stainless mayhem

[Jayson Kramer]

(unfortunately i can't get my hands on hanita varimills) too bad using these on 304 now using a 1/2 ball 4flt roughing at 300 sfm and .0065 chip per tooth. AP is .130 to .160

 

finishing with another one at start of 500 SFM Chip

AP is .02 on all surfaces and running F138. and tool lasts all day but I am throwing allot of coolant at it.

 

Are these carbide coated and have you called the Rep for some SFM for there tool in 304?

[elraiis]

yes they are carbide coated and i requested SFM and specs for the tools but for 2 days now i got nothing. The tool needs to be changed 2 to 3 times a day so far but i didn't get to use the data i got from you guys yesterday... i should be doing that today as soon as i get to work.

now tell me something.. is it better to cut steel and stainless steel dry? or with coolant?

 

peace

[Jaz]

quote:

---

is it better to cut steel and stainless steel dry? or with coolant?

---

Unless my cutter rep or catalog tells me otherwise I always use coolant. Currently the only time I cut dry is using inserts on steel. In your case probably you will have better tool life if you cut with coolant.

[elraiis]

Thank you

[Jayson Kramer]

I am with Jaz.

[elraiis]

aye.. i did the test and it went all good and nice.. chips color seemed good.. the machine's humming as well was no so bad... no sparks .. but hardly any improvement on the tool life! which was disappointing and i do not understand why! anyhow.. all help was really appreciated guys... as a matter of fact it could be normal for the tool to live this short when cutting stainless! i wouldn't know, all previous experience was aluminum and brass.. but i still find it hard to believe this should be normal... i mean if the part was mild steel or so i think the tool would have lived 5 x the life of it when cutting S.S. if not longer even

 

good night guys... it was a long annoying day am sooooo expecting to dream about this even tonight..

[cobra95kev]

quote:

---

good night guys... it was a long annoying day am sooooo expecting to dream about this even tonight..

---

Ahhh, the life of a programmer all right there in that quote.

 

In reality I was told iscar feedrate specs on their solid carbide endmills are based on a 20 min. tool life. So if you are beating that you are in the ball park, especially if you are cut ss at high speeds. Tell your boss to look at the amount of material removed in that twenty minutes, of course you could slow it down and get the tool to last longer but I would bet the amount of material removed would be similar. So you might has well run fast!

 

[Guest CNC Apps Guy 1]

It's the nickel in the stainless that chews your tools right up. Nickel is so abrasive.

[neurosis]

Can anyone offer an idea as far as cubic inches of material removal would be considered "good" before the endmill starts to fail?

[elraiis]

quote:

---

Can anyone offer an idea as far as cubic inches of material removal would be considered "good" before the endmill starts to fail?

---

hence i was asking for help i don't think you should take what i say in consideration. but i do not think there is a specific value answer to your question or even something close. this is my opinion and i'm happy to learn that i'm wrong as it would mean i learned something new from the experienced guys here again. but there are just sooo many factors to consider that affect the tool life. Holder, overhang, machine rigidity, coolant concentration + the type of operation you do. I'm starting to believe there is no such thing as a formula for feeds and speeds at all. All there is in books is a feed and speed starting point... thats only where you start then based on your jugdement and experience.. you improve it.. or like me screw it up. lol..

 

good luck.

Is cold rolled S.S. more nasty to cut?

 

have a good day guys

[dolphin1]

quote:

---

Is cold rolled S.S. more nasty to cut?

---

the thinner stuff is like any finished surface with plastic protectant on it and usually the more its worked at the mill when rolled out.

[neurosis]

elraiis,

 

I understand what you are saying, but there is a point that you must ask yourself whether or not its worth the cost of the endmill not to consider machining a different way. Which is why I asked the question. If you are not getting a minimum of X amount of material removed then something is either wrong with the process or the cutter.

 

Im sure that the tool manufacturers would give and idea but I would like to hear it from people that are actually cutting metal every day.

 

We are running a stainless job right now but I couldnt offer you advise because our material is 15-5 rather than 304 or 316. We are removing approximately 8 cubic inches per minute of material with a 1/2" 5 flute carbide endmill that is Tialn coated. We are able to get close to 220 cubes before the endmill quits on us. That is allot of material but as far as how long the tool lasts, well thats only 30 minutes of actual cut time or in our case, nine parts.

 

Jaz has pretty much been right on the money with all of his advise. One thing that I didnt see in your posts (I may have over looked) is how long your tool is actually lasting. What type of cutter path you are using, which could also make a huge difference, and some other particulars that would help assess the situation.

 

We are running our 15-5 job a little hotter/faster than some of what is recommended above but we started slow and worked our way up. Were still not sure that we cant get it to run even faster yet.

[Matthew]

Try and get a demo on a Niagara Stabilizer or Hanita Varimill. Most sales guys will test a tool for you. See what kind of tool life you get from them compared to your standard coated end mill. I thought at one time they were too expensive, but after using them on small production runs the time and tool life savings were more than enough to justify the cost of the tool. On day to day stuff a 1/2" variable helix carbide end mill will last a month here (I do prototype stuff only). In the past on production parts, I've remove 3/4x2 1/4 x 2 1/4" of material from 40 blocks and showed little signs of wear on a Niagara Stabilizer in 4140 Annealed material.

[Fred @ Slate Industries]

Tool Jockey

Is there anyway to get the ToolExpert to

input and output across the board English/inch?

 

Thanks

Tony

[Rob @ Target Machine]

elraiis - I hope you understand why it is important to "Break the skin" when cutting stainless. The outer "skin" is harder than the inner core of the stock.

 

I use an insertable to break the skin on both sides (top & bottom) before attempting to machine the first operation for two reasons.

 

1. Internal stresses.

 

2. The hard skin is all in the same plane.

 

If this is a large piece of stock, a comvetional cut around the periphery (profile) of the stock with an insertable EM can also help extend tool life.

 

This "peels" the skin off the outside, instead of "slicing" through the hard skin. This "peeling" method is more commonly used for flame-cut stock.

 

This is commonly called "blanking", or as I mentioned earlier, "breaking the skin".

 

With this strategy, my tools last much longer (it's cheaper to change inserts than endmills), and I spend less time fighting the bow/twist.

 

 

[ 06-19-2009, 08:02 PM: Message edited by: Mastercam Guru ]

[Rob @ Target Machine]

Tony - I was thinking the same thing. Too bad it's metric.

 

It would be nice if MC tool library had that type of interface with popular tool manufacturers entire line of tools .... updated daily.

 

LOL... I don't ask for much, do I?

[elraiis]

heyy.. .sorry for the late reply i was out of town in the weekend.. really sorry...

220 cubes? ok! to be honest i do not know how much my tool cuts before extermination. u got the formula to calculate it or i look it up? we are running production no prototyping. and i can't decide what type of tools is purchased here either... unfortunately.

 

i'll look up the formula and let you konw the how many cubes my tool eats before dying... we actually got a mitsubishi insert tool! it ran good at the beginning and i set a counter for 20 parts change.. so it ran good for 2 days.. then on day 3 inserts broke and holder burned and the counter wasn't even 12! and when i say i put the counter to 20, trust me the tool could make more and it was in good shape at 20 count. but for safety i put 20 anyways... however, out of nowhere... 12!! no accident, no part pulled out to cause damage.. nothing.

[neurosis]

The formula is quite simple. Instead of putting it in my own words,

 

Copied from MMSOnline.

 

mrr = ipm x woc x doc

 

Where:

mrr = material removal rate

woc = width of cut

doc = depth of cut

ipm = inches per minute feed rate

 

Finding your overall material removal after this is simple also. Use mastercams built in setup sheet tool. You will see at the bottom of the page that it gives you a cycle time and also the actual feed time.

 

so,

 

MMR * feed time will give you your material removal per part.

 

I cant say that this is 100% accurate but it will get you in the ball park.

[elraiis]

hi

if i calculated this right my

MMR X FEED TIME= 13.4/part how screwed up is this? or normal? and the tool dies in 7 pcs so does that make it 93.75? is this bad? what average?