Efficient roughing

[Smit]

Hi all,

I've uploaded a part to Cadcams FTP site in the MC8 directory named Hsrough. Material is 440SS. 15 Rockwell hardness. The operations are for roughing the part, using a 3 fluted insert mill and a 1" rough mill. On the 3 flute I've used the speeds, feeds and depth of cut recommended by the sales rep. According to the backplot there's less than a minute savings using the carbide. So in my never ending quest to save time I was hoping that somebody might have a more efficient way to get that rough material out of there. I've heard of people using high speed techniques to take smaller depths of cuts at a much higher feedrate but can't find any data on doing this. We'll purchase tools if necessary to achieve this goal. Thanks in advance for any input you might wish to lend.

Larry

[RAJ]

USE INGERSOLL INSERT ENDMILL ENDMILL(HIGH POSITIVE) 1.0 DIA .075-.125 DEPTH OF CUT DEPENDING ON WAT YOUR MACHINE CAN HANDLE 1850RPM INSERT GRADE 847 60.0 IPM.

THIS SHOULD REDUCE UR CUTTIN TIME CONSIDERABLY.

[Smit]

Thanks Raj,

Are you aware of a web site where I can get information on this inserted mill? Our normal supplier doesn't carry Ingersoll, and a web search didn't get me anything. 60IPM in 440 Stainless sounds pretty great!

Thanks,

Larry

[Christian Raebild]

Using the search program 'Copernic 2001 Pro', it took me just under 2 minutes to find the manufacturers site, www.ingersoll.com

I am sure they can tell you where to find a local dealer.

I have also seen good results with 'SECO' and 'Iscar' tools, so you might contact their dealers, too.

Which type of machine and control are you using? If you are doing 3D work, some controls have functions to implement NURBS or parabolic interpolation. I have seeen examples, where using those functions halved production time, and improved the surface finish.

[Smit]

I am running this part on a Haas VF-8. 15 horsepower, 7500 RPM spindle. No complicated 3D machining on this part. Just the need to remove some pretty tough material fast. I've talked with the Iscar rep in this area, and his recommendations will save some time, but nothing like the 60 ipm RAJ mentioned in an earlier post.

[mcrae_andrew]

60ipm Does sound good, however, the more important parameter is feed per tooth (Stainless likes at least .006 and as much as .012 **True FPT**). Keep the FPT up and apply a chip thinning factor to get bonus table feed value. Ingersoll, Iscar, Seco, Kenna and the rest are all useless for help - Call the Swedes and get the proper tool. Use a Sandvik R390 Endmill with a 1025 Grade Insert - Positive Geometry Chip Former and watch the chips fly off. The Sandvik Rep copuld help you calculate feeds and speeds based on Chip Thinning and also optimize the Carbide Grade for better edge security.

My 2 cents will turn into Your Multi $$ Profit (Which James will tell you to buy a new machine with... He hates Haas!)

Andrew

[Tony]

There are two school's of thought...

1). F the cutter

2). F the work piece

I was brought up F the work piece

cutters were to valuable and harder to come buy.

 

Then one day down the last 17 Years,

I was working with the other theory...

This guy programmed all steel removal at 200 ipm.

Then while cutting whatever he was cutting he would look at the chip's and back it off as needed.He ruined cutters and holders and BUT I learned what you could get away with.

The End

[ 10-13-2001: Message edited by: Tony ]

[tirenut]

Larry,

Just thought that I'd drop in with a little "relevant" information for you. I say relevant because we have the EXACT machine as you and cut the EXACT Materials. Our VF8 is a 1997 model and has been eating steel since the day it was born - so we know a little about making this machine cut. I will start by saying that it IS a different animal because of its size.

I will start by saying that since you own one of these things, you obviously know one of the limitations of the VF8 - in one word -SPINDLE OVERHANG! Yep, these guys on here will give you info on what they have seen, and that is good, but there is a HUGE difference between a small C frame machine (IE. HAAS VF1,2,3,4, Fadal 2016,4020,etc) which have less than 20" of spindle overhang and a machine like ours which has 40" of spindle overhang (from the column to the tool centerline) - Big rigidity problem, but it can be overcome.

How do you make it cut you say? There are many keys to it.

Number 1. Pick a tool manufacturer - we use Ingersoll and Iscar High Positive Tools and they will rip! I'm not real sure where Andrew gets that the ingersoll tool reps are useless. Maybe he has a bad ingersoll rep, but their applications guys are the envy of the tool manufacturers who compete for automotive OE work around here. That is why Iscar bought them - for their App guys and their specials capability. Ingersoll's inserts have been made by Iscar for a while now anyway, so no quality compromises were made when they got bought out.

Number 2. Get the absolute shortest cat40 toolholder you can find - all CAT40 Holders are not created equal. This makes a HUGE difference in all machining - but especially when you are eaking out all you can from a machine like ours that doesn't ooze rigidity. Stub that sucker up at all costs and you will benefit.

Fitz Rite makes the shortest projection 3/4" shank Weldon CAT40 holder on the market. It is super short compared to Command's, Lyndex's, or ETM's. The tool shank actually projects clear up by the tool knob inside the holders taper. This, in turn, will force you into using a 3/4" shank cutter. This isn't too bad because you can get an Ingersoll 1" diameter, 3/4" shank high *** tool with 3 inserts, .4 max DOC, and 1.5" projection from holder. Load it with 847 grade inserts and you are ready to mill stainless. There is one tool out there that will outfeed this tool and its Iscar's Mill2000, but you can only get the 1"diameter, 3 flute with a 1" shank which forces you into a longer projection toolholder which negates the feed gains you get from the tool. This particular insert is stronger than Ingersolls design and lends itself to higher feed per tooth, but our machines don't really have the ponies to take advantage of it. Both of these tools (Ingersoll and Iscar)WILL smoke a Coro390 from Sandvik in like material on like machines - been there, done that, and have video to prove it. In the Coro's defense, it does have better mismatch control on multiple depth passes than the two I's tools.

Nubmer 3. Take advantage of Radial chip thinning like Andrew said - it WILL boost your programmed table feed on contour cuts. It isn't rocket science and everyone should be doing it anyway. The key to RCT is to remember that unless you are contouring with atleast half of the cutter diameter (thereby attaining the programmed feed per tooth at tool centerline), you aren't getting the feed per tooth that you think you are. Adjusting feed for RCT will give you more scientific results because you actually know what chip thickness you are getting.

Number 4. Don't run coolant on these inserts! You NEED the heat in the chips for everything to work right. Use high pressure air to clear your cut and stabilize the cutting enviro temperature. This is key! You don't want heat in your part after your cut. If you have it, slow your SurafceFeetMin or boost your FeedPerTooth to get the heat in the chip and out of the part. Chips should be a perfect nubmer 9 with smooth edges. If you have jagged edges on the leading edge of your number 9 chip you are going to start the chatter battle which can be a long one.

Number 5. Make your setup as rigid as possible. If you are holding in a vise, put it in the jaws as deep as you can. If you are holding with clamps, put another one on. Do Not overlook this step! You want the absolute shortest distance possible between the spindle face and the bottom of your cut (derived by toolholder, tool combination) and similarly, you want the absolute shortest distance between the bottom of your cut and your holding device (derived by your workholding system being used.

Nubmer 6. Play with it and learn something in the process. Get a hold of an Ingersoll rep and tell him that you are looking at his tools for a particular job. I haven't run across one yet who wouldn't come in a prove it out with no cost to you for blown cutters. You will have to play with Depth of Cut, RPM's, and Feedrate to get the results you desire. But you WILL get to atleast 60ipm in stainless at around a .1875" to .200" DOC with this machine and these tools.

Sorry so long, but I had some time, so I thought I'd give a little tooling basics 101 for future searches. Alot of people overlook the most critical part of all cutting operations and then wonder why somebody else is making money and they aren't.

Brett

[Guest CNC Apps Guy 1]

I wouldn't say hate, I just like MORE machine. More rigidity, more Horse Power, Better Accuracy, Better Repeatability, etc.... Though I wish Gene Haas would make a machine like a Mori, Makino, Kitamura, Yasda, etc... then I would consider "Buying American", but until an American Builder can build a real honest to goodness "Mother Machine" (machine capable of reproducing itself), I'm not interested. BTW, Mori Seiki does not use machines that are not their own in Japan with the exception of machies that they do not manufacture. ex. they need a 90' bed on a machine that has 5 sided machining capability to machine the castings, obviously they do not make one of those so they got one from another builder - Ingersoll. Stuff like that, otherwise all the machines in the factory that make components , spindles, etc... are Mori Seiki. I would venture to say that very few builders in the world can make this boast.

That's my story and I'm sticking to it.

[maestro]

If anyone needs help with the chip thinning issue, the Iscar guys in Arlinton, TX. have a nice RCT calculator done in Microsoft Excel format that works great. Contact them or email me and I can email it to you. They supply this to customers at no charge.

[RAJ]

OH STAINLESS,i was cutting a2-tool steel wirh those parameters.

[Smit]

Thanks for all the very good input. We're going to try an Iscar Heli2000 1" mill (3/4" shank), IC328 insert, 300SFM, 21IPM, .1875 depth of cut, 3/4" width of cut, milled dry, and adjust it from there. This is well above the range that the Iscar rep recommended I try. I'll let you all know how it works out!

Thanks,

Larry

[RAJ]

i think tirenut knows his job,i wouldnt listen to ur rep too much.

 

try wat i said it should work fine

i use those parameters on a fadal 4020 and it works well

[Smit]

FYI: We ran a test on the 440SS with our Iscar Heli2000 mill @ 1850RPM, 60IPM, .100 DOC with limited success. It sounded good for a short time and then the inserts chipped. We settled on 300SFM, 21IPM (.006 chip per tooth) and .300 DOC. It ran well through the part and the inserts still look good. So in the future we'll experiment to see how much more we can get out of it. I'm really puzzled that the Iscar rep wasn't able to help out a little more. It's a pretty major thing for a tool salesman.

Once again thanks for all the input.

Larry

[mcrae_andrew]

Brett, Raj, Larry and all the rest.

Great information here on Cutting Parameters. My complete disapointment in 90 percent of the sales people in the area comes from my personal experience. We can see here that the Iscar Rep for Larry has suggested an insert grade that is at least 10 years old and there are several newer Iscar alternatives(IC928) that will work even better. I have been spoiled with the best concentration of Sandvik Talent in North America (South Western Ontatio) and these guys know how to make tooling cook.

Brett - I would like to thank you for such a great posting. There are a few people that have done their home work. Lets start a new post on torque(FPT), HP and RPM.