[mcardoso]

Just wanted to open a discussion on what people find works well for benchtop class machines for CNC strategies.


I have a 2.5 HP spindle that I would like to take full advantage of. My machine (G0704) does not have the column stiffness to handle tools much larger than 3/8" nor does the 5000rpm max spindle speed allow me to run small tools really fast like a router table would. The sky is the limit when it comes to feedrate and accelerations for me (servos).


I have found that trochoidal toolpaths with full depth of cut engagement seem to work well, but I have always stuck to 15% of cutter diameter stepover in aluminum and roughly .001 to .0015 feed per tooth. This ends up only using <1HP. Specifically for roughing, what strategy would you recommend to take advantage of the remaining spindle power? Would you increase radial engagement for a wider chip or rather increase the chip thickness? Would plunge roughing be worth looking into? I've always wanted to experiment with high feed milling as you can get high material removal with smaller tools at lower spindle speeds.

[CL_MotoTech]

I run my 3/8" 2 flute at .003" fpt. Generally this is something like 6k speed and 36ipm feed. I use trochoidal paths as well and find that I get really good results this way. I'm sure you get better rapids than I do (200ipm), but even when I max my spindle to 8k I still am rarely running feeds over 50ipm, only with a 4 flute .5" rougher have I consistently run over 50ipm.

I've never done plunge roughing, but it has been on my radar as something to try.

With my 2.2kw spindle I have run as large as .5" end mills for roughing, but for finishing I have the best luck with 3/8" and .25", but I can get away with using the full face of the tool this way.

[hanermo]

I suggest you are chasing a unicorn.

You are already getting excellent results, much better than most, and a lot of it is probably due to the servos.
Not at all due to power, or speed in rpm, but because you get very low lag and deflection since the servos react so fast. (Like mine).
Typical update loop = 12 khz, so the servos try to catch up in 0.1 ms, a bit less.
So this keeps the frame steadily loaded.

Your machine frame probably twists like spaghetti, already.
For example a classic Bridgeport 2 HP, 1000 kg, 20x40", twists == 0.04 mm with two fingers pressure on the edge of the table.
A BP cannot use + 2 HP of cutting power efficiently.
Almost all use is under 0.5 HP.

A typical traditional cut in steel, 1.5-2 HP, would require about 50-70 kgf of push force. Near 180 lbs.
Formulas online.

Corncob roughers can cut the load 60%+.
So can HSM.

Example.
Imagine standing the machine on its side.
Step on the spindle mounted tool, with your approx 70 kgf / 180 lbs mass.
If 10 kgf on a steel table of 200 kgf mass (BP) distorts 0.04 mm = 0.002", how much will 180 lbs do on your spindle mounted tool.
Will your toolbit stand 70 kgf mass ?

A: No.
A: Yes.
Tiny DT/DM/Brother Speedio machining centers do 200-400 kgf++ tool forces for tens of thousands of hours.
Using extremely good spindles, collets, toolholders, tools.
A long gage length. = Taper length of toolholder inside spindle. Gage power 3 = rigidity.


Example.
A full blown HAAS machining center - I used to sell these - 25 kW - ISO40 - typically will cut at about 1-2-3 kW in steel, mostly.
A large majority of all cuts are about 1 kW or less.
Entries into material peak, for sub-second.
Accelerations are 25 kW, for 1-2 secs, to get to speed in rpm.
Cutting is mostly under 0.5-0.8 kW.

Your limiting factors are likely frame rigidity, spindle mount rigidity, tool mount rigidity (Maybe ER of some kind), tool rigidity and tool quality.
The HAAS DM and Brother Speedio machines can do 20 kW+ output in ER 20, ER30.
An SK taper machine might be 10x more rigid in the same size.

Having said that, I got 30x the cutting performance in milling on my lathe.
30 times faster.
50 mm thick 200 x 400 steel slab as mount. Yes, about 30 kg mass.
ISO40 insert face mill in spindle (held in 4-jaw chuck). 4 inserts, apkx.

Cutting 3.5 mm deep in tool steel, and 600 rpm, and fast feed, resulted in about 30x the total MRR I have ever done.
Spindle power is now 2.5 kW ac brushless servo, about 2-3x a normal ac motor.
90 Nm torque at 1:3 via HTD-8-30 belts (rated 30 kW+).

I went from 200 to 700 in feed by mistake via analog pot on the remote, and the cut was 3 mm deeper than it was meant to be.
The surface finish was exceptional.

Yet:
On a lathe the loads go to the saddle->body.
The mount plate was exceptionally rigid, and so are my ballscrews, and 750W 10.000 count 220V servos. (Screws, old, 0.750").
Free length == 140 mm from lathe bed.
10" 4 -jaw chuck of 12 kg adds huge inertial dampening.
MT5 spindle taper is probably much more than most small DIY/CNCz/home mills.

So it IS possible to load 2.5 kW of real output power into cutting steel.
I have done it 3-4 times on the lathe.
But I think it is unrealistic for most mills, and for most users.

[mcardoso]

Totally agreed hanermo! I have 1.8kW continuous available but doubt I'll be able to use that much continuously. That being said, being smart about toolpath selection will probably get me pretty far compared to straight slotting. Just curious. I don't need to do any crazy material removal rates, just want to be efficient.

[mcardoso]

To go along with the above questions, I've heard the comment made about lathe inserts that you shouldn't buy more carbide than you need (choose the smallest insert that meets the depth of cut requirement). Not sure if I have heard the same for endmills. Is it better to run a larger tool but maybe not run it as hard as it can go, or run a smaller tool harder? Tool deflection comes to mind. I know I can do a 20% stepover on a 3/8" endmill, but would I be better doing a 40 or 50% stepover on a 1/4" endmill?

[CL_MotoTech]

I suggest you are chasing a unicorn.

You are already getting excellent results, much better than most, and a lot of it is probably due to the servos.
Not at all due to power, or speed in rpm, but because you get very low lag and deflection since the servos react so fast. (Like mine).
Typical update loop = 12 khz, so the servos try to catch up in 0.1 ms, a bit less.
So this keeps the frame steadily loaded.

Can you explain how low lag servo reactions reduce deflection?

[ninefinger]

To go along with the above questions, I've heard the comment made about lathe inserts that you shouldn't buy more carbide than you need (choose the smallest insert that meets the depth of cut requirement). Not sure if I have heard the same for endmills. Is it better to run a larger tool but maybe not run it as hard as it can go, or run a smaller tool harder? Tool deflection comes to mind. I know I can do a 20% stepover on a 3/8" endmill, but would I be better doing a 40 or 50% stepover on a 1/4" endmill?

Its going to depend on your spindle speed capability - if you can run fast then a smaller cutter will be the tool of choice - but if you can't run high rpm then a larger (by a little) cutter will be better for the machine. The smaller cutter will typically have lower cutting forces so less deflection but the tool is less stiff due to smaller diameter, but a larger diameter cutter can have less deflection despite larger cutting forces. Play with what you got to find the optimum.

Mike

[CL_MotoTech]

In my experience a .25" 3 flute carbide end mill with as little tool stick out as possible gives me the best accuracy and repeatability on small pockets and faces. I run it slow to get that though, something like 20ipm. Once I get the machine much over 50ipm dimensions get a little dicey. I get great results with a .375" two flute as well, but again, once the feeds get too high the machine rigidity becomes an issue.

I like to leave .02" for my finishing routines and really turn down the feed and speed. I always finish in climb.

The only reason I run such a large spindle motor is for tapping, the majority of the time it's not needed.

[Oon86]

Hi. Im new here
My boss factory using Mitsubishi vmc1000
Everytime i need transfer program for processing
But why sometimes the memory of vmc1000 so fast over?
Can i add om memory to the machine or my configuration of the machine having problem?
Tq guys
Appreciate very

[ChrisAttebery]

mcardoso,

I have a G0704 with a 1100W motor on it. I ran it at 4500 rpm for a few years and then bumped it up to 6750 rpm last year. I generally shoot for a MRR of 1.3in/min. I use high quality HSS end mills because they are cheap and these machines don't have the rigidity to use carbide efficiently.

My go to parameters are:
3/8" 2 flute YG-1 aluminum end mill
Speed: 6000 rpm
DOC: .500"
WOC: .05"
Feed: 54 IPM

My general rules for HSM in aluminum are to use full depth, 10-20% WOC, 1-2% feed per tooth. If I need to reduce DOC I increase WOC up to 20%, then I start adding feed. I wish someone made a 3/8" 3 flute in HSS. That would be my next step.

All of this assumes that you have a coolant system of some sort. I use a home brew mist system.

Good luck,


Chris

[ChrisAttebery]

No idea. You're posing in the Benchtop machines forum. Find the correct forum for your machine.

Hi. Im new here
My boss factory using Mitsubishi vmc1000
Everytime i need transfer program for processing
But why sometimes the memory of vmc1000 so fast over?
Can i add om memory to the machine or my configuration of the machine having problem?
Tq guys
Appreciate very

[ChrisAttebery]

BTW: I have used 3/8" 3F carbide end mills in the past. They worked great but cost about 3X what the 3/8" 2F HSS end mills do. I decided that for my needs it wasn't worth the extra expense.

[Jim Dawson]

To go along with the above questions, I've heard the comment made about lathe inserts that you shouldn't buy more carbide than you need (choose the smallest insert that meets the depth of cut requirement). Not sure if I have heard the same for endmills. Is it better to run a larger tool but maybe not run it as hard as it can go, or run a smaller tool harder? Tool deflection comes to mind. I know I can do a 20% stepover on a 3/8" endmill, but would I be better doing a 40 or 50% stepover on a 1/4" endmill?

What happens if you use a 40% stepover with a 3/8 endmill and a trochoidal cutting path? This is what I use with my machine, with a 3 HP spindle, normally ~1D DOC, 20-40 IPM.

[steelcogs]

My go to cutting recipe for 3FL 1/4" and 3/8" endmills are 5000 RPM and .003ipt at 1x diameter depth and ~20% stepover. I did once forget to add a multiple depths pass and a 3/8" endmill took a 5/8" DoC with it setup for 20% stepover (it was cutting a small area I'm not sure how close it got to that 20%) like a champ, and that was only with a 1HP servo. I was using mainly Lakeshore carbide tools but just recently bought some YG-1 endmills and am really impressed so far.

As far as smaller endmills (like 1/16") it's tough but still doable. I just had a project where I made basically 3D extruded letters and I needed to use a 1/16" 2fl, uncoated endmill to clear out as much of the material between the letters as possible. My best recipe ended up being 5000 RPM, .001ipt, 1x DoC, 20% stepover. I only broke this tool because when I went back to do the 2d contour and clean up the insides there was just too much material left in a very tight V corner and it was too much for it. Previously it did the roughing program in 1 1/2 hours with no issues. Previous to this I had tried single flute 1/16" endmills because it was all I was able to order and get on short notice. I went through 5 of these with super conservative recipes before giving up and ordering 2 fluters.

I'm also using a DIY fogbuster with Kool Mist for all these cuts.