) and usually around 7-9ipm for roughing endmills/flycutter etc and 5 or so for finishing end mills. DOC is usually about the diameter of the cutter. WOC for slotting you don't have a choice, it's the full width of the cutter but for step-over in the case of pocketing etc yes I plan to use adaptive primarily to extend the life of the tool especially around the corners. However,  adaptive clearing does cut air and if you don't have high rapids and feed rates you could extend the machine time quite a bit- which as a hobbyist doesn't matter to me all that much.


----------



## Jake2465 (Apr 29, 2018)

stioc said:


> fancy high speed VMCs



I find an odd sense of satisfaction when I have to duck for cover when the chips are flying off of the end mills. I some times have to hide behind my enclosure and hover my hand over the Estop .


----------



## stioc (Apr 29, 2018)

I do that too! especially when the flycutter starts doing its thing. I like your enclosure, I actually just built some shields this weekend for mine to contain the chips from flying all over the garage.


----------



## JimDawson (Apr 29, 2018)

Jake, this is the first time I've see a picture of your machine.  It looks like it wouldn't take much mechanically to put hand wheels on it.  You just need to move the monitor, mouse, and keyboard to a position so they are comfortable to use when standing in front of the machine.  My keyboard and mouse move with the table. The DRO works when the machine is E-Stopped.  At least you would have X & Y manual.  A little software mod would allow you to turn off the X & Y programmatically and keep the quill under jog control.  We could make that almost a full manual/CNC machine.


----------



## Suzuki4evr (Apr 30, 2018)

Jake2465 said:


> I can probably run 5hp without a problem in my shop. So, probably around 17 amps at 220V. I have one of those R2E3 mills that has the odd motor configuration where the spindle motor is between the Varispeed belt compartment and the solid ram. I took measurements the other day and it would basically need a short, fat motor to replace what's already in there. I thought it would actually be cheaper to make a motor relocation bracket and a idler shaft to put a more common Baldor Super-E motor in it's place.
> 
> I checked the voltage and amperage figures off of the data plate of my mill spindle motor, and it's really not 2hp but more like 1.6hp. So, by the time the power gets to the end mill, I imagine I have something like 1.4hp at the tool and perhaps 1.2hp useable without bogging down the motor to the point where it wants to stall.
> 
> ...


Kind of looking like a spaceship going to take off any moment now.......... hope your roof is solid


----------



## Jake2465 (Apr 30, 2018)

JimDawson said:


> It looks like it wouldn't take much mechanically to put hand wheels on it.



I wish that was the case. The detail that makes hand wheels a problem is that the ball screws don't turn on my mill. Instead, the cog tooth pulleys are mounted in one spot and when they turn, then the ball screws shift one way or the other. For whatever reason, BP set this mill up similar to a big VMC that has really fast rapids and they did not want the ball screws to start whipping around. 

I do need to move that monitor, keyboard and mouse. I had them off to the side because of the chips that would fly off of the mill. I guess I am concerned that having the keyboard closer to the mill will cause more chips to get in between the keys.


----------



## Jake2465 (Apr 30, 2018)

stioc said:


> I do that too! especially when the flycutter starts doing its thing. I like your enclosure, I actually just built some shields this weekend for mine to contain the chips from flying all over the garage.



I wonder how a fly cutter would do on my mill. I don't own one, but I do have this nice little 2" Sandvick 4 insert face mill that I picked up used off of eBay a couple years ago. I found that if I spray the surface down with WD40 and then take about a .010" DOC with it, It gives me a nice shinny finish.


----------



## Boswell (Apr 30, 2018)

Jake2465 said:


> I do need to move that monitor, keyboard and mouse. I had them off to the side because of the chips that would fly off of the mill. I guess I am concerned that having the keyboard closer to the mill will cause more chips to get in between the keys.



Check out one of the waterproof, flexible keyboards. I have one from a company called WetKeys. it is a full sized keyboard with number pad and touchpad. I don't need the flexibility but it is TOTALLY sealed and water proof (chip and coolant proof). Don't expect to touch type at at speed but it has worked out GREAT for what I need to operate Mach3 and day to day computer stuff.  When swarf starts to build up, just blow it off with the air hose.


----------



## Jake2465 (Apr 30, 2018)

Boswell said:


> Check out one of the waterproof, flexible keyboards. I have one from a company called WetKeys. it is a full sized keyboard with number pad and touchpad. I don't need the flexibility but it is TOTALLY sealed and water proof (chip and coolant proof). Don't expect to touch type at at speed but it has worked out GREAT for what I need to operate Mach3 and day to day computer stuff.  When swarf starts to build up, just blow it off with the air hose.



I will definitely check that out!


----------



## JimDawson (Apr 30, 2018)

Boswell said:


> Check out one of the waterproof, flexible keyboards. I have one from a company called WetKeys. it is a full sized keyboard with number pad and touchpad. I don't need the flexibility but it is TOTALLY sealed and water proof (chip and coolant proof). Don't expect to touch type at at speed but it has worked out GREAT for what I need to operate Mach3 and day to day computer stuff.  When swarf starts to build up, just blow it off with the air hose.



I take the opposite approach, I buy only the finest $5 keyboards and mice, purchased from the local outlet store to use on the machines. I keep a couple in stock, normally go through about 2 per year.


----------



## spumco (Apr 30, 2018)

Jake2465 said:


> I took measurements the other day and it would basically need a short, fat motor to replace what's already in there. I thought it would actually be cheaper to make a motor relocation bracket and a idler shaft to put a more common Baldor Super-E motor in it's place.



Found a couple of tear-down images on the web of your motor.  Not a standard motor at all - it appears to be a face-mount in a custom housing with a very long shaft (unless it has a sub-shaft in the photo I saw).  You aren't going to find anything that fits in that hole and mounts up to the existing location.  And it looks like the drive end of the varispeed parts are attached directly to the motor shaft, so you'd need to fabricate some jackshaft thing with bearings to support them and drive with an offset motor as you mentioned.  Might be worth calling a motor rewind shop and see if they can build you a better 3-pase motor based on the case and stator.

Nothing is ever easy, is it?


----------



## Jake2465 (Apr 30, 2018)

spumco said:


> Found a couple of tear-down images on the web of your motor.  Not a standard motor at all - it appears to be a face-mount in a custom housing with a very long shaft (unless it has a sub-shaft in the photo I saw).  You aren't going to find anything that fits in that hole and mounts up to the existing location.  And it looks like the drive end of the varispeed parts are attached directly to the motor shaft, so you'd need to fabricate some jackshaft thing with bearings to support them and drive with an offset motor as you mentioned.  Might be worth calling a motor rewind shop and see if they can build you a better 3-pase motor based on the case and stator.
> 
> Nothing is ever easy, is it?



It's always something . If I go that way, I plan to get rid of the Varispeed system altogether to simplify things and allow for a little higher RPM on the top end. Apparently, the Varispeed does not like RPM above 4500 and it's use tends to beat up the shaft it slides up and down on.  The one good thing it has to it's advantage is that the spindle motor can remain at it's optimized RPM while the spindle can change to something else.

That's partly why I would go as big as a 5hp motor. Without the Varispeed, the motor optimization would go away and I would be forced to get a motor with more torque to handle the lower rpm without stalling. The good part is that I should be able to sling the spindle up to 6,000 rpm for use with those 1/8" end mills and such. As far as I know, I should still have use of the bull gear if I need really low RPM.

That's kinda what I had in mind. And yes, that mod would look weird. A random jackshaft where a motor used to be and another belt for the sake of getting the replacement motor out of the confinement area of the head and ram.


----------



## Charcole (May 10, 2018)

Jake2465 said:


> I have been watching some of these guys on YouTube using their high dollar mills to machine things. I commonly see where they like to turn a real high RPM and then take the width of cut down considerably while having a full depth of cut. I am not sure if this is what people refer to as "High Efficiency Machining" or not. Part of me wonders if there is really that much of an advantage to machining that way or not. The mill has to perform tons of movements to complete it's too path. I thought "Hey, why not just drop the RPM down to something reasonable and just increase the width of cut instead of trying to make the mill run like a CNC router with a 20,000 rpm spindle?".




HEM*  There is a advantage with tool geometry.  
You need to consider chip clearance.  If I'm going to cut a 2. diameter from .75 start with a .5 endmill with a .150 step over isn't going to take very long to perform. I'm mean cheap ass steel.  I'mm talking 6112rpm and feeding at 122ipm.    Add a couple of passes because of deflection and bam.

Or Cut a keyway.

.468 deep and .875 wide 4 inches long.  Same part but another key but .750 key and 1.625 long and .450 deep.  3.36 minutes.  Using .625 carbide endmill stepping down .025 for a doc.  ANd starting .2 above the part.  Its worth it.  And that is being conservative.  
I use the same speed and feed for helical interpretation.  

THe place I currently work for buys LMT endmills.  .4375 and above I run them 800sfm ranging from .0055 to .0072 witha step over of .150+ ans .025 to .250 in crappy ass steel.  Now I use a different brand of end mills run them at the same speeds and feeds.  

I have some aluminum end mills.  I'm so fast the machine slows down because of calculating arc segments.  THen I have a special .750 dia 3fl insert cutter that I run 8100rpm f800. with a doc of .025.  Doesn't take long to get down through 2 inches of material.  Full width of tool.

When I started out in machining it was common to crawl through material witha hog mill and clean up witha finishing endmill.  Now days, because of changes in technology, just use a end mill and shallow doc and haul ass.  Hog mills have a place still.


----------

