.015 Area milling

BrokeStatus · Mar 23, 2017

Hi,

New to the forums, and very new to the machining world, so sorry if I misuse any terms or lingo. I'm having difficulty machining 420 stainless with micro endmills, due to speed limitations. Working with a VF2 with 15k spindle. When reading the tool charts from Harvey tool I'm confused about what these speeds and feeds calculated actually are applied to. Do they just apply to dynamic milling, area milling etc? The recommended speed for the tool is 50k at 200 sfm with .28xDia radial and .3xDia axial. So since I can only spin at 15k that is roughly 29% of needed, do I adjust the rest of the parameters for 29%? I've just been breaking so many small tools that I'm becoming extremely frustrated.

Again, sorry for any confusion or lack of knowledge.

Thanks

Red James · Mar 23, 2017

Yes, you must adjust for the reduced rpm. Many people program feed rates by inches per minute so you may be feeding 3 times as fast as you should. Problem goes away if you program in inches per revolution (g95? check your machine to be sure) because as the rpm changes, so does the in/min feed rate.

BrokeStatus · Mar 23, 2017

The problem I'm having is that Mastercam uses FPT and everything else is calculated using IPT. What is the difference?

brian.pallas · Mar 23, 2017

What is the tool running out at? There can't be any runout at all with a tool that small.

I would start out leaving the cutting parameters, the width and depth of cut, the same. Back them off if you are troubles with breaking endmills.

FPT- feed per tooth
IPM - inches per minute

IPM = (FPT) x (# of teeth or flutes on the cutter) x RPM

What type of toolholder are you using?

BrokeStatus · Mar 23, 2017

Parlec collet style cat 40. Runout is .0002

Mastercam's speeds and feeds are

Feed rate ------ Spindle Speed------
FPT ------ SFM------
Plunge Rate------

So if Harvey tool recommends .00004 IPT for the tool do I put that in the FPT?

Mtndew · Mar 23, 2017

BrokeStatus said:
So if Harvey tool recommends .00004 IPT for the tool do I put that in the FPT?

Yes, feed per tooth and Inch per tooth are the same thing in Mastercam (unless you're in metric mode)
BUT
You have to make sure you have the tool defined with the correct number of flutes, so it's accurate.

BrokeStatus · Mar 23, 2017

Great, that is really the clarification I needed. Thank you.

Bobw · Mar 23, 2017

Back to the basics..

At a shop I used to run, I had the speed/feed formulas written in Sharpie on every
control in the shop.. I had no problem giving my guys/gals speeds and feeds(Surface speed,
and feed per tooth/rev), but I'll be dipped in dog doo if I was doing the calculations for
them to get RPMs and Inches Per Minute.

Yeah you need to back down the feed to keep the proper chip load..

Hopefully next week you have the same problem on the other side of the equation.. Running
out of feed rate and having to calculate backwards to get the optimum spindle speed to maintain
proper chip load...

OR, my favorite, having to calculate backwards due to HP limitations.

It may seem confusing now, but it gets easier.. Just always think in terms of Surface Speed, and
Chip Load.. RPMs and Feed Rate (IPM) are calculated #'s, and really don't mean a whole lot (except
the fact that you need to calculate and input them).

BrokeStatus · Mar 23, 2017

Still curious about if the recommended IPT is for all machining styles 3d,2d,etc..

Captdave · Mar 23, 2017

BrokeStatus said:
Still curious about if the recommended IPT is for all machining styles 3d,2d,etc..

.
Yes it is, all the tool care about is how much material is being cut per tooth

Hazzert · Mar 23, 2017

Well if your width of cut is reduced enough that radial chip thinning becomes a factor then some compensation is in order but I'll be damned if I will be using HSM on a .015 endmill. Lots of endmill manufactures will have different posted feeds for things like slot milling or side milling but if you're not given that information you're best starting shallow and slow and working from there.

brian.pallas · Mar 23, 2017

I would think that for a .015 endmill in stainless steel .0002 runout is too much. Simplest solution I can think of off the top of my head is to get those collet nuts that have set screws on the sides to allow the tool to be dialed in to, at least, less than .0001 runout. I have never used those collets with milling though, only with reamers.

.0002 runout on a 1/64 endmill is percentage wise like having .0064 runout on a 1/2" endmill. (Which is a lot)

Search

Largest Manufacturing Technology Community on the Web

Search

.015 Area milling

BrokeStatus

Banned

Red James

Stainless

BrokeStatus

Banned

brian.pallas

Hot Rolled

BrokeStatus

Banned

Mtndew

Diamond

BrokeStatus

Banned

Bobw

Diamond

BrokeStatus

Banned

Captdave

Titanium

Hazzert

Stainless

brian.pallas

Hot Rolled

Similar threads