newb talk, 2 flute vs 4 flute cutters

[DerHammer]

The 1/2 cutter is to profile the outer perimeter of my part which is roughly 11"x11". The 1/4 is for my inner slot milling/pocketing. The pockets are narrow. just barley larger than the 1/4 bit. The plate stock I'm working is 6061 aluminum about 3/4 inch thick. with the exception of the inner pocketing, its mostly rectangular movement being done.

Its pretty simple 2.5D stuff really, I'm just a little lost on where to start with the feeding speeds and depth per pass since I'm new to this. Even a conservative suggestion would be great because I could always bump the speed up later if its seems to be puring away. I just don't want to feed to fast or plunge too quickly and crash. Should I be as cautious as I am about or should I just see what happens?

Also, I've been doing some reading, can somebody enlighten me as to what SFM is as well as Doc? Seems like their should be some standard of how much stock should get removed per minute depending on various factors. Am I correct in assuming this? and if so, where do I find a chart with this data in it for various materials?

[dertsap]

http://metalworking.com/shareware.html

download machine zip ,its a neat lil prog to give an idea of how much force is on the tool

http://www.niagaracutter.com/techinf...eed/index.html
should give you a general idea as to speeds and feeds

[DerHammer]

thanks for the links dertsap, ill be sure to check em out

[Paul_S]

End Mills the feed is based on per flute cuts. So a 4 flute cutter can be ran faster than a 2 flute cutter. Type of material being cut and the type of cutting can also make a difference as to the number of flutes. In general use .003 per flute in a steel and .010 per flute in a light metal like alumium. And index this based on the diameter of the cutter. So a .25 dia cutter the feed per flute would be .003 x .25 = .0008 (.00075) per flute.

Also side cutting you would adjust the feed per flute by the sqr of the dia of the cutter divided by the side width of cut. So if the .250 dia cutter is taking .05 per side then the .0008 per flute becomes .0008 x sqr(.25/.05) = .0018 per flute.

Now finishing isn't per flute but per revolution. Yes, per revelution of the cutter. (Unless you have holder and tool runout less than the finish you want per revelution.) So the number of flutes 2, 4 or 6 makes little differnence (except for along the length z depth of the cut can be better with more flutes. But no better than the finish on the edge of the tool.)

For peripheral AA finish use .0405 x sqr(tool dia) x sqr(finish / 125 ) = ipr.
For the ID adjustment, linear ipr x sqr(( id - tool dia) / id) = id ipr.
For the OD adjustment, linear ipr x sqr(( od + tool dia) / od) = od ipr.

[fpworks]

...So a 4 flute cutter can be ran faster than a 2 flute cutter...

Good advise overall, but this statement is not true for roughing aluminum. A two flute tool can be fed FAR faster than a four flute endmill in any geometry when roughing aluminum.

That is, unless you're talking about large indexable cutters, then you are correct.

[DerHammer]

Ok, So I have searched through several sites now with various calculators on them and I still have the same question I did when I first started. All of the calculators seem to be a basic simple triangular formula, which can be manipulated to solve for any of the 3 variables. Now, This is awesome if you have two of the three variables but what if your like me... and you don't know any of them or maybe just one.

Like for instance, you can calculate Rpm if you have your cutter dia and SFM. In this case, of course I know my cutter Dia but I don't know my SFM or my RPM so this formula is no good unless I know one more bit of info. Can somebody tell me what I'm not understanding? Someone start at the basics for me plz

[Cory]

Ok, So I have searched through several sites now with various calculators on them and I still have the same question I did when I first started. All of the calculators seem to be a basic simple triangular formula, which can be manipulated to solve for any of the 3 variables. Now, This is awesome if you have two of the three variables but what if your like me... and you don't know any of them or maybe just one.

Like for instance, you can calculate Rpm if you have your cutter dia and SFM. In this case, of course I know my cutter Dia but I don't know my SFM or my RPM so this formula is no good unless I know one more bit of info. Can somebody tell me what I'm not understanding? Someone start at the basics for me plz

The two values you want to start with are cutter diameter and SFM. SFM can be found in the machinist's handbook, or on many online sites. Your best bet is to find your cutter manufacturer's website. Most should have feed and speed charts where they will list the reccomended SFM and chip load for various materials and cutting situations (profiling, slotting, etc).

From there you have everything you need to calculate RPM (4*SFM/Diameter) and IPM (Chipload*flutes*RPM)

[DerHammer]

I figured there had to be something that I was missing, Is there a general chart listing for finding your SFM for standard mill sizes by chance. I have some no-name brand stuff I got from enco.

does anybody happen to have a website for the SFM ratings for various sized, two and four flute end mills. I'm pretty sure mine are just plain standard center cutting end mills, nothing special.

[Cory]

I figured there had to be something that I was missing, Is there a general chart listing for finding your SFM for standard mill sizes by chance. I have some no-name brand stuff I got from enco.

does anybody happen to have a website for the SFM ratings for various sized, two and four flute end mills. I'm pretty sure mine are just plain standard center cutting end mills, nothing special.

SFM should vary only based on the material of your cutting tool, and the material you're cutting. It should stay constant regardless of end mill size.

I have a decent number of Niagara cutters, and I've found their speeds and feeds to work well for me. You can find a lot of info on their site, here.

What will vary with the size of your end mill will be chip load. Bigger end mill, higher chipload.

[dertsap]

I figured there had to be something that I was missing, Is there a general chart listing for finding your SFM for standard mill sizes by chance. I have some no-name brand stuff I got from enco.

does anybody happen to have a website for the SFM ratings for various sized, two and four flute end mills. I'm pretty sure mine are just plain standard center cutting end mills, nothing special.

you should be able to find all the info you need from the niagra link i posted , you may have to search around their site some but it should answer your questions

[DerHammer]

Thanks for the links. Is FPT (feed per tooth) the same as IPT, which I am assuming means (Inch per tooth)?

[Paul_S]

Thanks for the links. Is FPT (feed per tooth) the same as IPT, which I am assuming means (Inch per tooth)?

Yes, if the feed is in inches. In metric [which I don't use], feed per tooth is MMPT (millimeters per tooth.)

[SFPM (Surface Feet Per Minute) is used to calculate RPM using feet to inches, diameter to circumference calculations.

SMPM or SMM (Surface Meters per Minute) is used to calculate RPM using meters to millimeters, diameter to circumference calculations. Metric.]

[SORCHEROR]

if your cutting aluminum i use 3 flute data flute high helix endmills,i rough and finish with the same dam endmill,those thing are industructable and fly thru like butter,i run 4500 rpms at 60 imps .400 a pass to rough the chips are like at terminal velocity when coming out,the trick to aluminum is uncoated endmills with good coolant flood,coated endmills the alum. will stick to it and build up,if you have 2 + 4 flutes only than i prefer 2 flute to rough and one slow pass with 4 flute to finish,sometimes the 2 will do both

[DerHammer]

thanks for input, I'm doing a relatively small production type run and I don't have an ATC mill, so its important to me to reduce the number of tool changes I need to do. Basically I'm attempting to cycle say 20 parts, tool change and then recycle. Since this is the case, I'm trying to finish with my two flute also and so far its been decent. It doesn't look polished or anything after the cut, but it seems to feel very smooth so I'm happy. I'm currently feeding my tin coated 1/2 at 36IPM and about 3600 RPM which is all my old clinker has in it for the spindle. I would love to feed faster but I don't have anymore RPM left in it. I'm also taking off about .125 per pass.

[gibbsman]

For roughing 2-3 flutes for sure but for finishing the more flutes the better as long as you can get the proper amount of chip evacuation.

[Paul_S]

For roughing 2-3 flutes for sure but for finishing the more flutes the better as long as you can get the proper amount of chip evacuation.

If you run your cutters real slow for finishing, it can make an improvement along the Z length of the cut of the end mill.

Finish cuts are per revolution of the cutters. Really. A 6 flute 3/4 end mill at 3000 RPM at 41.56 IPM and faster feeds, will give you the same finish as a 2 flute 3/4 end mill. Only end cutting (not periphery) will the 6 flute give you the better finish.

[DerHammer]

So I've been doing some experimenting with various end mills while cutting my aluminum and what I've found so far is that I seem to be breaking the smaller bits quite more than I would like. I like to use smaller cutters (around 1/4 inch) because it allows me to cut the entire part with one tool, but the outer profiling seems to be putting on allot of millage on that little bit. Once I'm a few parts deep the cutter breaks. So, my question is whether or not there is any cost effective advantage of going with a Carbide or cobalt end mill over HSS when doing only aluminum or should I just eat the cutter cost on the cheap bits and buy a surplus of them.

[fpworks]

...my question is whether or not there is any cost effective advantage of going with a Carbide or cobalt end mill over HSS when doing only aluminum or should I just eat the cutter cost on the cheap bits and buy a surplus of them.

Spend the money on the tools. FWIW, I avoid HSS endmills for aluminum cutting. A typical exception for me is custom ground form cutters, which are quite a bit cheaper in HSS vs carbide, especially if the usage is low. (like $200 vs $400 for one tool)

At any rate, you still shouldn't be breaking your tools. I suspect a problem with your cutting parameters. It would really help if we knew more about your application, such as the following:

DETAILED tool description:
--Brand & Series:
--Coating:
--Cutting diameter:
--Shank diameter:
--Flute length:
--Overall length:
--Number of flutes:
Length of tool protruding from spindle:
Tool runout, in spindle:
Tool clamping method:
Spindle speed:
Feed rate:
Operation type:
Axial depth of cut:
Radial depth of cut:
Coolant type:
Coolant pressure and flow rate:
Workholding situation: (post picture)
Toolpath geometry: (post screenshot from your CAM, and/or your g-code)

This is right off the top of my head, so I may have left out some things. But ANY one or combination of the above could be causing your problems, so please try to answer everything.

Justin

[JROM]

Out here in the real world three flute carbide endmills are the only way to go when cutting alu. They run faster, balance better, and live longer.
Forget about HSS unless you are a hobbyest, if so putter away!

[Paul_S]

If your breaking smaller end mills sooner than the larger end mill, try indexing your cuts.

For example: If you are using .007 ipt on a two flute 1/2 end mill then your index for the flute per cut is .014. index value = ipt / tool dia. So a 1/4 inch end mill would be .0035 ipt = .014 x .25.

You can also index your cubic inch removal rate. CIPM index = cipm / (dia ^5 / (cutter lenght of cut) ^3)*. So your new cubic in per minute remove rate with a different size cutter would be = CIPM index x dia^5 / (cutter length of cut)^3. And this can be maximized by using (cutter length of cut - z depth of cut)^3 instead. Generally I use 1/2 the z depth of cut instead of the full depth of z cut for the calculation. This miniumizes tool breakage using much smaller cutters and longer cutters. (With longer cutters chatter can be another issue.)

*Also the maximum cipm index is simply CIPM = cipm / dia ^2. If the value of dia^5/(length)^3 is greater than dia^2 use the dia^2 value.