sparks and fireworks

[elraiis]

hey guys.. finally weekend is here..

can someone give me any sort of tip or hint for cutting 4130 steel? i ordered some TiAlN coated tools but looking at the feeds and speeds chart.. am not sure its correct.. rpm1100! i may be a total ignorant i know but am more familiar with alum where i never run under 10000. Just need a general hint to direct me like.. side milling with 1/2 EM say TiAlN coated.. lets say am cutting .4 deep one shot at a ar of .1.. according to the catalog i got with the tool i had to go 1100 rpm as i said with feed 8.8!!! isn't this a bit too slow like the job will take total forever. and with TiAlN we usually cut dry? u know i decided to miss around with the feed and speeds and i tell you.. i thought the sun was rising inside the machine.. the sparks were beautiful it brought tears to my eyes.. especially when i was making a helical cut.. any feedbacks.. and sorry for being so annoying guys.

peace

[Guest]

How about starting at a more reasonable 350 SFM

 

With the coating you may be able to bump up a15-20% further but that should be a decent starting point.

2600 RPM

 

.002-.003 CPT x 4 FL = 20. IPM to start

[elraiis]

oh! no way to cut steel at like at least 7000rpm say? feed 50 to 80 like? i really am asking to learn not to argue. is there a suggested different coating better than what i am using for this application? any clue?

[RobertELee]

I'm going to guess and say if your used to cutting aluminum you are currently using a 2 fluted endmill? If so change it out to a 4 flute.

[elraiis]

yes i did change it to 4.. learned that the hard way... as a matter of fact the tool i burned was 5 flutes.. lol... i tried running it at 6500 with feed 80. i made 6 parts with it... but after that.. usually with TiAlN we cut dry though? or with coolant?

[crazy^millman]

Really comes down to life of the tool. I was asked one time to take a 4 hour run time down to 45 min. I told them I could do it but it would cost them $3k of tool for every part. They left me alone after that. If going through an endmill every 6 parts works for you then any speed and feed will work. I personally have no problem burning and endmill up on every part if the time is short that my shop rate time. We get $100/hr here. Endmill cost $22.50 so I neeed to imporve my run time and change out time by 15 min to justify replacing endmills every part.

 

However if you are side cutting why not get an inserted cutter or is space that tight? Then you could get up to maybe 450 sfm and .006 to .008 per tooth with the right cutter. Now if I were running a High feed cutter I would be looking at a combimaster from Seco maybe 4000 rpm .025 depth of cut and 225 imp. That would probably last about 2 or 3 parts at that speed and feed, but again time would keep more expensive that the tool so who cares.

 

HTH

[cobra95kev]

I think you could easily take that tool up to 500sfm with a .003 cpt. Just remember the key to get the most out of the endmill is to take the largest axial cuts possible and light radial.

 

I would use up to 90% of the flute length with .030 to .050 radial stepover. The endmill may wear out quicker this way but you will remove a whole lot more material with it in a shorter amount of time. I would run it dry too.

 

 

[elraiis]

lol.. i like that mentality man.. time costs more i agree.. but here they are actually expecting a long living tool life + fast cycle.. and i forgot to mention am only limited to 150kb memory in the machine... so a 0.025 deep cut each time will cost me more memory no? not like i mind doing that but its just that am not sure the machine will let me.

is it true that yellow inserts are for dry run and everything else is to be used with coolant? someone told me that once.. a myth?

[elraiis]

thanks cobra.. i will surely try that.. thanks.

[crazy^millman]

I would run it dry with an air blast.

 

Well with a tool presetter life becomes easy when you care only about time and can show the tool is cheaper to replace than the time.

 

Good luck, but yeah I would try 500 sfm as well maybe as much as .005 per tooth. Heat is your enemy and the high the chip load the less heat in the chip. The lower the chip load the more heat in the chip. Just like on a lathe. Take a small cut with a high feed rate and then a small feed rate and see which chip turns blue and which one does not.

[elraiis]

so blue chip is no good? damn.. all chips i saw were dark blue... close to black... totally screwed up ya! thanks for all the help guys

[Guest]

The blue chip IS what you want, that means the heat came out in the chip and as it cools it turns blue.

[elraiis]

hi again.. ok! i WANT blue chips.. i want blue chips.. i'll keep that in mind.. lol.. man i feel like a toddler. thanks for helping me through this. but i don't have to see sparks and such right?

[crazy^millman]

Yes you want blue chips. What I was trying to demonstrate is when you increase chip load on tools you make the chips cooler. It becomes a balance between to much chip load and not enough was what I was trying to point at is all.

 

There are a lot of factors that go into selecting any tools for the job. The horsepower, The spindle speed, The size of the holder, The set-up, the flute angle on the endmill, the coating of the endmill, the number of flutes of the endmill. Then you got the material in which best works for that. I take what the book has and normally go 20% to 50% about that. I believe in the 2 for one rule in Manufacturing. For every minute I save is 2 minutes I gain. The one minute I got and then next minute I put on the next part or Job. If you take a job and cut 20 min out of the run time per part. You gained 20 minutes per part on the next job. So if you go through 10 endmills you need to justify in our case $250 of time saving by doing so. Math is Math problem is most people worry about that $25 endmill and not he $1000 of time they lost trying to make that $25 endmill last. To me sounds like you got the right method and good for you.

[Justin Beebe at Folsom Tool]

You might want to try a variable helix endmill such as a Hanita Varimill or a Niagra Stabilizer. You will be able to cut faster than a conventional carbide endmill and you will get better tool life.

[elraiis]

thanks justin.. i'll see if they'll agree to buy the stabilizer.. although i doubt they would. but thanks anyways i looked it up and lets hope it works as they made it seem it would.

[nofalloff]

Below are a couple of good vid on youtube of an imco 5flt cutter in 4130 running at 43ipm. I just did a job in 4130 and used one of these end mills as a finisher (roughed with a 1" indexable with 4 TiALn coated APKT style inserts from ultradex. The insert cutter I run between 600 and 650 SFM and the IMCO at 450 to 500sfm.

 

http://www.youtube.com/watch?v=NVJnyEiYtds

 

http://www.youtube.com/watch?v=T_vDpWRplbU...re=channel_page

[Hitachi]

How about a SGS Z-Carb to rough and a 4Flt CEM to finish?

 

Elco1971

X3 MU1 Mill L3 Lathe L1 5X

SolidWorks 2007 SP3.1

Dell Xeon 2.8GHz 2GB Ram

NVidia Quadro FX 4500

Windows XP Pro SP2

[tedly]

If you are going to heat treat this part later on, you should heat treat first before cutting it. We found out it will cut much better and easy on tools after heat treating to about 40RC.

[TMozzone]

ted,

back to work.