feeds and speeds

[scott gault]

i'm new at programming. i am used to setting my feeds and speeds by feel as i'm machining. i've downloaded cimco's feed and speed calculator and it looks like good stuff, but i am a little confused. there are fields to fill in to give fpm feed rate. but nothing to give depth of cut at the feed rate calculated. is there a rule of thumb that i don't know about ie. 25% of tool dia. or something. An example, if i use the feed and speed calc. and select a 4 flute .5 cutter and select .003 feed per tooth and 300 sfm. the calculator tells me 2291 rpm. and 27 ipm feed rate. How deep of cut is this calculated for? obviously coolant and material being cut are variables but how deep is this calcuation based on. thanks for any help.

[spade117]

Average axial depth is 1/2 to 1-1/2 times the endmill diameter.

[chris m]

Also depends on slotting, profiling, pocketing, etc. As long as you are going to be around the machine when it actually runs your program you are better off programming conservatively and see how the thing cuts. While the program runs you can play around with it and get a feel for what works; as you build experience you can feed that back into your programs.

[scott gault]

I'm kinda slow sometimes so let me make sure i got this straight. if we use the example i gave i should be able to cut .25 deep with .5 in. 4 flute cutter at 2300rpm and 27 ipm.

[spade117]

It depends on what application are you doing and material being cut.

[scott gault]

mostly doing pockets and contours in 6061 alum. i've been doing .015 depth cuts and running about 40 ipm with .250 cutter dry.( i run dry because i don'thave a containment cabinet and the mess would not be tolerated. military has to be clean and shiny you know) it seems to go good but, would like to go deeper if possible but don't want to go too deep and gall aluminum to tool.

[Tim Simmermon]

quote:

---

i am used to setting my feeds and speeds by feel as i'm machining.

---

Use that experience to help determine DOC. For a good rule of thumb DOC is dependent upon your application, Feed & Speed are dependent upon your material. Of course they cross over, but you get the idea. DOC is mostly determined by chip evacuation (and Machine HP). Obviously there is better chip evacutaion if you are cutting on the side of the part, so you are able to take a deeper depth of cut. If you are slotting, the chnces of recutting chips are greater so you take a lighter DOC.

 

quote:

---

I'm kinda slow sometimes so let me make sure i got this straight. if we use the example i gave i should be able to cut .25 deep with .5 in. 4 flute cutter at 2300rpm and 27 ipm.

---

It depends, are you using a carbide cutter and what type of material are you cutting? The DOC is a good start.

[Mcam Nut]

Alot on doc depends on the rpm you have on your machine if your max rpm is low you may want to run at a bit deeper cut, but if you have a high rpm machine I find you will get much better results at at high speed/feed and a light doc. I would run a 1/2 2 flt SC at 12000rpm and around 250 ipm at a .15 doc pocketing 6061 on our horizontals, and on our verticals the top rpm is 7000, and not as rigid as the horizontal, I would run the same tool at 6500rpm around 65ipm at a .375 doc, so I guess it depends alot on the machine and the application you are doing

 

 

:EDIT: Just read you are running dry, forget the speeds and feeds I put there, they will NOT work

[Tim Simmermon]

.015 is definitely a light cut, but not using any coolant will tend to cause problems. When cutting alum there should always be plenty of coolant. 2 flute cutter would be best. The SFM should be a lot higher for alum.

[HevyMetl]

Run coolant, clean it later. I use the blizzard endmill from OSG and it runs pretty good dry, but it you want to really push it you need coolant to help get the chips out.

 

1/4" Ø 3 flute I would run at .125 doc full width possible at 18300 rpm at 211 ipm. This equates to about a .004" chip load and these little buggers scream. Suface finish is surprisingly good with good holders. Tool life is fenomenal. HTH

[scott gault]

i guess i should have stated my machines limitations. it is a vertical 9 x 48 bridgeport style with a 3 hp motor and limit of 4000 rpm i'm not a production programer just little jobs for special f-16 tools so i'm not pressured for speed. i have run with cooloant but without cabinet it makes such a mess. maybe i should consider making a splash cabinet? all the help is greatly appreciated and i think i may be able to work the machine a little more than what i am. thanks again everybody.

[HevyMetl]

The blizzard will help you with dry chip evacuation at that low rpm. Drop you feed down to match your rpm. Also watch running a bridgport style spindle at max rpm for more than a few minuets, because it will start getting hot and start growing on you.

[Mcam Nut]

quote:

---

18300 rpm at 211 ipm

---

Thats pretty impressive John, man I got to try them endmills. We max at 12k, but even there we would make up alot of time, I just have regular osg here for our 1/4" but i cant seem to be able to get the tool to last at all at feeds over about 80. I was pretty impressed with a 1/2" ma ford I tested, but I heard alot of good things about the blizzard, time to give it a try

[HevyMetl]

I bought them for the model shop next door after they were having some problems with their standard 3 flutes. They were trying to run 12k in their subspindles, (auxillary 40K nsk mounted to the side of the head) and it required more than the small motors wanted to deliver, so they were rubbing the material gauling ect. I bought these and proved them out over here in our Makino by monitoring spindle load and was very impressed by how little they required to run at that rpm and feed rate. They have been running them for about a year now and that is all they want to use. I will say that OSG has been SEVERLLY slow on delivery as of late.

[chris m]

OSG tools = good

OSG service = bad

 

they are, however, "working on cleaning up the backorders"

[Gramby]

Scott 2 or 3 flute cutters work good on alum. 3 flute are just hard to measure after resharpened unless you have a 3 flute micrometer. 4 flutes in alum don't give the room for chips to excape.

For what your doing "job shop work" I would go 50% of dia. for depth of cut.

Can you use a coolant mister? I understand flooding would not be pratical. Misting with coolant would give a little lube to prevent gauling and reduce heat a little.

I assume your familiar with manually calculating speed and feeds?

 

RPM= 3.82 x SFM / Dia.

 

Feedrate = Rpm x number of flutes x chip load

[scott gault]

depending on what i'm doing (pockets or contouring)and availability, i'll either use 2 or 4 flute mills. after seeing everyone's suggestions i think i'm gonna try to build a splash cabinet for my mill and use coolant all the time. feed & speed formulas? yea i saw them once back in air force machinist tech school. i've not really had to use them much until now, i've just went by feel and experience in the past, so they are a good thing to refresh my memory. thanks again.

[Mcam Nut]

John, I am putting in a order for a couple 1/4 blizzards, but i am unable to find any info on a 3 flt, I got the info for a 2. Can you please send me a link for the 3 flutes?

[Guest SAIPEM]

quote:

---

i'm new at programming. i am used to setting my feeds and speeds by feel as i'm machining. i've downloaded cimco's feed and speed calculator and it looks like good stuff, but i am a little confused. [Confused] there are fields to fill in to give fpm feed rate. but nothing to give depth of cut at the feed rate calculated. is there a rule of thumb that i don't know about ie. 25% of tool dia. or something. An example, if i use the feed and speed calc. and select a 4 flute .5 cutter and select .003 feed per tooth and 300 sfm. the calculator tells me 2291 rpm. and 27 ipm feed rate. How deep of cut is this calculated for? obviously coolant and material being cut are variables but how deep is this calcuation based on. thanks for any help.

---

http://www.machinist-toolbox.com/mtb.htm

[HevyMetl]

Shawn here is the link that I use for all of OSG's High Tech cutters as they call them. If you are going to get into hardmilling of tool steels I would reccomend Jabro through Tesco as the way to go. HTH

 

OSG's Blizzard page

[Mcam Nut]

Thats what im looking for John

[Tim Johnson]

Use can use hss for 4000 rpm. Get a spray bottle and adjust it for a "heavy mist". You should be able to start at 24 ipm with a 1/8" doc with no problem, just keep the end mill wet enough so the alum doesn't stick. The area around you should stay relatively clean also.

[67 Yankee]

Yes what Tim Johnson said.

 

Also you can get a spray mist unit for your bridgeport machine which will allow you to let something run while you go do something else.

 

I used to run a manual Bridgeport type machine and even there the mist unit was a huge help because I was able to use both hands on the machine without the part going dry.

 

 

I don't know anything about the seller, but here's what I found on my first spray mist unit search just so you can see what I'm talking about if you're not familiar. Spray mist unit