Cutter Depth

[grantmi1]

I am using thru the spindle coolant at 400psi and a walkasa carbide insert cutter at 1" 4 flute. I am told that the sfm 250 and chipload is .005". How does this relate to depth what depth would you guys run at. Do you adjust the rpm for different depth of cuts or just leave rpm alone.

I am cutting unhardened 420 stainless.

[GOMEZ107]

grantmi1,
My experience is with Ingersoll cutting tools. Based in that I used 1250 rpm,20 ipm feed, and .300 depth 75% diameter.
If I remember correct material was 4140. I know is a lot different than 420, but I get those numbers from the Ingersoll salesman
any chance you can call the sales dept. from walkasa?.

GOMEZ107

[grantmi1]

Thank you for your input, I called Waukesha and they gave me 1850rpm and 7ipm at .250" of cut.

[hardmill]

250sfm may even be a little conservative
Especially w/ thru spindle coolant. see what
happens since thats what they recommend.
Make sure and post to let us know what happens.
Peace

[grantmi1]

I appreciate that info, I am going to run tests over the weekend or on a friday, since we work 4 1o hour days and are closed on fridays. I will use you as a reference.

Sorry about the short phone call yesterday, I had someone waiting for me to send them program. We are working on a real hot job right now. Did you say that you teach CamWorks? Or CamMill. I have more questions that I cant remeber right now. Feel free to call anytime.

[grantmi1]

I don't get it so I got some feeds and speeds from a cutter comapny and it reads like this.

0.250 ball endmill 4 flute
.300" total depth of pocket
3.5" diameter of pocket
3000 rpm
.006" stepover
.250" depth of cut

That just seems slow and awfully deep to me.

[grantmi1]

I took a Velocitytool (velocitytool.com) TA2 series cutter a .250" 4 flute carbide cutter at .032 depth of cut and 3500rpm with 40% stepover at 40ipm and the damn cutter started glowing. It was ruined. I was cutting 420 stainless that was not hardened.

[HuFlungDung]

I've had zero experience machining 420 stainless, but I have machined a bit of 316 and 304.

The heat builds up in the chip and the stuff has quite an affinity for welding itself to the tool, even a simple drill bit cannot be "rushed along" in stainless.

I think your feedrate is about 4 times too high. Another thing about a ball mill, is if you are using the bottom side of it, there is often not great rake available for the cutting face of the flute, and this makes it a b!tch to get the chip out of there, and another reason you cannot feed it hard.

I'd try a two flute, just for the fact that there is a little more room to work on grinding the flute and even grind a bit more rake face if necessary. I guess that destroys any coating the face had, but what else can you do?

[hardmill]

Now that i know who you really are MIKE.
For some reason it did'nt click until i talked
to Dale awile ago. What your going to need is
a Mill that looks like this. Its a 6 flute cutter made
for High speed and hard milling.

You can go w/ about 3x's dia. depth of cut, step
over 5-7%.

[grantmi1]

This is a lens type cavity, would it still be the same type of cutter. Picture the face of a large spa light for hot tubs or even a pool light.

[hardmill]

the company i was at made lens molds for Oakley.
This is going to fun for us both.

PEACE

Perfect meaning i can show you how to apply different
tecniques to hard machine your project.

[Paul_S]

Estimating feeds and speeds is always of great interest to me. Since typically I am on my own trying to decide what is best. Currently I have to machine some D2 air harding tool steel. The program has not been ran as of yet.

From a starting point for surface speed I use the recommened SFPM from the 19th edition of the Machinery Handbook. At home here, I only have my 26th edition. And it does not provided the tradtional SFPM for carbide, only HSS. But has so-called tool life tables which does include for carbide end milling.

So from the HSS table for 420 gives SFPM 95 for 135-175 Brinell which would be the annealed condition.

Since I typically use SFPM 70 for 303. And the book recommends 100 SFPM. I would use 60 to 66 SFPM for 420 to start.
And since I use 225 for Carbide using 303 I would choose 150-180 for 420. Now just guessing. and estimating.

I would use .003 per flute index value for the cutter feed. (I use .004 index for 303.)

So if I was to calculate the feed for 1/4 carbide ball em 4 flute.
.003 x .250 x 4 x RPM.

My max RPM using 180 SFPM. Calculates out to 2750 RPM.
The roughing feed would be 8.25 IPM. If I am side cutting with a step over of lets say .008 per pass I would up my next and remaining feeds to 46.11 IPM (IPM = ref IPM * sqr(.25/.008).) But I would check this against another program that I have written depending the flute length of the cutter and depth of cut given the dia of the cutter. I don't want to break the cutter. That program recommened 17.62 IPM using a chip load of .0003. And my starting feed would be more like 3.3 IPM.

(giving the flute length of about .85, z axial depth of .5 roughing with a side cut of .008 step per pass.)

My finish feeds though can be much faster for spring cut finish clean up. Using a .008 finish step over the feed would be typically .008 * RPM > 22. IPM.

Summery. My first estimate might work. But I do not want to break my cutter. So I go with the more conservative estimate. (Using an experimetal algorithm which I have been using with generally good results for the past few years.)

Checking another earler (now modified) program that I have suggests a reduced RPM of 1790 (a reduced 117 SFPM) with a feed rate of 18.49 IPM with the .008 step over during rough out. I would be inclined to use these values because the feed is higher here. 18.49 IPM. The index chip load being .00046. The lower RPM giving better tool life (even though it is more of a HSS SFPM range.)

The programs are written in TI-BASIC on a TI-86 programmable calculator.

Then kick up the RPM to 2750 for finishing at the 22. IPM.

Anyway I would also be inclined also to use a HSS/Cobalt roughing cutter to take out most of the material first before roughing and finishing with a 1/4 ball.

But only if it looked like it would give me shorter maching time over all. It depends on how mach material must be roughed out.