feeds and speeds

[lito]

i really need help with speeds and feeds. i've been machining for 8 years now and i have only taken up an entry level trades training. when i started working, there was no machinist employed so i had to learn by trial and error. my problem is when milling , my endmills don't last very long. i use carbide endmills and i mill steel and stainless steel. after 2 or 3 cuts, either the endmill has broken or has chipped its edges. the machines i operate are all CNC's. i've tried the formula CS x 4/DIA. and rpm x IPT x no. of teeth, but i still keep getting these problems. We do mostly R&D work. just this afternoon, i was flycutting a 3/4 thick 6 x 10 steel plate, cutting .070 depth. after 2 passes, the inserts have chipped. Is there a rule that I can use to calculate speeds and feeds, and depth of cut. i think it's the depth of cut and the corresponding feed that really stumps me.

[Ken_Shea]

Lito,

Here is a link to ME Consultant, I think it is still free but he is just now upgrading to a Pro version that he will be selling, I have used them both and find the Pro version has much needed enhancements.

Do your self a favor and get it, when the Pro version is released purchase it.

http://www.mrainey.freeservers.com/

[lito]

thanks ken. i will try it

[Paul_S]

Hmm... I had to cut some slots in a 1.00 steel plate for tooling, the spindle horse power was 15hp. I was using a 3/4 rouging end mill. The machine didn't flinch. After about an 1.00 of travel the tool broke. Hmm... This changed how I approched my feeds and speeds.

I look at unit horse power per cubic inch per minute. I assign values to my tools based on dia and length. Dia based in the square of the dia. And length based in the cube of the length. The formula I use is not in any book. dia^5/length^3. And the limit not to be more than dia^2. (i.e. The tool length not calculated for shorter than the tool dia.)

I also look the unit horse power as to what is available at the spindle at a given RPM. If you exceed this you will break a tool too. Mess up the setup. And worse yet damge the machine tool.

Inches per minute x width of cut x depth of cut. CIPM (Cubic inches per minute) unit hp per cubic inches = hp / CIPM, or K value = CIPM/hp
(These unites are some time inversed.)

I use CIPM/hp. .5 for steels in general, .7 for 303 CRES, 3. for aluminum. It is approximate, but works.

Index chip size. .003 x dia of the tool for steel. .004 x dia of the tool for 303 CRES, .010 x dia of the tool for Aluminum.

Want a formula to estimate this? .0048 times the 1 1/2 root of the cubic inch per minute per horse power. .0048 x (K)^(1/1.5) for the tool chip index value.

So a feed rate IPM would be, index value x dia x number of flutes x RPM.

If a full width of the cutter is not being used, I increase my feed by square root of the dia of the tool divided by the side width of cut.
IPM = index x dia x number of flutes x RPM x sqr(dia / width)


More on indexing your feed rates. If you know 1/2 carbide cutter works fine at .0025 chip load at half the cutter dia and at the cutter dia depth for a given material. You can index for other size carbide cutters from this. And keep a record for future reference.

The index value becomes, index = known inch per flute x sqr(width/ dia)/dia. The z axial depth of cut being the same to the dia of the cutter. Index the z depth too. So if the 1/2 cutter is 1/2 deep, a 1/4 cutter indexed feed would be to 1/4 depth and so on.

Now you can apply this to any size carbide cutter in that material.

A different depth? New IPM = Old IPM x ((lenght of cut-new depth of cut)^3/(length of cut- old depth of cut)^3). But the CIPM must be the same or less. Check it. If the new CIPM is more, reduce the feed to the old CIPM. CIPM = width x depth x IPM.

Carbide cutters even though they are 3 x tougher than HSS - do not push them more than 1 & 1/2 times. Also if the cutter is to change direction in the cut, use a dwell between changes in direction, not to snap the cutter. One to two revolutions of dwell should do the trick. Dwell time = seconds per minute divided by RPM. More than three revolutions may also reduce tool life. The dwell is just to clean out hanging chips that can hold on to the tool when the tool changes directions, so not to pull and break the tool.

I hope this is of some help.

[DareBee]

Also, as a general rule of thumb, if your cutters are chipping your feedrate is too high and if your cutters are prematurely wearing the edge dull your feedrate is too low.
What chipload where you running these tools at.