[Idbdan]

I'm new to milling aluminum. I'm ancient history in CNC operation. I remember the first wooden bit. lol Been searching for 2 months finding info on Speeds & Feeds for milling aluminum. Found 6 calculators, downloaded 3 programs ..... and not even one matches another's recommendation. This is getting sooooo old. This whole metal cutting speed and feed calculations is atrociously confusing. And then after I did all my research I keep reading that most have to experiment to find the "sweet spot".

I'm braking bits like there's no tomorrow. Someone please get me to a base setting where I can just cut my parts and get this whole metal thing done and I can go back to my wood projects. I don't need production speeds. Just a setting where the bit doesn't break and it doesn't travel at sloth speeds.

The confusing part is that HMS advisor has input parameters that contradict what I've used on wood. I have an RPM a Table Speed and a Plunge rate. Why does HMS have 2 feed categories in the Speed and Feed box? Way too confusing. It keeps giving me a 33K RPM???

Equipment: EZrouter 5'x12' table. 10hp Spindle motor is up to the job and then some. Gantry system same. Auto load tool. Vacuum table hold down. Torque is not an issue.

Cutting 6061-t6 1/4" & 1/8" plate.

Using a ("diamond like") coated 1/8" end mill 1/8" shank 3 flute 3/8" cutting length 3/8" protrusion from chuck. (Their spec's = 18k rpm 14 ipm 'not working')

Cutting out triangle and square shapes (mill cut) Perimeter cuts leaving 1/16 tabs on all sides to prevent dust vacuum from lifting parts after final cuts.

Getting very small chips. Approx 1/6" in length at 10k RPM 45 IPM .016 DOC 3.5 IPM plunge. Continuous air at bit with very fine tap fluid spray. 15 passes to cut 1/4"?? Driving me crazy watching something go that slow.

When I get to a 90 degree corner it's a guess whether bit breaks. So I exploded all my objects to single line cuts. Still get occasional breaks when cuts are diagonal to X-Y.

At this rate I'll be done in September because my table edge stop system is at +.75" and I have to use a 1" Z clearance setting. Up and down at 3.5ipm for every .016 cut. And I'll have $500 in bits. And the bit coating stops a good touch off for 0 'Z' so I have to paper set for Z every time I break a bit.

Any help is greatly appreciated. Thanks.

[peteeng]

Hi Dan - A couple of things a) a 1/8" bit is way too small and not stiff enough for what you are trying to do b) get a 1 flute 1/4" bit and life will be easier. A 3T bit has a very small gullet so has no room to evacuate chips. A 1F tool has a big gullet so has a better chance to fling the chip. Tools need to be sharp and clean for aluminium. Al loves to stick to a tool surface. Once it builds up a little its history as its attracts more material, looses its edge and gums up. Now to the cutting spec. The thing to check is the mm/tooth or chip loading as sometimes called. This is the thickness of the chip the tool takes every bite. This can be calculated using chip load (or thickness) = Feed/RPM/no of teeth. So in the 18000rpm/14ipm/3T case (I work in metric) its 18000/355mm/min/3T. So this is 0.006mm/tooth. This is very very thin and the tool is rubbing vs cutting. Look at the 10000/45ipm/3T case ie 10000/1143mm/min/3T is 0.038mm say 0.040mm or 0.0016". I usually start at 0.05mm but 0.04mm is good. But a 3T means its filling up the gullet. Try a 1T at 0.05mm so at 12000rpm/600mm/min/1T = 0.05mm. Surface speed could be a little high here but a sharp tool with good lubricant will work here. Peter

look up chip thickness once understood and you have a a figure that works for your machine stick to it! For timber try to make it bigger until it jams then back down. This will give you large clean chips that don't get recut and no rubbing. This will max your tool life. Peter

[machinehop5]

...2 Flute Carbide center cutting endmill with min flute for your depth of cut. No coatings. just good old Carbide from a Brand name Mfg. Also, tapping fluid is maybe not the best choice. Mobil 100 or equal type using spray mist best if, available. Run your Spindle Speed about 10k with Feed of about 60-80 IPM for the 1/4" EM. Which is about (.003-.004) Chipload. Ramping Z side to side to plunge also works good if, possible.

Good luck,
DJ

[Idbdan]

Hi Dan - A couple of things a) a 1/8" bit is way too small and not stiff enough for what you are trying to do b) get a 1 flute 1/4" bit and life will be easier. A 3T bit has a very small gullet so has no room to evacuate chips. A 1F tool has a big gullet so has a better chance to fling the chip. Tools need to be sharp and clean for aluminium. Al loves to stick to a tool surface. Once it builds up a little its history as its attracts more material, looses its edge and gums up. Now to the cutting spec. The thing to check is the mm/tooth or chip loading as sometimes called. This is the thickness of the chip the tool takes every bite. This can be calculated using chip load (or thickness) = Feed/RPM/no of teeth. So in the 18000rpm/14ipm/3T case (I work in metric) its 18000/355mm/min/3T. So this is 0.006mm/tooth. This is very very thin and the tool is rubbing vs cutting. Look at the 10000/45ipm/3T case ie 10000/1143mm/min/3T is 0.038mm say 0.040mm or 0.0016". I usually start at 0.05mm but 0.04mm is good. But a 3T means its filling up the gullet. Try a 1T at 0.05mm so at 12000rpm/600mm/min/1T = 0.05mm. Surface speed could be a little high here but a sharp tool with good lubricant will work here. Peter

look up chip thickness once understood and you have a a figure that works for your machine stick to it! For timber try to make it bigger until it jams then back down. This will give you large clean chips that don't get recut and no rubbing. This will max your tool life. Peter

Thank you very much!

I can't get decent quality 1T bits delivered quick enough to meet my completion time. Working this entire weekend to get it done.

You've been very helpful but I'm getting more lost than ever with going from 20 years of wood cutting to metal cutting. I believe I'm going to drudge thru this and pledge to never touch metal again. It appears it's become rocket science without reason? I started learning CNC with punched hole tape. CNC's complexity is ignoring the KISS policy now.

Thanks again!

[Idbdan]

...2 Flute Carbide center cutting endmill with min flute for your depth of cut. No coatings. just good old Carbide from a Brand name Mfg. Also, tapping fluid is maybe not the best choice. Mobil 100 or equal type using spray mist best if, available. Run your Spindle Speed about 10k with Feed of about 60-80 IPM for the 1/4" EM. Which is about (.003-.004) Chipload. Ramping Z side to side to plunge also works good if, possible.

Good luck,
DJ

I have a few new Whitestone carbide 2 flute up cut bits I use on MDF. Giving them a try in the morning. I've got to change all my nesting for 1/4" now. I have limited space for any increase in cut width on the blank size of the material I'm using. My nest was getting 95% usage. Hope it fits with the new cut width?

Is 'chipload' my DOC? .003 is going to take forever? And what would I use for the plunge rate? Been using 3.5 IPM.

From what you said this is what I see: 10K spindle RPM - 60 IPM Table Feed - DOC .003?? - Plunge rate ???

That's all the info I need to get started. Everything else is greek.

My zig zag plunge is doing strange things on this project. Must be the super slow plunge rate I'm using? The zig zag is starting at my clearance height and is going so slow I can barely see it. So I quit using it. The same happened when I applied ramping? How fast (IPM) can I plunge with zig zag or ramping? Right now at 3.5 IPM/2 degree a zig zag entry takes 55 seconds on every pass. And with a .016 cut that's 16 passes of "please shoot me" agony for every cut.

Thanks for taking the time to help. Greatly appreciated.

[Idbdan]

Went back to HMS to review my S&F this morning before I keep breaking bits and my bank account. Nothing is making good sense and breaking bits to find your speeds and feeds is a ridiculous concept. Found some seriously expensive bits today from a local machinist. First one broke on entry this morning.

Can someone please tell me what "axis" the "Speed" (red square) is referencing (see attachment)?? And in all the web calculators I've used, and my attempts to do the formula calc's myself, there's always an "unknown" that's not referenced 'SFM' or 'Cutting Speed'. SFM or Cutting Speed to me is table travel speed. And it's a designated number not a 400 to 1200 ... you take a guess figure.

RPM is self explanatory. Feed should be my x&y axis cut. And Plunge is self explanatory. Material hardness is a constant. So why isn't this a simple process??

And why is HMS giving me data that is not in line with what I'm getting from user suggestions?? IE.. 33k rpm when everyone is telling me 10 to 15k? 137IPM feed when that's also not what I'm being told? etc.

I'm almost at the point of paying the outrageous price I've been given to have these darn parts plasma cut.

[ToolHIT]

I'm sorry about all the issues you are having, not a fun time! Speeds and Feeds are generally all over the board as it is difficult to account for the rigidity of the setup as well as runout in the machine/holder from application to application. The End Mills you have should work great, the main issue is when you come into the 90 degree corner: you are doubling the engagement on the end mill at that point and an end mill as small as 1/8" Diameter usually breaks as it is too much tool pressure and there is nowhere for the chips to go. To solve this issue you need to cut your feed rate in half to reduce the pressure and allow time for chips to evacuate. Another option is to use a drill to drill out the corners before milling.

The rule for slotting is your Axial DOC should be 1/2 your tool diameter. So you should be at .0625" Axial DOC. Here are speeds/feeds I'd try:

Standard Speeds/Feeds:
Axial DOC: .0625"
SFM: 400-2,2200 (Start at 400)
RPM: 12,000
CLPT: .0008"
IPM: 28

Standard Speeds/Feeds:
Axial DOC: .0625"
SFM: 400-2,2200 (Start at 400)
RPM: 12,000
CLPT: .0004"
IPM: 14

The 400 SFM is very conservative, but you can always increase it (usually at around 800-1600 SFM in Aluminum). If you can drill out the corners that would help a ton. You also want to make sure your end mill is for Aluminum so there is extra room for chips to evacuate and in the 35-40 degree helix range (a 45 degree helix end mill is not as strong). Or you can even change to a 2 flute end mill for aluminum or go to a larger size if possible.

I hope this helps!

Mike

[peteeng]

Hi Dan - Chipload is not Depth of cut (DOC). CL is the thickness of material that each tooth cuts as it feeds. Feed speed is the velocity of the tool centre point and surface speed is the speed that the tool surface has (or the tooth tip velocity if you like). The faster the rpm the faster the SFM. As the SFM goes up friction goes up and either wear or coatings fail at some SFM. So each tool and tool coating has a recommended range of SFM. So 1) stay in the recommended SFM (surface feet per minute) range or below and use good lub to minimise friction. (your calculators will show SFM) Tool metal surfaces have high friction co-efficients and rubbing makes lots of heat. In aluminium this melts the AL and it sticks to the tool AL has very high surface friction. Once this occurs you lose the edge and it goes south from there. The lowest friction surfaces are diamond like coating (DLC) tools or PCD another diamond coating. These are 0.05 to 0.1 co-efficients. Other coatings are 0.3-0.4 or more so make 4x the heat 2) You are climb cutting and not conventional cutting? climbing is best as with conventional you tend to rub more as the chip is zero thickness at start of cut 3) Use a low DOC to start so tool load and chip clearing is maxed out. Use lub and an air blast to get chips out of the cut. Recutting chips again produces more friction more heat more galling - failure 4) If you dont think you are melting alum if you look at unlubbed cutting of steel the chips are red hot. Red is 650degC which is the melting point of al... thats one reason they flood cool mills 5) Too small a CL will produce rubbing, so start at say 0.025mm (0.001") 600/12000/2= 0.025mm or 0.001". try on scrap. Then go to 1200/12000/2=0.050mm or 0.002" then 1800/12000/2= 0.003" or 0.08mm CL... 6) now if it works on the straight you then have an issue in a corner as the CL increases in a tight corner. So you may have to halve the feed rate to compensate for the corner speed. Some controllers have an arc compensation function for this. When the tool goes in a straight line the tool center point (TCP) and the tool perimeter are travelling at the same velocity. When the tool goes around the corner this is not the case. The cutting edge speeds up so your chip load could double (or more) and then the tool fails. The velocity difference is the ratio of the TCP rad to the cut rad. So you will have to slow down in the corners via a controller setting or just go slow around the whole course. 500/12000/2=0.02mm 500/8000/2=0.03mm and in the corner this would be say 0.06mm CL so OK. Most CAMs slow down at corners but with curves same effect can happen. Peter

Chip Load: Guide for Beginners - MellowPine

https://youtu.be/zzzIpC39WUg