.020" carbide endmill, .100" slot-316 ss-HELP

landm1 · Feb 14, 2018

Hello,

We are making a .020" wide, .100" deep slot in 316 stainless. We have access to a nice 12,000 rpm spindle.

Any ideas for speeds and feeds? The end mill will have to be a bull nose, the bottom has radiuses on the sides and a slight flat bottom.

Type of end mill:

Speed:

Feed:

Depth of cut:

We probably have to do about 3" total, four of five slots, .7" each, so the tool has to hold up, we can feed down mostly in air.

Milland · Feb 14, 2018

Use this style of cutter to rough as much material away as possible: Harvey Tool - Carbide Miniature End Mills - Square Long Reach, Stub Flute Ramp in, don't plunge. Do everything you can to ensure chips are flushed immediately from the cut zone. Be certain the tip of the cutter is running true, as close to perfect as you can get.

If you really need a .020 slot you should be using a .018 cutter to avoid rubbing on the conventional side. If you can finesse the geometry to allow a .022 final slot width stay with the .020 cutter.

Change out cutters before they dull, don't allow the cutter to stay stationary against the metal. You want to avoid work hardening.

If the machine is older or hasn't been maintained well you might want to confirm current backlash settings are good. If there's excess mechanical play in the ways you could have issues with finish or even snapping cutters.

For speeds and feeds do some test cuts on a scrap piece of the same material as the final parts. You can use the tool vendor's recommendations to start, adjust for type of coolant or air blast you'll be using.

pmack · Feb 15, 2018

If both ends of the slot are open to the air, turn it 90 degrees and use a jewelers slitting saw. If not, here is what I would try. I would probably buy a slightly undersized tool from a company that does quite a bit of miniatures such as Harvey tool. Feeds and speeds recommended by the manufacturer. Tool run out needs to be kept to the bare minimum. Ramp down back and forth in the center of the slot not exceeding about 10-20% of the cutting tool diameter for each ramp pass until you are at final depth instead of cutting in steps. Then ramp the perimeter finishing to size. You need to clear the chips effectively too with preferably high pressure thru spindle coolant or air blast. Very minimal deflection will break the tool. At 12k it will be painfully slow, a spindle speeder would be nice.

pmack · Feb 15, 2018

Milland said:
Use this style of cutter to rough as much material away as possible: Harvey Tool - Carbide Miniature End Mills - Square Long Reach, Stub Flute Ramp in, don't plunge. Do everything you can to ensure chips are flushed immediately from the cut zone. Be certain the tip of the cutter is running true, as close to perfect as you can get.

If you really need a .020 slot you should be using a .018 cutter to avoid rubbing on the conventional side. If you can finesse the geometry to allow a .022 final slot width stay with the .020 cutter.

Change out cutters before they dull, don't allow the cutter to stay stationary against the metal. You want to avoid work hardening.

If the machine is older or hasn't been maintained well you might want to confirm current backlash settings are good. If there's excess mechanical play in the ways you could have issues with finish or even snapping cutters.

For speeds and feeds do some test cuts on a scrap piece of the same material as the final parts. You can use the tool vendor's recommendations to start, adjust for type of coolant or air blast you'll be using.

What he said! I type too slowly.

White Lightning · Feb 15, 2018

In hard milling I will often use a ball cutter to rough with then finish with a bull cutter. The corners often will break down on the bull cutter faster leading to failure over roughing with the ball.

Sent from my XT1585 using Tapatalk

White Lightning · Feb 15, 2018

I know 316 ss is not hard just my 2 cents

Sent from my XT1585 using Tapatalk

SteveEx30 · Feb 15, 2018

Cutter: Any .5MM Ball, 3MM REACH

RPM: 12000 RPM
Feed: 5-7"/Min
DOC: 0.0008"

Be sure to blast coolant. Ramp into cut as someone else mentioned.

If the slot doesn't break out on the ends, I would draft the ends, because that's most likely where you will break cutters. Hopefully the machine is tight!

AARONT · Feb 15, 2018

pmack said:
If both ends of the slot are open to the air, turn it 90 degrees and use a jewelers slitting saw...

If this is an option, I would go this route. If not, Milland is spot on.

sneebot · Feb 15, 2018

I had to do a similar slot in 303 recently-- but I was using a 0.015" end mill with a 0.093 reach. Like Milland suggests I was using a Harvey end mill. I called them up and verified feeds and speeds based on the charts they have on their web-site- they are quite helpful. The slots I was cutting took ~3hrs per part.

Milland · Feb 15, 2018

sneebot said:
I had to do a similar slot in 303 recently-- but I was using a 0.015" end mill with a 0.093 reach. Like Milland suggests I was using a Harvey end mill. I called them up and verified feeds and speeds based on the charts they have on their web-site- they are quite helpful. The slots I was cutting took ~3hrs per part.

Hiya Sneebot,
Harvey is great for fast access to small cutters, and they have a broad range of geometries. I usually mention them when such jobs come around. But if I'm doing tricky work in harder or tougher materials (and I have the budget) I look at higher-end tools like from Mikron.

To our Aland Islander, 316 is usually not hard (can be work hardened), but it is tough and should be respected when dealing with small cutters. When the chips are stringy and fairly hard they'll take the flutes off a small tool quickly if not flushed out properly.

2outof3 · Feb 15, 2018

Any chance you can turn the part on it's side and use a Robbjack saw?

Milland · Feb 15, 2018

2outof3 said:
Any chance you can turn the part on it's side and use a Robbjack saw?

Even easier, just sub it out to a shop on the equator...

pmack · Feb 15, 2018

You may want to consider subbing to a shop with a sinker EDM too.

hanermo · Feb 15, 2018

Why not drill the end or ends ?
Or perhaps most of the body of the slot.

I may be all wrong on this, but ...

sneebot · Feb 15, 2018

Milland said:
Hiya Sneebot,
Harvey is great for fast access to small cutters, and they have a broad range of geometries. I usually mention them when such jobs come around. But if I'm doing tricky work in harder or tougher materials (and I have the budget) I look at higher-end tools like from Mikron.

To our Aland Islander, 316 is usually not hard (can be work hardened), but it is tough and should be respected when dealing with small cutters. When the chips are stringy and fairly hard they'll take the flutes off a small tool quickly if not flushed out properly.

I'll have to look into the Mikron tools-- where do you usually purchase?

Milland · Feb 15, 2018

sneebot said:
I'll have to look into the Mikron tools-- where do you usually purchase?

These are the companies repping Mikron in MA: find your Mikron Tool Sales Partners- Worldwide

[You may have to fill in Country and State again]

I've got no specific preference (outside of not MSC), and you may be better off choosing a NH company to save on sales tax (can't remember if you'll have to pay MA sales tax anyway).

landm1 · Feb 15, 2018

pmack said:
If both ends of the slot are open to the air, turn it 90 degrees and use a jewelers slitting saw. If not, here is what I would try. I would probably buy a slightly undersized tool from a company that does quite a bit of miniatures such as Harvey tool. Feeds and speeds recommended by the manufacturer. Tool run out needs to be kept to the bare minimum. Ramp down back and forth in the center of the slot not exceeding about 10-20% of the cutting tool diameter for each ramp pass until you are at final depth instead of cutting in steps. Then ramp the perimeter finishing to size. You need to clear the chips effectively too with preferably high pressure thru spindle coolant or air blast. Very minimal deflection will break the tool. At 12k it will be painfully slow, a spindle speeder would be nice.

Sorry, hardly a right angle on the part, saw is out!

landm1 · Feb 15, 2018

Thank you people, I really appreciate it,

The ball end mill for rough was a new one for me. Saw is out, no right angles on the part. Micro came out with a through spindle/tool coolant down to .3mm endmills, 1/8 shank. anybody used one yet?
Our machine has a Mazak spindle and is a tight machine with through spindle coolant. We are using Esprit cam so we have a lot of options for feeding in but I think we should be able to feed down in air.

Milland · Feb 15, 2018

I'll respect those that have made ball endmills work,, but to me the poor cutting action near the center of the tool doesn't make sense for applications like this. Especially when dealing with a work hardening material, I don't want a form the rubs with a near solid, slow SFM center.

My ideal rougher would be a slight corner radius, short flute, solid shank of whatever length (but short as possible) to get the material out, then finish as needed.

White Lightning · Feb 15, 2018

Milland said:
I'll respect those that have made ball endmills work,, but to me the poor cutting action near the center of the tool doesn't make sense for applications like this. Especially when dealing with a work hardening material, I don't want a form the rubs with a near solid, slow SFM center.

My ideal rougher would be a slight corner radius, short flute, solid shank of whatever length (but short as possible) to get the material out, then finish as needed.

I haven't machined a lot of 316 ss but I have machined miles of small ribs " slots" in 30 plus years of mold making. I've found ball cutter are the best method if cutting ribs. The problem with small corner radius cutters the corner is the first thing to wear out causing the cutter to push hard making it lean in which makes the flute to dig into the floor which makes it grab and break or machine over size on the width. A ball cutter will hold it's edge better, track straight and can't dig in and break because of not gaining length when leaning. I'm not concerned about work hardening when these cutters will hold up to 60 rc hard tool steel. It's not like drilling. Lots of coolant or even better oil mist. Then pick the floor out with a corner radius cutter. Good luck!!

Sent from my XT1585 using Tapatalk

.020" carbide endmill, .100" slot-316 ss-HELP

Cast Iron

Diamond

Cast Iron

Cast Iron

Aluminum

Aluminum

Stainless

Stainless

Stainless

Diamond

Titanium

Diamond

Cast Iron

Titanium

Stainless

Diamond

Cast Iron

Cast Iron

Diamond

Aluminum

Similar threads