[Skeeterd5150]

OK here is the situation. I am facing off 5.5" A36 structural steel blocks that are 12" square to a final depth of 5.125". I am cutting with a 2"seco octomill with 4 F40M TiN inserts. This is my first tool with indexable tooling so I aproach this project with some trepidation. I am cutting with Lenox bandade synthetic band saw cutting fluid(don't laugh). With the cutting parameters of 350sfm with the chip load of .006 and .1 doc, I get a decent cut and good loose #6 shaped chips. I am running the spindle at 669 rpm and feeding 16ipm. By my caculations I am cutting 3.2 cubic ipm. My question is I feel that I should I be cutting faster than that but I don't want to screw up my inserts prematurely. I feel like I could go up to 450 sfm with chip load of .008 and the same doc. Running the spindle at 860 rpm and feeding at 27.5 ipm. Again that would give me 5.5 cubic ipm. Any thoughts would be appreciated.

[Geof]

I think ditch the coolant and go with an air blast or even nothing. Facing steel you can get a negative effect from the coolant because it chills the hot insert and can cause micro-cracking leading to edge breakdown.

You should be able to take the speed up to 450, maybe even higher with a good depth and feed like you are considering. When everything is nicely setup the majority of the heat from the cutting will end up in the chips and your inserts and the part should be cool enough to touch even if only briefly. Your chips may even come of glowing dull red which is pretty well the best condition.

Also you will be able to see a characteristic cratering on the inserts a few thou back from the cutting edge. This is where the chip is making contact.

Monitor the surface finish, initially it should have nice clean shiny tool marks but as the inserts start to go it will change to a duller appearance and eventually start showing sort of minute tear marks. This means your inserts should be replaced.

[Skeeterd5150]

so i should be able to go with the .002 thousands higher chip load and be fine? And are all my numbers good? I am just starting to figure all this sfm stuff out. I was just guessing for a year. Also should you drop the sfm with a higher doc and how much? Is there a decent ratio?

[Geof]

Trepidation is a good thing but experimentation is also a good thing. I am surprised no one else has come on with comments because it would be nice to see if my opinion is backed up.

I loaded up a couple of pictures: First one is the chips produced from running a 1.5 dia four insert face cutter at 1000 rpm, 0.008" feed per tooth and I think 0.15" deep in hot rolled steel more or less equivalent to A36. Second picture shows the surface finish which is starting to dull down a bit because the inserts has removed quite a lot of material; these pieces started out as 3" round bar 17" long and where taken down to 2-1/4" by 1-3/4". This was all done with air blast.

I was a bit limited in power, this was done on a Haas Super Minimill which has direct belt drive so torque is limited at low rpm; not really the correct machine for ripping off steel.

If you are doing several of these blocks I suggest you go about varying things systematically: Always keep an eye on spindle load and try taking the speed up toward the 650sfm. Maybe take the feed up to 0.01" if you have the torque and if the machine is handling that increase the depth of cut.

And monitor the condition of the inserts. As I said you should see cratering wear back from the cutting edge and you should see the surface finish change as the inserts wear.

Your comment about premature insert wear is not completely relevant. Do you mean premature in terms of cutting time? Or premature in terms of amount of metal removed.

I think you can accept that if you mooched along really slowly your inserts would last forever and would remove a lot of material. But time is money so you don't want to take forever.

On the other hand you can go like a bandit and kill the inserts within a very short time. Sure you are removing metal very quickly and saving time but at the cost of paying more for tooling.

Somewhere in the middle is the place you should be where there is a balance between your cost in time and your cost in tooling. For instance if you increase speed, feed and depth of cut so you are removing metal 50% faster and your insert life is cut in half maybe that is okay because what you save in time is worth more than the expense of replacing inserts more frequently.

[MDLang]

Nice chips Geof, Maybe a bit more surface footage if the insert life is good.

I pretty much always start at 600-650 SFPM these days for alloy steels, hardened alloys at 550, and 750+ for low/medium carbon when running 90 degree inserted end mills/face mills..

A36, I'd start at 650 for sure and work up, same DOC, .008 -.01 chip per tooth( remember your running a 45 degree lead angle so there is some chip thinning occurring).

Leave a .012 for a finish pass at 800-850 SFPM at .005 chip per tooth and you'll get a shinny finish.

I'd start at the above hoping for 25 - 30 minutes in cut before indexing. Adjust accordingly.

Standard just my opinion disclaimer applies.

BTW, Nice chips Geof. Oh, I already said that, just a little darker blue I think would be just right.

Just noticed the cutter there. Looks like an APFM 1604, style insert 15(75) degree cutter (Handy way to use up the unused 1604 corners). For that cutter I'd say your chips are perfect.

Maybe an Iscar? The inserts look a bit wide for 1604's.

My only gripe with that style of cutter is the low feed required for a good finish on finish passes.

Mike

[Geof]

.....BTW, Nice chips Geof. Oh, I already said that, just a little darker blue I think would be just right.....

Not with a Haas Super Minimill. I was running about 110% spindle load, direct drive motors just don't have the grunt.

It is an Iscar, nice little cutter.

[joecnc1234]

Inserts have a sweet spot for doc either below the screw or above it. If you get above the screw you will definitely need an air blast I recommend an air blast on steel as Geof said coolant is hard on inserts running at high temps. The major factor is rigidity of the set-up. You don't want any vibrations or harmonics as they will lead to premature insert failure.
Joe

[MDLang]

Geof,

I have to say I'm really impressed to see chips like that come from a Supermini. I've tried to find out how they run in real life but there are very few around here.

I keep thinking a Supermini would be the perfect tool for getting the small work off the 125,000 dollar machines that run the parts at 5% spindle load.

We have a couple machines that are pushing 7 years old and the president is thinking time to trade them in. I envision one new replacement equivalent to the current machines and two Superminis in place of the other(literally in place of as 2 minis would occupy the same floor space).

Mike

[Geof]

....I keep thinking a Supermini would be the perfect tool for getting the small work off the 125,000 dollar machines that run the parts at 5% spindle load....

Yes.

If you do look into something like this get the raised Z option. The top of the machine is lifted 4" giving you greater Z clearance. This way you can run a HRT 210 Rotary Table. My Super is outfitted with two Kurt vises that can be switched for the rotary. If space is limited and the parts are small I think the Super is a good value for money.

[Skeeterd5150]

Yeah sorry I took so long responding. I bumped up the speed to 475 sfpm at 860rpm and 27.5 ipm. Chip load was up to nine thousanths. My chips were getting browner and the finish was starting to look alot better. No cratering yet. The inserts look just as good as when I put them in(just dirtier). I'll get some pics next work day. But the only thing I am worried about is the doc. I am running a Swi DPM V5 cnc bed mill. It only has 5hp spindle motor. I was screwing around with seco's milling calculator and i was saying at full width cuts I am exceeding my machine's capacity.

[Skeeterd5150]

i meant 889rpm and 32.1 ipm

[Geof]

..... But the only thing I am worried about is the doc. I am running a Swi DPM V5 cnc bed mill. It only has 5hp spindle motor. I was screwing around with seco's milling calculator and i was saying at full width cuts I am exceeding my machine's capacity.

Yes, be careful; I was also horsepower limited. Nominally the Super has 10hp but this is probably reduced quite a bit at low speed. However, I have spindle load monitoring activating autofeed so my controller backs off the feed in 10% steps if the spindle load goes over 120%. I can afford to be a bit daring because it is not likely I am going stall an expensive cutter without stopping the feed. This can not only kill the inserts but also the pockets.

If your chips are still brown it is possible you could take the feed up a little more but maybe take the doc down by the same percentage; i.e. feed 0.01ipm, doc 0.09".

And take photographs with labels showing the conditions so you can refer to them in the future when you have forgotten what you did this time. I often take notes...but then forget where I stashed them .

[eorourke]

I believe that I would try a harder grade. I would try a P-25 grade of carbide. I think that .006" per tooth is a good start as far as chipload. I would also make sure that I was climb milling with an air blast. I would also take .125" depth of cut if necessary. One could run their chip load up to .008" to .010" per tooth depending on the radial engagement and the HP of the machine. Finally, with a P-25 grade of insert, I would run it at 725-1000 SFM.

[Skeeterd5150]

What is the C grade of P25 and is it available in an octagonal insert?

[eorourke]

Good question! The C grades were big back in the 60s, 70s, 80s but started being phased out as the coatings for the insert started to blur the distinctions. The International Standards Organization (ISO) developed new classifications of carbide inserts due to applications. The first company to use color coding of insert grades was Seco in the early 1990s. They classified the inserts as follows: 05 thru 50 designated the substrate hardness with 05 being the hardest substrate and 50 being the softest- P-Steel applications Color Blue- M-Stainless Steel applications Color Yellow- K-Cast Iron applications Color Red - These were the original color codes. Later Green was added for nonferrous metals(aluminum) and grey(I believe) for Hard Machining applications (>50Rc). For Instance, The substrates were identified by P for steel and then 05, 10, 15, 20, 25, 30, 35, 40, 45, 50. If you observe most carbide companies now label their insert grades according to the type of coating and then the substrate hardness. For example Seco might say that Their grade is TP25M. This means that it is Titanium coated with a P-25 substrate and the M would stand for Milling. Kennametal and Sandvik and other companies use similar types of coding for their grades. Thank you for reading this rather long winded essay on carbide grades.

[joecnc1234]

geof,
did you take those chips from the drill press and throw them in the mini mill.
I've worked with a dozen mini mills and never seen those type of chips. not even in aluminium:withstupi

[Geof]

geof,
did you take those chips from the drill press and throw them in the mini mill.
I've worked with a dozen mini mills and never seen those type of chips. not even in aluminium:withstupi

I have to admit I have never seen blue chips in aluminum. I suppose I could run off to my anodizer and get them done but at $1.25 per it might cost as much as the machine .

[joecnc1234]

see, you better make a good relationship with the anodizer, one of my good friends is my local anodzer and fellow harley rider he could hook me up with blue or red or orange chips if I needed it.
Joe
If you need anodizing look up ace anodizing in tucson ask for andrew good man.

[Skeeterd5150]

I get good results at 625sfm and .1 doc. I have the chip load at .008. I finish it at .01 doc and it looks nice and shiny. I can get the chips blue though. Some of the ends of them are blue. I tried to go deeper and I got a ton of vibration in the machine. Thanks for all the help guys. One more question. Does the same practice of no coolant apply with 304ss as well. And what sfm should I start at with the same inserts. DOC, more or less?

[Geof]

You have 5hp available so I would say you are probably at the limit of your machine.

Regarding stainless...this is a whole different kettle of fish. You may get other advice but my experience is: lots of coolant, around 300sfm (maybe less), possibly the same feed or even greater.

Stainless work hardens so you do not want the tool to rub; you want it peeling off a nice chip that is thicker than the work hardened layer created by the machining.