[orion_134]

The part is a handgun slide with a surface-hardened Melonite coating. I am machining a 1/4" pocket (with 1/16" radius corners) and was hoping to run a pocket with the 1/8" tool. I'm manually adding Tapmatic while trying my best to keep the chips clear. I first tried an 1/8" 3 flute carbide at 768 rpm and 1.4 feed (0.000625 IPT), .48 plunge and it snapped on the plunge. After exhausting my only carbide tool I switched to a HSS 4 flute and a toolpath that ramps to depth using same specs but a 1.9 IPM feed (using the same 0.48 IPM feed during the ramp). It trashed the face of the end mill after the first 1.5" of cut.

So...where did I go wrong?
1) Is my feed/speed calculator off? I usually drop sfm/rpm by 60% because I'm manually adding oil, should I be doing the same on something moving this slow (and has such a high risk for work-hardening)?
2) I realized that I ran the carbide at HSS feed/speed. Is that a problem? Does it NEED to be ran like a carbide?
3) I fear that I'm getting some work hardening. Should I be using plunge rate or feed rate during the ramp?
4) What kind of chipload should I be seeing?

I have already done some machining on this slide, but I had the luxury of endmilling in at depth and not plunging. This cut is obligated to plunge.

So my work-around was to buy a 15/64" end mill to plunge as beefy of an endmill as I can in to rough it, then finish the cut with the 1/8" so it enters the cut at depth. It will be here tomorrow.

What do y'all think?

[newman55598]

Not sure about the melonite but for cold roll steel your plunge rate is way to high. Try 2383 rpm and feed per tooth of .0028 = 20.02 ipm for the plunge try .0014 and that will be 10 ipm. If you can't run your spindle that high here are the calcs for 768 rpm. Fpt .0028 ipm =6.45ipm Plunge .0014 fpt = 3.23 ipm

[orion_134]

It's a Haas GR-510, it can do it. Maybe I didn't clarify, 0.48 IPM on plunge. You want me to do 10 IPM on plunge?

[newman55598]

Like I said I'm not sure how the melonite affects the situation. For just 1018 steel my calculator (Bobcad) recommends 78sfm with .0028 fpt for cutting and .0014 fpt for plunge at 2383 rpm that comes out to 20.02 feed for cutting and 10.01 for plunge. Are you getting chips or just fine dust with your current feeds? I'm thinking that you are cutting to slow and work harding the piece. These speeds are for hss.

[orion_134]

Thanks for the quick responses!

It's ok to run the carbide like a HSS tool? The Melonite apparently takes the first 0.020" to a 68 Rockwell. The first cut sucks the most, then when it's being cut by the flutes it chips off.

[newman55598]

That's a good question. I believe that you can use the speeds for hss on carbide as the advantage to carbide is being able to run higher speeds. I'm sure there are lot of people on here with a great deal more experience then I that would be able to answer that better. I run hss normally because of the cheaper price and my spindle only goes to 6000. So there wouldn't be a huge advantage for me until you got into the bigger cutters. For example the recommended speeds for a 1/8in carbide is 600sfm 18335rpm at 154 cutting and 77 plunge feed rate. With the chip load being the same as the hss.

[newman55598]

Another thing with carbide is if you have any vibration ie poor work holding or an in-ridged mill it will destroy the cutter quickly.

[acannell]

heres some things that would help your machining operation:

increase the radius of the corners
if you must keep the small radius corners, drill the corners with a small radius drill and use a larger radius tool for the rest of the pocket
use a bigger end mill
drill entry holes instead of attempting to plunge them with an endmill
avoid plunging an end mill into this hard to machine material
if possible, practice on this material using a larger endmill to get a feel for how it responds to various chiploads and surface speeds

[diamond.3211]

For a plunging cut you need to slow down the IPM's those F&S's may work for milling but for plunging I would drop it down to around .3 IPM and increase to 2000 RPM. Maybe peck so that you can get that Tapmatic down in the cut. If you have to plunge, why not drill out sections then follow with an endmill to clean up the uncut areas.

[orion_134]

Should I be reducing speeds/feeds like I do in aluminum because I'm manually adding oil and air instead of flooding/misting?

[acannell]

Should I be reducing speeds/feeds like I do in aluminum because I'm manually adding oil and air instead of flooding/misting?

dont worry about that. this is micromanaging this operation when you need to be focusing on the major factors that impact the cut.