feedrate help

[majariley]

this may sound stupid but what is the difference between ipm and sfm. i was taught to use the formula csx4/dia=ipm, then mutiply times three for carbide. that was ten years ago, and i have worked by myself so i haven't updated. i would love to here the different ways and reasons of other peoples feedrate formulas. i am currently using mc3 and fadals with carbide endmills programing 3d patterns.

[crazy^millman]

Well look at it this way. Rule fo thumb I have is for every 1000 rpms I usally have 10 ipm feedrate for 2 flute endmills and 15 ipm for 3 flute and 20 ipm for 4 flute endmills. This works aout to .005 per rev per tooth feedrate in inches. The SFM relates to what is the best surface feed for the endmill for a Spefic Materail. Alum in mind I am always limited by the machine not the cutters. SS then you have different option depending on the tool little as 28-42 sfm for HSS and 60-250 sfm depending on the endmill and the coating and more if you got the machine, right fixturing and so forth. If you ran Mazak's for years like I did you always worked in SFM and RPT feedrate so to get to IPM I made a formula for my Calucator I just punch up and get where I want for rpms and ipm on feedrates on Material and tooling that I using.

 

HTH

[Tim Johnson]

The best thing to do is to use the speeds/feeds in the catalog from the makers of the tooling. If your using Niagra tooling use the Niagra speeds & feeds for starters.

[mrainey]

majariley,

 

I wrote a free program that, among other things, calculates and illustrates the relationships between speed, feed, horsepower, etc. It has a user guide which defines a lot of terminology in terms that a machinist can understand. Several of the guys here have looked at the program, maybe it would be useful to you.

 

The calculated speeds and feeds are based on averages of data found in a bunch of different tooling catalogs, the Machining Data Handbook, and my own experience.

 

http://dl.winsite.com/bin/downl?14500000037133

[chris m]

Not to be nit-picky, but I think the 4 x SFM / dia is actually 3.8197 x SFM / dia [since pi= 3.1416 and not just 3]

 

As far as speed and feed selection goes, it varies a lot from mat'l to mat'l and from operation type to operation type. If you have no experience with a certain material or if you are looking to double-check yourself it is definitely a good recommendation to check out what the cutting tool manufacturer suggests and tweak from there.

 

C

[Threept82]

chris m

your awesome.

[chris m]

My spidey sense is picking up some ball-breaking...but now I get the handle anyway

 

C

[Storkman]

(sfm x 12)/(dia of tool x pi) = RPM

 

RPM x #flutes x chip/tooth = feed

 

 

It can get more complex if you want to figure in the radial chip factor.

[Threept82]

Ball-breaking? Yes.

But not directed at you chris.

[kathy]

Good Morning Guys!

 

Is there a place in Mastercam Define Tool function where I can specify my feed rate as IPR vs. the Feed/IPM field.

 

I have some special formed cutters and the manufacture's recommendations for feed are in IPR. Now, I know I can calculate the IPM (taking a mean diameter up the taper of the cutter), but I would prefer to let Mastercam do the calculations.

 

Btw, my tools are defined as a taper mill.

 

~Kathy

[Guest]

Kathy,

 

Not sure this is what your after but here goes...

 

After you define you contour and pick your tool, right click on the tool in the tool parametres page, there is a define speeds and feeds dialog box that comes up, looks like it might bo doable in there.

 

HTH

[kathy]

Jim –

 

I checked that page out (didn’t know it was there ). Unfortunately, I don’t know all of the other parameters for these tools (chip load, SFM, etc.) to get a good calculation. Plus, I have a specific RPM I want to hold and not be recalculated when I change feeds, and that seems to be happening when I use the feed/speed calculation page.

 

Okay – you guys can’t make fun of me cause my math brain is totally gone this morning –

 

But if the recommendation is .001 IPR @ 3000 RPM I get 3 IPM. I’m looking more for a feed of 30 IPM.

 

But, I just want to be able to input feed as IPR vs. IPM so I can tweek the cutters per the manufacture’s recommendation..

 

And – thank you for your response.

 

~Kathy

[Reece L Gibson]

Just type in as .oo5 in the feedrate rate prompt, I believe you can set up a switch in the post to inform the machine to output a G95 or G94 (what ever your control needs) and let the machine figure it.

I have a client that does that, just one of his things he likes to do. He says that way if the operator changes the RPM, the feedrate follows.

(Like the lathes)

[88Matt]

Just a quick mention about calculators and formulas. No matter how accurate someone swears they are, it is only a STARTING point. The true test is cutting chips. A calculator that allows you to input info about cut type, fixture rigidity, horsepower, etc., as well as the standard info will get you much closer. But nothing can replace cutting that first chip.

[88Matt]

Oh, hey Reece, see ya Thuresday. Hope you had a good holiday.

[Joel Walker]

sfm / dia. / .262