Tiny Endmills

I need to make a tiny slot 0.050 deep 0.050 wide 0.1 long

I have a 40 taper CNC machine It's supposed to have a 10k spindle but it seems to start to vibrate around 6k and even up to around 8500 it's not too bad but makes a bit of a hum which I'm sure isn't good for delicate end mills. I'm not sure if that's the issue or it's my feeds and speeds the tool is held in a shrink-fit holder probably can't do much better for runout.

I'm using a stubby little 1mm (0.040) 4 flute center cutting carbide end mill. I've broken two already and haven't made much progress. the material is 17-4 stainless. I'm taking 0.0003 per tooth trying to ramp into the material at a 3-degree angle just milling back and forth while raming down. I had the RPMs at 8k. so that recipe definitely doesn't work. Barely made a scratch.

I'm wondering what parameters I should start tweaking, I really don't know another toolpath to accomplish what I'm trying to do maybe plunge straight into the material and cut across. It's full engagement which I know ideally I would be taking a small radial. Also, everything being equal can I slow the spindle down to around 5k and run slower, so I can be sure the vibration isn't a factor? I know these little cutters are most efficient as far as material removal at a certain SFM but I can run it slower right?

What can I do to make these end mills live a little longer? Please help.

Typically a humming sound as the rpms increase are a sign of the tool not being balanced. I would probably drill the slot out and keep the tip 2 or 3 thou shallow of the bottom to remove the majority of the material then zigzag the endmill down in small steps like 2-3 thou to get the slot to depth then finish the walls with another constant ramp. You could plunge the center of the slot out after drilling but would have to be light on it. As far as rpm, I would worry too much if you only run 5k. Probably drop your feed to 0.00015 per flute to start.

I made this mold hot stamp part with a cheap 50 watt fiber laser from Amazon the depth was .06 the part about 2 inch diameter took about 5 hours to get to the final depth sure was easy to do
Don


Sent from my iPhone using Tapatalk Pro

D Nelson said:

I made this mold hot stamp part with a cheap 50 watt fiber laser from Amazon the depth was .06 the part about 2 inch diameter took about 5 hours to get to the final depth

Click to expand...

Material and part size.?
Was focusing z needed? Draft on sides?
Moving or fixed laser and part?

It helps to have a small precision mill for doing small precision parts. My Derbyshire Micromill was built around 1945, but I finished rebuilding it and converting it to vertical a few years ago. The collet will hold up to 8 mm shank end mills and the spindle is driven by a brushless DC motor up to about 8000 RPM. I have lathes that use the same collets that are great for small turning jobs. That is actually a re-purposed lathe headstock on the mill.

The pictures show it cutting a .050" keyway in 12L14 with a HS end mill. The two bushings were turned on a Hardinge lathe with 5C collet spindle. I know 12L14 steel is easier to cut than stainless, but my mill would probably cope with milling stainless. Just turning a couple cranks seems a lot easier than worrying over programming CNC feed rate and such on a relatively huge mill. Of course, I only needed to make two parts this time.

Larry

CarbideBob said:

Material and part size.?
Was focusing z needed? Draft on sides?
Moving or fixed laser and part?

Click to expand...

It was 420 stainless it shines a dot and a line for focus line them up and ran it straight wall no draft it was a non moving head fiber laser just a Chinese 50 watt we use it for part numbers and logos and such it is a little money maker
Don


Sent from my iPhone using Tapatalk Pro

It sounds like your angle is too steep if it’s 3 degrees. I wouldn’t recommend going any higher than 1 degree. Using a two flute would help with chip evacuation too.

As far as parameters go I would keep the rpm wherever you can to avoid vibration in the spindle and then a 0.0003” feed per tooth if you stick with the 1mm end mill

Hi I<3CNC:
Your ramp angle is way too steep...try 0.75 degree instead.
Aim for a chipload of 0.0001" and run it as fast as your spindle will go.
Keep it slathered with Rapidtap and go for it.

Your slot is actually pretty substantial; you can run a 3/64" stubby cutter.
When you said tiny I was thinking 0.015" or smaller.

What condition is your 17-4 in?
If it's solution annealed you might wish to consider heat treating it to condition H1150 before cutting the slot.
It will be nicer to machine than it is in solution annealed condition.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

First thought that comes to mind is why not EDM. I hate 17-4, but I've never gotten a batch that was properly hardened and it's always been super gummy and super inconsistent. Second thing, when the tool gets to the end of the slot, you're likely going to be contacting the walls full depth and it's going to want to bounce all over the place, I prefer to predrill any slot ends or corners in high radial engagement situations over any depth. And slotting, I never just go back and forth, I always step over at least a thou or two so tool deflection isnt' causing you to bounce from one wall to the other.

That said, I may be wildly off, luckily I never had to deal with much slotting in stainless.

Spindle vibration - does it make that noise at full speed with no toolholder installed? With any empty toolholder? Might it just be your shrinkfit holders?

Just about any cheap holder you can buy is balanced to G6.3 @ 12krpm minimum. There would have to be something really horribly wrong with his shrink holders to cause any noticable vibration at 6-10k.

Most likely OP has a belt driven spindle with a ruined belt.

I'd ramp the full length of the slot, and keep the angle at about 1deg. 17-4 responds well to trochoidal slotting, but that's probably a no-go at that size on that machine.

Definitely agree with Marcus that you don't want to be doing this in 17-4A, but disagree about the rapidtap (assume that's some kind of tapping oil?) - you want that well flooded to get the tiny chips out cleanly with no recutting. Air blast is effective too.

I've done thousands of these over the years. These are also 17-4 done with 1/32 solid carbide endmill.
Nothing fancy, no coating.

They are only .010 deep but I also had a lot of problems. What ended up working best for me was 3000 RPM, plunge in at F0.5 then feed at F1.0

OP said TINY endmills, I thought he was talking about .031" and smaller.

Mike1974 said:

OP said TINY endmills, I thought he was talking about .031" and smaller.

Click to expand...

I came here because I thought I might have some insight on how to get good performance out of an .017" endmill.


Here's the important questions: What condition is the 17-4 in? H900 is a piece of cake. Condition A sucks. That makes a big difference. What's the coolant situation like? How well are you flushing chips out? Finally, who made the endmill? That can be a big factor...

When I was running a 5-axis Microlution, "tiny" was anything under .005" diameter...

Hey everyone! thank you for all the info! As many of you pointed out my feed was way too high and my ramp angle was too high. I put it to a very shallow ramp with a .00015 chip load and everything held together was able to make my slot, cut just fine at 5k RPM.

1mm is by far the smallest endmill I've ever run, I was looking around and micromachining is just a whole other world of what you can do with a CNC very cool. Tiny is a relative term.

For the speculation about my spindle, the spindle motor had a bad bearing in the past, and after I replaced it developed a vibration. The spindle and motor shaft were rust welded together and it took a lot of force to separate one or both of the shafts deformed and bent a little bit in the process (it's a straight couple). It's not enough to make any real difference for most of the endmills I run and it's not worth it to squeeze out maybe a potential 1.5k RPM and I'm pretty sure it's going to involve replacing a lot of stuff at minimum the spindle motor so I just live with it for now, it's a CNC from 1999 as long as it's making parts I'm happy