[rustybotak]

I need help since i got no experience in cutting sus. i got a part which is a mold. i start by cutting pocketing which i normally do with AL and my ball nose cutter flatten.The whole thing BURN!!!btw i use coolant.
Tool Dia=10mm
Flutes = 2
Stickout = 40mm
stepover = 1mm
RPM = 8000
cut depth =0.5mm
feed rate= 850mmpm

pls advice...

[rustybotak]

[txcncman]

RPM should be about 1200. Not 8000. Then recalculate your feed for that RPM.

[zero_divide]

Here is a calculation:
FSWizard

shortly for a 40mm long 10 mil dia uncoated 2 flute EM you should go:

RPM=1893, FEED=156.62mm/min
DOC=1.5mm, WOC=10mm

I would recommend a 4 flute tialn coated variable helix carbide EM.

[rustybotak]

so do i need to pre-drill or something?

[zero_divide]

so do i need to pre-drill or something?

No. You just cant pocket SS at 8000 RPM unless you are using thoroidal toolpaths, which is obviously not the case here.

Drop you Spindle speed to below 2000RPM and try this:
RPM=1893, FEED=156.62mm/min
DOC=1.5mm, WOC=10mm

Have no idea what tool you are using and coating so those speeds are for uncoated carbide.

[fizzissist]

I don't do metric unless I have to.... so you can do the conversions....

For a 10mm, or ~.40", I'd use a 3fl bullnose coated solid carbide.

You can run it easily at 275surface feet per minute, .002"/tooth chip load, and a 60% stepover. When doing a full width channel, keep the depth to less than 1/2 the diameter.

Use a good air blast, not coolant. Just get the chips out, and it'll be ok.

I've done hundreds of 304SS parts with 3/8, 1/2, and 3/4" solid endmills.... 3fl, from Dataflute or Helicall... Any of the good ones should do it for you.
... and don't use a ball nose... you'll just kill it.

[rustybotak]

ok thank alot guy...now that i know where is the the problem.i should have no problem. thx!!!! now i will go try it...

[fizzissist]

RPM should be about 1200. Not 8000. Then recalculate your feed for that RPM.

I'm coming up with a conservative starting point of 2400rpm and 14ipm on a 3 fl....
It's worked well for me in milling 304L with the cutters I've suggested.

[rustybotak]

I'm coming up with a conservative starting point of 2400rpm and 14ipm on a 3 fl....
It's worked well for me in milling 304L with the cutters I've suggested.

hi i need help again.....

i now cutting ss41 steel this time....need advice...
doing pocketing.....

dia 6 carbide coated wait TIALN = RPM 5000 FEED 500 ENGAGE 200 DEPTH 0.5 H=30MM
dia 3 carbide coated wait TIALN = RPM 10000 FEED 500 ENGAGE 200 DEPTH 0.3 H=30 L20
use oil base coolant ramp angle 3 deg
this is there anything i did wrong here because cutter wear super fast!!!

[txcncman]

Your RPM should be near 2000 and 4000 respectively. You are running RPM way too fast.

[rustybotak]

Your RPM should be near 2000 and 4000 respectively. You are running RPM way too fast.

btw im using 2 flutes cutter.... so u mean i should change my rpm to 2000 for dia 6, 4000 for dia 3?

[wizard]

Because stainless work hardens you need to keep the RPM to a minimal on your tooling and feed Fast enough to prevent rubbing the surface or having a flute cut the hardened surface. The surface will harden very quickly and if you hesitate may be difficult to penetrate with your end mills.

Second it is advisable to get a speeds and feeds calculator to help with beginning spindle speeds and feed rates. With stainless be conservative when it comes to spindle speeds.

Third it has already been mentioned but you need to keep the cutting area free of chips / swarf as the stainless chips are extremely hard. These hard chips will crack, chip and break end mills if recut. Thus the suggestion to blast the chips out of there. Cutter damage due to this problem is very serious with stainless steels.

Once a piece is damaged from work hardening it can be very difficult to save it. If the geometry allows it I've had success in the past for coming at the hardened area from the opposite direction. You may cut through the hardened area that way at the expense of an end mill, drill or whatever. If you are lucky. It is usually worth a try especially if you have to send the part out for annealing or need to have another cast. Which brings up another point, make sure the castings are annealed.

[rustybotak]

Because stainless work hardens you need to keep the RPM to a minimal on your tooling and feed Fast enough to prevent rubbing the surface or having a flute cut the hardened surface. The surface will harden very quickly and if you hesitate may be difficult to penetrate with your end mills.

Second it is advisable to get a speeds and feeds calculator to help with beginning spindle speeds and feed rates. With stainless be conservative when it comes to spindle speeds.

Third it has already been mentioned but you need to keep the cutting area free of chips / swarf as the stainless chips are extremely hard. These hard chips will crack, chip and break end mills if recut. Thus the suggestion to blast the chips out of there. Cutter damage due to this problem is very serious with stainless steels.

Once a piece is damaged from work hardening it can be very difficult to save it. If the geometry allows it I've had success in the past for coming at the hardened area from the opposite direction. You may cut through the hardened area that way at the expense of an end mill, drill or whatever. If you are lucky. It is usually worth a try especially if you have to send the part out for annealing or need to have another cast. Which brings up another point, make sure the castings are annealed.

so if now i need to cut stainless steel hole with a dia 1mm cutter what will be the best rpm and feed. i calculate around 12000rpm and 270 feed rate... DOC 0.1mm...is this alright?