[joeavaerage]

Hi,

Late last year went Starlink and its great.

Similar comments are posted in NZ too.

Craig

[peteeng]

Heres a really good article on HSM - Peter I've copied this here so I can find it....

A Machinist’s Guide to Trochoidal and Peel Milling – Make It From Metal

What High Speed Machining Is And How You Can Do It – Make It From Metal

How to Machine Aluminum: All You Need to Know – Make It From Metal

The writer calls it Peel Milling but I've always known it as thin chip or thick chip strategy.

[peteeng]

Morning all - steel cutting info
https://huanatools.com/carbide-end-m...hensive-guide/

https://youtu.be/FNP8OdYSaYE

This router is cutting steel at 220m/min with MQL approach - a 4 tooth 8mm tool at 8700rpm gives you this surface speed. Can't identify the coating... This is Fz=0.035mm/tooth

Hopefully the zone gets its act together soon............................................

https://youtu.be/fEJ0z1uuni0

[joeavaerage]

Hi, peteeng,
well, the only thing left to do is to try it. Can you replicate the results?.

Craig

[peteeng]

Hi Craig - I'll have to get my mister working.... May push my 1.5kW air cooled spindle hard but I haven't really stressed it yet....Peter

More research shows that DLC is not the go for ferrous. The TiSiN series seems to be the go. I'll survey my tool stock and pick something useful.

[joeavaerage]

Hi peteeng,
I bought a little PVD coated 0.5mm two flute endmill from Harvey Tools. Not cheap, $78USD plus shipping and that was about eight years ago.
At the time I was doing very thick copper layered circuit board (12oz/sq yd or 420um in real numbers!). The problem was not so much the copper, that could be cut quite handiliy with
my regular two flute 0.4mm and 0.5mm Kyocera tools, but it was the inevitable little bit of fiberglass underneath that caused the tool to degrade, ergo the PVD tool. As it turns out using
a software utility called Autoleveller was able to reduce the fiberglass in the chip stream and found I could get plenty of life from my regular tools.

The PVD tool I used for about 40hours cutting, and surprise surprise, I did not break it, 0.5mm carbide is very tender. Even after 40 hours its still as sharp as ever. My regular tools cost about $5USD
each, so its about a toss-up between PVD and plain carbide cost wise. Were the waste stream or material any more abrasive then the PVD tool would be favoured economically. You do need a well sorted toolpath though.
To break one of these things is like throwing money away...it hurts!

As far as the steel question goes, I know what I've tried and found to be successful and more importantly know what I found to be an absolute failure. The three recurring failure modes are trying to spin the tool
too fast, failure to keep it cool, insufficient torque which causes the spindle to stall. Your mileage may vary.

Craig

[peteeng]

Hi Craig - For my stuff I don't need to cut steel. I do need to cut composites which I have on the router with diamond tools and carbide burrs. Plus aluminium which the DLC seems to handle really well in my reading plus they mention composites so maybe you could try that as well. All seems to work well although I have no manufactures guides on how to use them The steel question is just about what's possible and occasionally I get asked can my routers cut steel. To which I say no, but I always take the line that steel is a Mills job not a routers job. There's lots of videos of people cutting steel on routers poorly, some like attached are doing it well it seems. If they are cutting steel well, its using a thin chip approach with flood or MQL. So since I always like to know the limits I'll plan on getting some suitable tooling and some bar stock. Then there's the question of the spindles bearings and how they will go. Time will tell. Peter

Guhring have coated tools for steel that top out at 340m/min which for a 6mm tool is 18000rpm so that seems doable on a router. Suttons docs top out Fc at 220m/min so they maybe more conservative...

[joeavaerage]

Hi,
as a suggestion, try using an uncoated tool. Firstly they are by far and away the cheapest and most readily available, but give a base line to work from.
What you learn from such an experiment is most likely to be able to be replicated. I would suggest say 3mm or 1/8th, because you can slow your spindle to
1/2 or 12000rpm with very low risk, and yet gets the surface speed down to the recommended levels from various manufacturers, feeds and speeds programs
etc......not withstanding the contradictions that the video suggests. Your 1.5kW spindle should have enough torque to drive a 1/8th tool comfortably, and hopefully one
of the failure modes disappears, again this should help others replicate your results.

I personally find with my little 800W spindle that I have to limit the cut depth to 0.5mm and 50% stepover and still be under the 0.3Nm torque my little spindle has.
So it is torque, or rather the lack of it, that so limits the cutting speed.

Craig

[peteeng]

Hi Craig - I wouldn't use a 3mm tool in practice so I'll start at 6mm maybe 8mm. Lanky my new router will have a 2.2kW Er20 spindle that maybe the test bed vs Scoot. So many things to get done, I need a minion or 2... Off to start assembling Lanky... Peter

[joeavaerage]

Hi peteeng,
the problem with 6mm or more it that you will perforce be operating at 200m/min or more. It is not practical or advised to slow a spindle below half speed. If you use 3mm
then you could, without risk to your spindle, get down to 118m/min, and that is what I'd believe (personal experience) is optimum, or near to it, for uncoated carbide.

You might be surprised what you can do with a 3mm tool operating in its 'sweet spot'. Sure, a toolpath can take two, three or four hours to run, but you can set it to run and walk away.
Tool life measured in hours or even tens of hours is where you want to go.

My little spindle is manual tool change, so to drill a hole, lets say 10mm, I'd run a circular interpolation type toolpath, simply because my spindle could not handle a 10mm drill in steel, and
I could not be bothered to swap the tool anyway. I can and do interpolate holes to 15mm depth, so there are limitations of course, but a 3mm tool is maybe more versatile than you think.

Craig

[peteeng]

Hi Craig - I looked up the torque for my spindle. 1500W ER16 0.5Nm. No torque curve so don't know if this is at 24k or slower. Maybe it drops off linear with speed? Anyhow looked at the Gurhring manual. Picked 6mm navigator bit 3 teeth. Vc slot max 270m/min... Fz=0.025mm DOC 6mm Put the tool data into FSwizard and heres the outcome.

12000rpm torque 0.66Nm (6mm doc) force 22.5kgf feed 921mm/min Vc=226m/min (under max 270) power 0.82kW so all doable except the torque so reduce DOC until it can cut. If torque droop is linear then at 12k I have 0.25Nm so reduce DOC to 1mm and torque required is 0.25Nm so around there is a good target for slotting... Will get some steel and bits and see how reality bits. Peter

Buy the way toroidal motion is rotary motion superimposed on a path. All machining has the tooling moving in a toroidal motion even in a straight line. So calling some machining strategies toroidal as if its special is incorrect (in my book). Circular or curved toolpaths always climbing and keeping the Fz constant is an attempt to optimise MRR and maximise tool life. Verses raster type cutting which involves lots of stop and starts that create an inconsistent Fz and lots of accles and decels which reduce the overall cutting time and the tool life.

Re: 3mm bits - The parts I envisage to cut if in steel (if I did) would be 10mm thick minimum up to 20mm thick. So 3mm tooling is a pointless exercise for me. I need 6&8&10mm diameter tools to do this... Milli would do these easily but she does not exist yet. Scoot and Lanky are routers so its a case maybe do it, maybe don't.... I can easily do these parts in aluminium but steel is 3x stiffer so attractive. But steel rusts so I have to paint it which is a big issue with fits or I get it plated 5um of zinc which is my preferred finish in this situation... I'm designing a new saddle and will cost the steel vs the aluminium one at my usual contractors to see the delta.. I'm also looking at having Epoch5 trunnion cast in aluminium or I cast it in CF and GF... then I can finish it on a router...

[joeavaerage]

Hi peteeng,

No torque curve so don't know if this is at 24k or slower.

No, the torque is constant down to zero. Most torque curves when published show decreasing torque from about 1/4 rated speed, but rather like a servo you can get torque at
zero speed....until it blows up! So below quarter speed should be considered a 'no go zone'.


Most experienced CNCers recommend no less than 1/2 rated speed, although I have gone as low as quarter rated speed, but its risking your spindle especially if it's air-cooled as mine is.
You should have rated torque down to half speed without difficulty so 0.5Nm at 12000rpm. If you were being conservative you'd ensure that the demanded torque is about half that value.....just for reliabilities sake.
Who cares if the toolpath takes longer, its better than blowing your spindle.

I need 6&8&10mm diameter tools to do this...

I understand, my own need is the same. It is just not possible with a 800W 24000 rpm spindle, and NOT for the lack of trying. I think you are being overly optimistic that a 1.5kW or even a 2.2kW
spindle will do 6mm, 8mm and 10mm tools in steel....but who knows. Indeed it is for this exact reason that I built a low speed spindle just for steel all those years ago.

I think that trying to maximize what you have is a laudable goal, and the tool you are looking at could just be the breakthrough required.

I have just used the engine hoist to get my trunnion table into the mill. I will not be swapping it in or out on a regular basis!!!. Turns out its 'big for its size'. Still to make limit and home switches for it,
and will need some covers etc...but its in place. I've got the A axis working nicely but have yet to program the C axis drive. I'm going to need to shift the Z axis bed upwards as the Z axis travel
is well compromised by the trunnion table.

Craig

[joeavaerage]

Hi,
now that I have my steel spindle (servo drive ER25) working again quite a few more options open up.

Having said that for the last few months when I've been without it I actually managed to do quite a bit with a 1/8th tool in my small spindle. Quite a bit of the
machining for the trunnion and the tooling for was done with a 1/8th tool and my little spindle.

It may not appear that there is much going on, but there is a 3mm pocket on the underside of the trunnion table into which locks the gear reducer. It provides guaranteed
alignment and no reliance on bolts for alignment. Similarly there are pockets into which the trunnion axle stubs mate, again ensuring alignment. The bolt holes
were done by circular interpolation or spot drilled, but all in one setup to ensure alignment. The only thing I could not do, largely because my steel spindle was out of action
was to machine the sides of the trunnion square and parallel, neither did I have anything powerful enough or rigid enough to do the T slots in the platter. Both of those jobs
were farmed out to a toolmaker. Not cheap but perfect results.

That tends to be my philosophy, if I can do it myself with good accuracy, then I'll do it, but if I can't for whatever reason then find and pay someone who can. That sort of expertise
and equipment for machining steel is ubiquitous.

Have got the C axis (fifth) dialed in nicely. It has a resolution of 0.01degree and can yet rotate at 444 rpm....so both very respectable speed AND resolution. The signaling rate
is 266.4kHz. Just got to love servos for this sort of application.

The A axis I'm going to do something a little different. Most of the limit switches of my machine are hooked to the controller, and the controller stops a servo from overrunning.
If something goes awry with the A axis, ie the trunnion then the whole trunnion could try to turn multiple revolutions and be a complete disaster. The trunnion table can rotate no more than
+90 degrees or less than -90 degrees.

The servos have eight digital inputs which can be assigned many (perhaps as many as two dozen) different functions. Two such functions are a CW limit and a CCW limit.
I intend to use them. They immediately stop the servo should the either limit be encountered. I might be being paranoid, but I like the security that hardware limits tied directly to the
drive.

I'll still use the controller functions for Homing, but may have to come up with some little wrinkle to get the A axis (trunnion) to Home reliably and consistently.

Craig

[joeavaerage]

Hi peteeng,
I've been scanning around for a bit trying to get a wider understanding of manufactures recommendations for surface speed. I've very much limited it to free cutting and mild steels.
There is plenty on tougher steels, but for the most part you and I are going to be concerned with mild steels.

I started with Kyocera SGS. I buy Kyocera Tycom tools for PCB making, and the same US supplier has Kyocera SGS tools at very fair prices. The top model
of endmill is the Carb-AP. Its coating is AlTiN-Namite-X, whatever that means. I suspect just a well sorted AlTiN coating. Note that for regular profile (side cutting) toolpaths
they recommend 169m/min. It's a little faster than I use (148m/min) but close. I can report that I get fair life from the Carb-AP tools at this speed, but get very much less life
at faster speeds.

The same US supplier has Destiny Tools Raptor's. They are just a quality US brand; I don't mean to suggest they are the best in the world or anything, but I do like them in steel and stainless.
They are AlTiN coated. The recommendation is 450ft/min or 145m/min. This is exactly the speed setting I use and can confirm that I get very acceptable tool life when using low volume flood cooling. I have
just taken delivery or another four 1/8th Raptor tools at $23USD each. I probably buy ten or a dozen a year, you might say I vote with my wallet.

The next one I looked t was Harvey Tools. I do buy from Harvey, but they are quite expensive, but the range of sizes and specialist cutter shapes is truly impressive.
Harvey Tools use AlTiN-nano coating on their topline tools. I presume it is just another well sorted AlTiN coating. I have posted two pics, one for low alloy steels and another for free cutting
steels as this is how Harvey split the data. For carbon steels they recommend 250 ft/min or 80.6m/min and for free cutting steels in the range of 425ft/min to 375ft/mi or 137m/min to 121m/min
depending on hardness. This comports with my use of them and have gotten useful tool life. Just a shame that he cost as much as they do.

These are three brands which I buy and use. In all cases I use either the exact recommended surface speed or very close to it and have had useful tool life from each.

Note that ALL of them are very much more conservative than the 200m/min plus that you are talking about.

I have downloaded the SECO solid endmill catalogue and am still reading through it. SECO use a material grouping scheme which is taking a little while to digest and cross reference. It does suggest
however, for the softest of free cutting steels 230m/min is recommended for regular profile type toolpaths. For harder steels, still mild and low carbon, that backs off to about 175m/min.
These types of steels are P1 through P4 in the SECO Materials Grouping (SMG) terminology. I have not used SECO solid endmills (yet), so I can't confirm the suitability of the recommendation.
I do use SECO inserts though, and it is a brand I have very high confidence in and would guess that the recommendation is solid.

Craig

[catahoula]

I was just going through some of these V(c) speeds too. Been using FSWizard and was surprised that the default surface speed for mild steel & carbide was usually in the 150-180 m/min because I had been reading about 100 m/min being a maximum on the forum somewhere. For some more references, Lakeshore Carbide puts the range at 75 - 150 m/min in low carbon steel (with advise to use heavy flood coolant). Harvey Tool cites 130 - 150 m/min.

These bt30 atc spindles (https://hz.aliexpress.com/i/3256803962109859.html) have a pretty promising looking torque curve, even the 100mm dia 24000rpm spindle cites 3000rpm minimum with 2.8 Nm torque. Figuring 4000rpm minimum for some margin for error, that's probably in the range for working with 12mm end mills in mild steel if surface speed can be at ~150 m/min with an HSM tool path and 15% stepover (theoretically, according to power calculation from FS Wizard). While maintaining the 24krpm capability for aluminum/composites. Bumping up to the 5.5kw spindle would give plenty torque margin with roughly 6 Nm at 4000rpm.

Craig, I'm looking forward to hearing about how things go with the 40krpm HSK32 spindle.

[catahoula]

speaking of spindles, anyone know why super high frequency vfd's aren't more common? it seems like in the general desire for a spindle with a wide speed range, an obvious option would be to use an 8-pole motor which has better low end torque and pair it with a 1600hz VFD to keep the high end at 24000 rpm. Am i missing something? too expensive? or does it do horrible things to motors at that frequency?

[joeavaerage]

Hi,

I was just going through some of these V(c) speeds too. Been using FSWizard and was surprised that the default surface speed for mild steel & carbide was usually in the 150-180 m/min because I had been reading about 100 m/min being a maximum on the forum somewhere. For some more references, Lakeshore Carbide puts the range at 75 - 150 m/min in low carbon steel (with advise to use heavy flood coolant). Harvey Tool cites 130 - 150 m/min.

That has been my experience also. I've suffered repeated tool failures, ie the tool gets red hot, at 200m/min and higher.

Craig, I'm looking forward to hearing about how things go with the 40krpm HSK32 spindle.

You and me both. It is in New Zealand Customs and has been for a few days. Could be just the Christmas break or they could be lining up to charge me GST (15% tax).
Even once I get it I'll still have to save up for a VFD to run it. Looking like $500USD to about $700USD for a high frequency Delta. Might be a while before I can afford one.

I did see on the screen shot of the manual that accompanies the spindle and its rated speed is 10,000rpm and its maximum is 40,000. Its rated torque is 3.34Nm. I'm thinking that if the rated speed
is 10,000rpm then I might get away with running it as low as 2500rpm. That would be great, because that would be in the 'good to go zone' for uncoated 12mm carbide in steel.
I'm a bit dubious that 3.34Nm is enough in steel. It's very easy to load a 12mm tool up and stall it in steel.

My current 'steel' spindle (1.8kW, 6.1Nm rated) runs about 50% of rated torque with moderate cuts in steel with a 12mm tool. I'm thinking I probably want a reasonable margin between demanded torque
and available (rated) torque. That in turn suggests that while I may be able to spin 12mm tools slow enough to get decent tool life, that I may have to limit the cutting speed/depth to accommodate
my spindles torque. It is still a major step up (ten-fold) on my 800W 24000rpm spindle. Now that I have my 'steel' spindle back in action after buggering it up earlier in the year....I'm a little less concerned about 'steel capacity'.
Still, I am looking forward to exploring this new spindles capabilities.

The spindle to which you linked to is broadly similar to what I have bought. The only real difference is HSK32 tool interface verses BT30 tool interface. Up to 24000rpm there really is no case for HSK32, BT30 will be
every bit as good. Over 30,000rpm HSK32 starts looking like a winner. To be honest I don't imagine that I give the high-speed end that much work....it's hard on the bearings and they wear out decidedly faster at high speeds.
For longevities sake I'll make sparing use of the 30,000 to 40,000 rpm capability.

Either way that spindle looks the part and is well priced. I'd be more than happy if it were installed on my machine.

it seems like in the general desire for a spindle with a wide speed range, an obvious option would be to use an 8-pole motor which has better low end torque and pair it with a 1600hz VFD to keep the high end at 24000 rpm.

It is too simplistic to think that an eight-pole motor has double the torque of a four-pole motor.

Like all electric motors torque is proportional to current. Let's say there is 1A flowing in each of the four poles, and that produces a torque of 2Nm. If you now made the same motor (with the same number of turns in each winding)
and supplied the same 1A into each then you could expect double the torque, ie 4Nm. The problem is that you only have a certain amount of space to wind the coils. Sure, you could make an eight pole motor
but you'd have to use thinner wire, and you'd end up in the same place. So, you could only run 0.5A in each of the eight windings for 2Nm of torque. It is seductive to believe that the more motor pole means more torque,
but it is an oversimplification that does not work in practice.

In order to get the greatest possible speed range really means that the motor must have high current capability in order to have good torque at low speed, but provided you can supply a high enough frequency
voltage there is no real limit to the top end speed. The issue then is really of cooling. High currents generate heat inside the windings. Larger windings of thicker wire reduce that heat, but that require a bigger motor
with bigger bearings which crimps you at the top end.

Of course, there are such spindles, all the big machines have got them...but they are huge and cost a fortune. The same Chinese company (Guangzhou Haozhi Industrial Co.) that made my spindle are still in business
and one of their big motors is 270mm in diameter, 840mm long and weighs 265kg with an HSK100 tool interface at 45kW!!!. It will do 10000rpm at the top end and has 309Nm continuous and 463Nm at S6-40%.
If you want to give me your credit card number I'll get them to send you one...and maybe one for me too! At 265kg I'm not sure what I would do with it....but it sure would be nice!

Craig

[joeavaerage]

Hi,
most standard VFDs are 400Hz, and increasingly frequently 600Hz. The Delta models I've been looking at are 1500Hz, as my spindle needs 1333Hz to get to max speed. VFDs that can do
1000Hz, 1200Hz, 1500Hz etc are rarer and somewhat more specialized. I did see a Yaskawa drive (I think, from memory) that was capable of 2000Hz.

Even the Delta's that I've been looking at can only do 1500Hz in V/F mode, you can't take advantage of vector mode and that sort of thing.

I suspect that the effective limit is that IGBTs that can switch at 30kHz are quite a bit more expensive and prohibitively so in the very competitive VFD market. Currently most VFD IGBTs switch at 15kHz.
You may well have seen there has been a quiet revolution in MOSFET design, with SiC technology and GaN technology being very promising. They are not yet sufficiently mature and have therefore come down in price
to the point that they will be competitive in the VFD market...but they are coming. When that occurs I think you can expect 2000Hz capable VFDs will be commonplace. At the moment you can have them,
but you have to 'pay up'.

Craig

[joeavaerage]

Hi,
I rather think that if there is any one feature that this new spindle offers that is going to be of real value it is ATC.

Sure, the numbers look promising that I'll be able to do more things with the increased power and rpm range, like steel cutting with 6mm, 8mm, 10mm and maybe even 12mm tools,
but not having to manually change tools would be a major time saver.

For example at the moment when I make a PCB I use three tools. The 60 degree engraving tool to do the 'copper etching', a 1mm carbide drill for the holes, and all holes over 1.5mm
I do by circular interpolation with a 1.5mm four flute endmill, the same endmill that I use to go around the outlie of the board. The three tools are chosen to minimize the number of manual tool changes that
I have to do. I'm hoping that ATC will mean I can have say, three carbide drills, say, 0.8mm, 1.0mm and 1.2mm. That would mean that I do not have to manually re-drill some of the 1.0mm holes to accommodate 1.2mm
part leads as I do at the moment.

Likewise when doing more normal and regular milling jobs I tend to do toolpaths in one, two or at most three tool sizes, typically 1.5mm, 3mm and 6mm. With ATC I could now call a tool change within the program
and can optimize the toolpath without a major time penalty with regard to tool changes. As an example, I use a four flute 1.5mm Kyocera tool very VERY commonly. It is a X3 tool, that is to say its flute length is only three
times the tool diameter, ie 4.5mm. It a great and tough little tool. If, however, I want a greater cut depth then I have to use a Kyocera two flute tool with a X8 flute length ie 12mm. In order to minimize the tool changes I would use
the longer tool, but necessarily slow the entire toolpath because the 1.5mm two flute tool is very much more tender. It will be a luxury to change tools to run an aggressive toolpath with the shorter, tougher tool and yet be able to
swap to the longer tool when necessary.

I can see that I have yet another project to design and build a useful ATC....but that's what good about CNC, it's a hobby that is a never-ending series of challenges.
In a related but separate challenge is shrink fit tooling. I'll probably have to build myself a small induction heater to do it. Fun, fun, fun.

Craig

[catahoula]

Thanks for the notes, good stuff.

I wasn't thinking twice the torque from 8 poles, but the chart accompanying those BT30 spindles (attached) indicates a roughly 25% increase from the 4 pole variant to the 8 pole. Not radical, but with router spindles, marginal gain is something.

I'm in a similar boat. My machine will be used for trimming carbon fiber/fiberglass laminates with 3-6mm router bits, so the sky is pretty much the limit for RPM in that application. I'll also do a fair amount of 3d contouring with 3-4mm ball end mills in aluminum, so 24k rpm is almost a minimum for that application and 40k would be quite nice. But my machine is in my detached garage so there's no reason I can't just run it all night when 3d contouring a mold. And while it's less of a priority, I'd like to be able to mill mild steel with an 8-12mm tool (in order to get enough reach for deep pockets and/or squaring up the sides of workpieces), for various tool/die creation, building parts for future CNC machines, or whatever. So while I'm fine with not being able to blast a 25mm end mill through hardened A2 steel, getting that minimum ~6 Nm + torque around 4000 rpm really opens up a lot of options.

I've considered a two spindle set up, with a servo driven low rpm main spindle like yours, and then a 40-60000 rpm ER11 tiny little guy for all the contour milling. Which would be pretty sweet but a fair amount of hassle. And as you point out, an ATC, or at the very least a manual quick-change BT30/HSK32 type set up, is the only sane way for long term use. I would set up an ATC with 3, 4, 6 mm ball end mills and 3, 4, 6, 8/12 mm square end mills. So getting just enough torque at 4k rpm with a 24k+ ATC spindle seems like the happiest medium. I've got plenty of power, so running a 65A breaker to the machine and having a 5.5kw spindle isn't outrageous, and on Aliexpress it's not any more expensive than a smaller one.

Getting ahead of myself though. I have a standard HY 2.2kw spindle and vfd and will get that set up initially. Should probably be programming that vfd instead of reading torque charts for ATC spindles!