[zaebis]

Ok I am sure some of you have had enough experience with the machine so enlighten me on the ballpark figures for RPM/Feed/DOC

HSS and carbide

Aluminim, 1018, stainless 304
- profiling, pocketing, roughing

thanx

[MichaelHenry]

That's kind of an open ended question. Have you done any research or trials on your own?

Mike

[zaebis]

Research yes, trials no since I dont hav the machine. The problem is that due to the nature of "mini" mills their feeds, sppeds and DOCs are quite different from what the big guys would absorb. So I was hoping to take on someone else's experience with small devices and what they concluded to be most suitable parameters.

[Ed from NY]

Actually let me piggy back on Zaebis' question...

Syil america has posted a UT video of the S3 taking 0.0375 in2 off Aluminum 6061-T6 (hardness 90) at 26 ipm. I presume he was using a regular chinese end mill (1/2" 2 flute). No RPM was mentioned. That is just under 1 cubic inch of material per minute.

The SGS demo video I linked to in the other thread is probably using a machine costing $100K and is taking 0.1 in2 on Aluminum 2024 (hardness 120) at 500 ipm and 12,000 RPM. That is 50 cubic inches of tougher material per minute, but presumably with a better end mill. Both are roughing.

That is a 50:1 difference! (for roughing, never mind capabilities)... still on one side you have a better tool, and on the other side you have a softer material.

It would be cool to see an "all things equal" comparison.



BTW, back to Zaebis question... did anyone publish a record of successful RPMs/IPMs/Steps/Tooling/Coolant/Materials for the S3... if not may be someone with a bit experience could start a thread. I think that would be cool, like a place we could refer to for a starting point -- would that make sense?

[MichaelHenry]

There's no shortage of recommendations on speeds & feeds for various materials on the web or in books. Machinery's Handbook is almost a requisite for any half-way serious home shop machinist and it has several pages on the subject. That gives you a starting point and experience will soon teach what works well for your mill and cutters.

It might also be useful to know how much HP is required for a given set of conditions as that will give you the upper bound on speeds, feeds, WOC, and DOC.

ME Consultant Standard or Pro are utilities that can do much of these calculations for you:

http://closetolerancesoftware.com/

Mike

[davereagan]

Allowable tool speeds shouldn't change much from large to small machine, but feedrates will of course be lower with a mini mill. RPM=(3.82*sfm)/tool diameter

For 1018, I'd drill at 65 sfm with HSS and 200 with carbide
Milling at more like 100 sfm for HSS and 300 with carbide because it is not constantly rubbing like a drill. Flood coolant is assumed. Coolant with some real oil is better.

For 304, I'd drill at 25-30 sfm with HSS (cobalt is much better)
Milling at 50sfm and 150 with carbide (coated cobalt and carbide are much better)

Example of formula: drilling 1/4" hole in 304 SS, 30 sfm

3.82*30/.25 = 450 rpm.

Feedrates: On my 40 taper CNC, I would mill in feed per tooth at .5% diameter for slotting. I use variable helix endmills allowing full slotting at one diameter depth. Sound will tell you a lot. Short holders, short tools.

[Ed from NY]

Allowable tool speeds shouldn't change much from large to small machine, but feedrates will of course be lower with a mini mill. RPM=(3.82*sfm)/tool diameter

For 1018, I'd drill at 65 sfm with HSS and 200 with carbide
Milling at more like 100 sfm for HSS and 300 with carbide because it is not constantly rubbing like a drill. Flood coolant is assumed. Coolant with some real oil is better.

For 304, I'd drill at 25-30 sfm with HSS (cobalt is much better)
Milling at 50sfm and 150 with carbide (coated cobalt and carbide are much better)

Example of formula: drilling 1/4" hole in 304 SS, 30 sfm

3.82*30/.25 = 450 rpm.

Feedrates: On my 40 taper CNC, I would mill in feed per tooth at .5% diameter for slotting. I use variable helix endmills allowing full slotting at one diameter depth. Sound will tell you a lot. Short holders, short tools.

Hi, how did you come up with these SFM's?

I looked at the datasheet for one of my end mills and the parameters it gives are not really applicable to a benchmill like the SX3.

If we pick the SGS 34800 which is a 1/2" 3 Flute end mill. The data sheet http://www.sgstool.com/catalogs/PDFs...s/sf_scarb.pdf says that if I'm cutting Aluminum they "recommend" 1600-2000 sfm. They say rpm = sfm * 3.82 / tool diameter (same you did), which gives us 12200-15200 rpm. The feed rate (feed per tooth x number of teeth x rpm) ends up being 220-273 IPM. Then they have the extended reach that is even more aggressive.

If we bring down the RPM to 3500, the feed rate becomes 63 IPM for an axial depth of 1.5x the diameter and a radial width of 0.5 the diameter.

In the ZCarbAP datasheet for a 1/2" cutter slotting a low carbon steel at 100% Rw they recommend 3360-4090 RPM and 32-39 IPM

All of these are way out of the range of a bench top mill. I mean you can program 3360 rpm and 32 IPM, but if we try to take a 1/2" wide and 1/2" deep slot on steel with that I suspect we will not have much success.

In these tables provided by the manufacturers the RPMs are high and the feed rate per tooth seem to require more power than we have.

So I'm not sure where to get the SFM and feed rate per tooth for this class of machine (?)

You did mention that "allowable tool speeds shouldn't change much from large to small machine, but feedrates will of course be lower with a mini mill"... Does that mean that in the two examples above we can run everything at 3000 RPM and tweak on the IPM and how much we are taking with each cut based on how much the machine complains? I mean that sounds like a plan, if it works cool

A kind of silly question, what is the difference between "slotting", "peripheral", and "contouring" which are sometimes used in these tables. I guess "slotting" is when you have 3 sides of the tool in contact with the material. Not sure about the other two. There is also "profilling" which I guess is either "peripheral" or "contouring"... Ideas?

[davereagan]

You are right on about slotting. I'm not sure about contouring vs peripheral. So, if your machine redlines at a speed below the sfm allowed by your tools, you just run your machine at full speed and adjust your feedrate. The speeds I gave are my own, but basically the same or a little lower than the Machinery's Handbook. I have burned a lot of drills and endmills in stainless, so I go even lower than they say in 304 and 316. The problem with the endmills you are looking at is that they will actually chatter more if you feed them less. If you try to run a 1/2" slot, 1/2" deep but run .0005" feed per tooth instead of .003", you will rub the endmill to death and it will sing. What I would do is find out what size Z carb endmill your machine can handle when fed correctly. Try a 1/4" Z carb at .001" fpt. If it can do that, try a 3/8" at .001, .0015" and .002" How much thrust does your machine have in the X and Y direction? How much horsepower? You should be able to easily remove 1 cubic inch of mild steel per minute for every horsepower. I have approached 2 cubic inches per minute per horsepower with a free cutting facemill on a 40 taper CNC. By the way, the Z carbs run longer dry. It is a hard thing for machinists to gt through their head, me included, but I have proven it to myself and others on here have too.

[Ed from NY]

That is a keen piece of advice... "find out what size Z carb endmill your machine can handle when fed correctly" Thank you!

I looked at the "Machine Shop Practice Vol2" by Moltrecht and found some formulas to calculate power requirements.

Rated at 1.34HP, according to Moltrecht I could get the X3 to do 3000 RPM and 27 IPM on aluminum and slot 1/4" (3 flute cutter 1/2" end mill). On a soft carbon steel do 1500 RPM and 21 IPM and slot 1/8" (4 flute cutter 1/2" end mill) -- that is with 1979 cutter technology.

With a smaller cutter or modern cutter technology things should improve... now I need to rum some trials... as soon as I get it all working.

Moltrecht says never to get at or below 0.001 inches per tooth "except with small end mills and when milling certain very hard materials. At such low feed rates the teeth will tend to runb against the workpiece instead of penetrating to form a chip, resulting in excessive tool wear"... so in the examples above I picked 0.003 and 0.0035 inches per tooth. Which is just like you said.

Interesting!

[davereagan]

Well, smaller endmills are cheaper to play with, but .003" is very high feed for a 1/8" endmill. Even with a CAT 40 spindle machine I would never feed a 1/8" endmill that hard except maybe with only .005-.010" engagement on the side. The feedrate per tooth that a cutter can handle without snapping from bending stress is proportional to its diameter, as well as the depth of cut you can take with it. I have actually snapped a 1/4" Z carb with only 1/4" depth full slotting at .0015" feed per tooth. It was quite a while ago and I have been monitoring my spindle runout much more closely since then. I looked at pictures of an X3. It appears to be a big bad macine compared to a Taig or Sherline. R8 spindle, right? I would use only collets, not endmill holders. Even on my Bridgeport, that made a huge difference. With any machine, you want the cutting edge as close to the lowest bearing of the spindle as possible. Any distance you have creates bending. Bending is proportional to the third power of the distance between support and loads, all other things being equal. I learned this in Mechanical Engineering and then again very intimately as a machinist. Some never really do. When I see a guy running a CNC with a 1/2" endmill and a holder with a 4" projection length I get really frustrated. Whatever machine he has, he could be cutting easily twice as hard with a 1.38" holder, not to mention having less runout on his cutter, because runout is proportional to length out of the spindle. You can prove this to yourself pretty easily with a vise and anything round that is a few feet long. Broomstick, threaded rod, anything. Clamp it in the vise with only 1 foot hanging out and get a feeling for how much it bends with your weight against it. Then leave 2 feet hanging out and do the same thing. You'll be flexing it 8 times as much. Yes, 2*2*2. That's because your bending moment was doubled, as well as the length over which it was applied. The third multiplier of 2 is hard to explain but it is true. Then leave 3 ft hanging out and you will get 27 times the deflection )3*3*3). I used to buy cutters with longer length of cut because they were only ~10% more money with twice the cutting edge. I wasted a bunch of hours finding out that I want the shortest cutter that will do a job. So when talking of small endmills, this is not less important, it's more important. I think your machine can handle a 1/4" varimill, cutting as much as a 1/4" slot in 1018 steel. I would use a scrap piece and build up to it. Run full speed at 3500 rpm, 1/8" depth, .001" feed per tooth (14 inches per minute). That's only .44 cubic inches per minute. See how it sounds. Listen for how much flex is released when it breaks through the material at the end of the cut. That will give you an idea of how rigid your machine is. If you want to run bigger diameter cutters, I'd run them more shallow with good feedrates ran than full depth and rubbing feedrates, but .003" fpt for a 1/8" is way high. That's a healthy feed for a 1/2" endmill fully engaged in steel. So if you wanted to cut with a 3/8" Z carb, you could try 3500 rpm, 1/4" depth, .0012" per tooth. That's 17 inches per minute and 1.6 cubic inches per minute. That is all I'd try with 1.34 hp and it may stall. Running 1/8" depth and then 3/16" depth first would be a good idea. By the way, the sfm numbers I see them giving for stainless have never given me more than a very brief experience with a tool. 303 stainless is nice. It's sulfurized and makes a nice chip, like 1018 cold rolled. Much different than 304 but with the same corrosion resistance. Let me know how it goes. By the way, I have a source for private label varimills that work quite well at about half the price of Z carbs. Email me if you'd like his email.

[Ed from NY]

Well, smaller endmills are cheaper to play with, but .003" is very high feed for a 1/8" endmill.

1/8" was the depth, the end mill was 1/2"

R8 spindle, right?

Yes.

I would use only collets, not endmill holders. Even on my Bridgeport, that made a huge difference.

I'm using collets as well.

I used to buy cutters with longer length of cut because they were only ~10% more money with twice the cutting edge.

I just made that mistake . I could have gotten the 1/2 ZCarbAP with a length of cut of 1", but I got it with 1-1/2" which increase the end mill length from 3" to 3-1/2". Same thing with the 1/4" which has a cutting length of 3/4" instead of the model which has 1/4"... however in this case the overall length did not increase.

I think your machine can handle a 1/4" varimill, cutting as much as a 1/4" slot in 1018 steel. I would use a scrap piece and build up to it. Run full speed at 3500 rpm, 1/8" depth, .001" feed per tooth (14 inches per minute). That's only .44 cubic inches per minute. See how it sounds. Listen for how much flex is released when it breaks through the material at the end of the cut. That will give you an idea of how rigid your machine is.

Cool advice! Will post results later.

If you want to run bigger diameter cutters, I'd run them more shallow with good feedrates ran than full depth and rubbing feedrates, but .003" fpt for a 1/8" is way high. That's a healthy feed for a 1/2" endmill fully engaged in steel.

That is exactly what it was. The HP requirements for that with a regular end mill turned out to be around the 1.34 Hp of the machine.

Not saying it is right, just here is what I did...

a. Feed rate per tooth = 0.0035 (because I wanted to stay away from 0.001 and most of the recomendations in the book start with 0.003)
b. RPM = 1500 (could have picked a higher RPM with a smaller feed, but then line (i) goes up)
c. Cutters = 4
d. IPM = 21 (calculated: d = a * b * c )
e. Width of cut = 0.5 (slotting)
f. Depth of cut = 0.125 (choice of removing 1/8" of material per pass)
g. Metal removal rate = 1.31 in3/min (calculated: g = d * e * f )
h. Power cte from a carbon steel with 100-120 hardness = 0.66 (from a table, based on material being cut)
i. Feed factor = 1.27 (interpolated from a table, based on the choice on (a))
j. Tool wear = 1.1 (from a table, factor for end mills)
k. Power at cutter = 1.21 hp (calculated: k = g * h * i * j)
m. Efficiency factor = 0.9 (belt driven, from a table)
n. Power at motor = 1.34 hp (calculated: n = k / m)

So if you wanted to cut with a 3/8" Z carb, you could try 3500 rpm, 1/4" depth, .0012" per tooth. That's 17 inches per minute and 1.6 cubic inches per minute. That is all I'd try with 1.34 hp and it may stall. Running 1/8" depth and then 3/16" depth first would be a good idea. By the way, the sfm numbers I see them giving for stainless have never given me more than a very brief experience with a tool. 303 stainless is nice. It's sulfurized and makes a nice chip, like 1018 cold rolled. Much different than 304 but with the same corrosion resistance. Let me know how it goes. By the way, I have a source for private label varimills that work quite well at about half the price of Z carbs. Email me if you'd like his email.

Just used the PM system in this board. You should have it.

Thanks for the advice! I'll start with the numbers you suggest and then see if I can build up to the numbers suggested in the book.

[Ed from NY]

I think your machine can handle a 1/4" varimill, cutting as much as a 1/4" slot in 1018 steel. I would use a scrap piece and build up to it. Run full speed at 3500 rpm, 1/8" depth, .001" feed per tooth (14 inches per minute). That's only .44 cubic inches per minute. See how it sounds. Listen for how much flex is released when it breaks through the material at the end of the cut. That will give you an idea of how rigid your machine is.

Wow that was pretty close...

a = 0.001
b = 3500
c = 4
d = 14
e = 0.25
f = 0.25
g = 0.875
h = 0.69 (126 hardness)
i = 1.6 (goes up A LOT with smaller (a)'s)
j = 1.1
k = 1.06
m = 0.9
n = 1.18 hp

[Edit]

I do not have any projects now that use steel. My next 2 projects use Nylon, but I ordered some A36 (two one-foot pieces of 1x4) and 1018 (one two-foot piece of 1x4) to run some tests, and to use in projects later. Got it from http://www.metalsdepot.com 1x4 seems to offer the best pricing and fits right in the envelope of the machine.

.

[Ed from NY]

Hi Dave,

I made the guy an offer for two 3/8" and two 1/2". The expectation is to break/chip at least one of each in the trials.

I did not get the 1/4 because I can probably work back the results based on the hp the machine is happy to work with. Also my guess is that the 1/4 is probably more likely to snap then to stall. I'm also hoping that the 1/2 fails by stalling not breaking (due to the low hp on the SX3). Will see.

Thanks! I feel empowered to experiment now

It should take me a week or two to get the other parts, resolve the spindle problem, and take the axis apart and put them back together. By that time I think I'll have a webcam in the basement and you will be able to hear me cheer or curse depending on the results of each run :lol:

[gn3dr]

I'm looking forward to following this thread - hopefully it will continue. I still have trouble settling on feeds and speeds. Like has been said previously I should really sit down and just experiment but I never put aside teh time to do that. I only remember when I am doing my next milling job and then it is a case of get the job done rather than experiment too much.

To throw a few figures out there - I'm using an X4+ (I'm also in metric land so all figures below are in mm)

For aluminium I've been running at approx 1500 rpm with an 8mm 3 flute HSS endmill with a feed rate of approx 150

For steel (not sure what type but probably plain BMS) I've been running about 650 rpm with a 11mm 4 flute hss endmill at a feed rate of about 30.

For plunging with any of the sizes of endmill the feed rate is drastically reduced as the head starts to vibrate and it's easy to miss z steps. Usually I run at at a z feed of no more than 20 - usually closer to 10.

I'm sure the figures above are conservative and I would like to push the machine more. Hopefully others will post some expample feeds on here as well.

By the way all figures above are without coolant - I really need to get an enclosure built and get the coolant running.

[Ed from NY]

By the way all figures above are without coolant - I really need to get an enclosure built and get the coolant running.

Hi, I can not comment on the figures yet, but speaking of coolant... I'm very psyched about using just compressed air for steel and perhaps mist for Aluminum. The SGS Tool guy told me that only 40 psi would do it, but plan on experiment and would not mind running close to 100 psi to really blow those chips out of the way ASAP.

The challenge is mist. Since you have a lot of air flowing (higher pressures) I guess you want a very "airy" mist. It probably atomizes big time. I would like to experiment with a negative pressure enclosure and an high volume exhaust line, but that seems to be very complicated and my exhaust line would run for over 50ft.

If the mist turns out to be too much to handle I would like to try flood at moderate pressures (like a good squirt gun pressure).

The idea I would like to play with is not coolant as much for cooling, but coolant to remove the chips right away and avoiding recutting... and keeping things neat

It would be great to hear from anyone that has had experience messing with that, pitfalls on building the enclosures, exhausting the mist, etc... It seems that a lot of little surprises/issues could come up

[gn3dr]

On the coolant - yes I agree flushing out chips is a big want for me too.

There's a thread on here where the guy built a very nice enclosure

http://www.cnczone.com/forums/showthread.php?t=76676

Personally I think the compressor is not the way to go. ALthough I have manually used an air gun to blow chips - it does work OK. I just would not want to listen to a compressor running too often.

Hi, I can not comment on the figures yet, but speaking of coolant... I'm very psyched about using just compressed air for steel and perhaps mist for Aluminum. The SGS Tool guy told me that only 40 psi would do it, but plan on experiment and would not mind running close to 100 psi to really blow those chips out of the way ASAP.

The challenge is mist. Since you have a lot of air flowing (higher pressures) I guess you want a very "airy" mist. It probably atomizes big time. I would like to experiment with a negative pressure enclosure and an high volume exhaust line, but that seems to be very complicated and my exhaust line would run for over 50ft.

If the mist turns out to be too much to handle I would like to try flood at moderate pressures (like a good squirt gun pressure).

The idea I would like to play with is not coolant as much for cooling, but coolant to remove the chips right away and avoiding recutting... and keeping things neat

It would be great to hear from anyone that has had experience messing with that, pitfalls on building the enclosures, exhausting the mist, etc... It seems that a lot of little surprises/issues could come up

[Ed from NY]

There's a thread on here where the guy built a very nice enclosure

http://www.cnczone.com/forums/showthread.php?t=76676

Wow, really nice. I have to get it up and running ASAP and I have a few others things going on, so I can not spend the time on such an elaborate build, but it is definitely something to keep in mind and build one like that later...

[pengineer]

I am cutting black ABS and in some spots it is melting and not really cutting. I am using a 1/4" end and ball mill to use the piece. I am new to cnc and was wondering if I should slow the feed rate, rpms, stepover or stepdown. As it is I have a .1 stepover and .06 stepdown and cutting at 7800 rpm. Thanks guys!

[Ed from NY]

I am cutting black ABS and in some spots it is melting and not really cutting. I am using a 1/4" end and ball mill to use the piece. I am new to cnc and was wondering if I should slow the feed rate, rpms, stepover or stepdown. As it is I have a .1 stepover and .06 stepdown and cutting at 7800 rpm. Thanks guys!

Hi, from a person that knows very little... that would be me...

I want to take a stab at this to see if I got the principles right. Please feel free to school me on what I got wrong.

I think you need to either generate less heat or to take heat away from the workpiece more efficiently.

To generate less heat, calculate you feed rate per tooth and make sure it is above 0.001 so that the mill is actually "cutting" as opposed to "rubbing" and reduce the RPM accordingly.

If that does not do it then try to remove heat more efficiently by: (a) more energetic cooling... blast it by hand with 60 psi just to see where it gets you and/or (b) increase feed rate per tooth to remove more material and with each bigger chip carry away more heat... you would still need cooling to move the chips away from the area being cut.

[Edit]

I think the stepover and stepdown are more closely related to spindle power and machine rigidity requirements. Not sure if they affect RPMs and feeds that much, assuming you have the power -- meaning if you do not have the power you would need to remove less material per second/minute. As long as you are able to remove the chips from the area being cut and the coolant continues to reach the whole area being cut I do not think they affect cooling requirements that much either.



[Edit 2]

Other ways to generate less heat would be lubrication of the material being cut and sharp tools.

There is probably more, but that is all I can think of.

[Ed from NY]

Here is a spreadsheet I have been using as one reference.

It is based on Machine Shop Practice by K.H. Moltrecht

[ame="http://www.amazon.com/Machine-shop-Practice-Vol-1/dp/0831111267"]Amazon.com: Machine shop Practice Vol. 1: Karl Moltrecht: Books[/ame]

[ame="http://www.amazon.com/Machine-Shop-Practice-Vol-2/dp/0831111321"]Amazon.com: Machine Shop Practice, Vol. 2: Karl Moltrecht: Books[/ame]

.

It has calculations for Milling (1st tab) and Drilling (2nd Tab)

For informational purposes only