S.O.S

[elraiis]

Hey guys..

is there anyone here really good in feed and speed calculation or someone who knows a good book he can refer me to that deals with this matter. today i was called by a friend to replace a broken tool. and i saw a shoking program 'to me that is' where the programmer was slotting .2 deep in aluminum using 5/32 standard carbide endmill at a feed of 60!!! The RPM was 9500. if i'm not mistaken shouldn't the feed at this feed and DOC be max around 30? am i missing something!!! i defenately am.. anyone who understands the math or whatever it is behind proper high speed feed and speed cutting for aluminum, brass, tool steel and such? buzzzzzz me plz.

[Jeff the haas_guy]

Dude...........Chill out...

 

Was is a 2 or 4 flute?

 

Jeff

[DavidB]

If it's working go with it. The Feed and Speed seem OK but I was suprised with the depth of cut been taken it's more than 1XD.

I read in here with Al most poeple have the idea push the cutter till it breaks then back off 5%

There is more to it than looking at Feeds and Speeds in a book or software. Number 1 is Rigidity. Then there is tool overhang, work holding, machine condition, etc etc.

 

If in doubt ask the Tool supplier there the first port of call.

[elraiis]

2 and again the tool was not profiling... slotting. thx man am chill.. just too anxious to know how they calculate high speed machining.

[Jeff the haas_guy]

I am more conservative with tooling. I would go 50% to 70% depth with a tool that small. A larger tool like 1/2 or 3/4 you can push. 5/32 is to small to push that deep.

 

Good Luck

[c-hook]

How long were these slots he was cutting? I have run .125 4fl carb. E.M. at .187 doc in a 304 SS casting before, and suprisingly it held up........ for about 2". Seems to me that pushing a tool that hard will GREATLEY reduce the life of the tool, I'm not saying it can't be done, but just doesn't seem very practical. Which in the long run, could be worse than taking smaller cuts. When you factor in the cost of tooling, time it takes to replace it, re-calibrating, restarting, it might actually take longer to get thru a job. But hey...if it works......

[elraiis]

he was making a heat sink type... the slots are about 10" long. but correct me if i'm wrong.. wouldn't the feed be the fpt X #of flutes X RPM? i mean for a cutter that has a diameter of .157 how much Chip load per tooth can it take?!?! 2 flutes! so that would be around what? 0.0032 per tooth? isn't this too much? the main reason of me asking u guys this is that am doubting the way i calculate my feed now... for instance i give the 1/2" endmill usually 0.005 chip load per tooth to calculate my feed. i know that wouldn't be the max the tool gives but i rather use than abuse the tools. so seeing a .157 run at about 0.003 vs my 1/2 running at 0.005!!!! i felt that maybe i should start pushing the 1/2 at 0.01 per tooth instead. but thinking that alone is freaky rather than me trying to do it for real on a machine... u hear me guys? so what is it then?!?!? i don't know.. help?

[Mr. Dayshift]

That little cutter should turn at .001-.002 per rev i'd say, and an engraving tool at .0005 per rev.

[c-hook]

I think the the key to having success cutting aluminum that agressivly is to have good chip evacuation. Alot of the time it is the chips getting caught up in the line of cut is what causes the end mill to break. Personally I feel that you are putting too much thought into the matter though. Consider that every job set up has it's own character if you will, what might work on one set up might not work on the next. There are just too many variables to consider. Seems to me that you understand feeds/speed enough to make a good decision. I have a habbit of taking note as to what works for ME and what doesn't, that way when a similar situation arises, I have a better stating point to work with than what the charts say. Just keep in mind that what you read in the charts is only a starting point.

[Jake Statz]

quote:

---

just too anxious to know how they calculate high speed machining.

---

High speed machining can be calculated many different ways. But usually HSM is calculated on high feeds with small Z steps. Just remember that the feed rate must always remain relative to the rpm to keep the same chipload. We work with aluminum everyday and do a lot of HSM. typically the rule of thumb for ROUGHING is to take Z steps of 10% of the tool dia. CS (Cutting speed) can typically range from 1200 to 1700 SFM (Surface feet per minute) with chip loads varying from .01 to .02. for example we would run a Carbide 3 Flute 1/2 Bull Nose at 12800RPM 750 IPM Z depth of .05. This ends up being a CS of 1600 and chipload of .02.

quote:

---

There is more to it than looking at Feeds and Speeds in a book or software. Number 1 is Rigidity. Then there is tool overhang, work holding, machine condition, etc etc.

---

+ 1000

These #'s are base on a cutter that is sticking out no more than 3 times the Dia. Anything sticking out farther should have the Feed and Rpm's reduced by 20% for every 1 times the Dia. more that its out.

 

So in our HSM theory the 5/32 Carbide 2 Flute EM would run 20000RPM(max rpm on our machine)at 400IPM .01 chipload with Z steps of .0156.

 

At first the feeds and speeds scared the crap out of me and I didn't beleive it would work. But It has been working great for over a year now.

 

Now these are just roughing numbers finishing is a hole other story.

 

Cutting 6013 Aluminum on a Makino S56 with a 20000 Rpm Spindle

[elraiis]

thx