Where to start? The answer to your question is... "it depends". Depends on the workpiece material, the type of tool and the PVD coating used on the tool. For your aluminum milling, you will want to flood and stay with coatings other than TiAlN. On some softer/gummier stainless steels, you will also want flood coolant. Same goes for titanium and nickel based alloys. On some of the harder grades of stainless however (or hardened stainless), you should run dry (with air blast) and using a carbon-nitride or aluminum-nitride coating. Any TiAlN coated tool should be run without coolant, as the coating needs the heat to provide that useful layer of aluminum oxide. On materials 40 HRC or better, TiAlN is the only way to fly IMO. On ballnose cutters, especially end mills, you will want coolant if surface finish is paramount. So it depends but you TiCN coating is much more forgiving than TiAlN. I'd still stick to dry machining unless you notice BUE on your cutting tools. -Chuck

Great advice on the runout and using a larger drill. I'd step up to a #53 drill (.0595) which should put you at 55% thread and you don't need any more for the length of thread engagement you likely need. I would slow the tool down to 30 sfm and use a .0008 IPR starting point. Peck .015 to keep the heat at the tool tip down. Yes, cobalt or better would have been better but if you're strapped for time, you've gotta use what you have. Been there. Do check with local tool suppliers and see if they have a #53 screw length drill in cobalt. May be an "in stock" item. Never had to drill that small a hole in 316L so I don't envy you. Hope this helps though. -Chuck

I don't get the recommendation against using them with ceramic bearing spindles. If you're lucky enough to have a machine with ceramic bearings then you get a spindle with better stiffness and ridgitity. I could perhaps see an issue with extremely high rpm, but with these cutters you'll probably never exceed 4000 rpm. So I don't get it... then again I'm not a mechanical engineer. This is the Toshiba cutter going to town in some low carbon steel. http://www.usshoptools.com/current_year/wh...ideo%20mpg1.mpg Mitsubishi has videos of the AJX on their website if you'd like to see it in action. -Chuck

I use thru-coolant-drills all the time without coolant.. sometimes drilling dry instead. You shouldn't have a problem unless you're working some really gummy type material. No peck cycles necessary. Take care, Chuck

Is the part something you could set up easily in a 90º or set of 90º v's, then cut your v-channel with a "flat" end mill? Just though I'd ask, cause that may save you a lot of grief. -Chuck

The typical process for achieving a thin walled part is to pocket all areas to equal depths, stepping each to the same depth each time. If you want to add a finish pass at each depth, then that's easy enough to do (don't need a pocket, just a wall cut unless you're at last pass). If you use good rigid tooling you may find that a finish pass is not necessary. Just depends on what you are trying to achive finish-wise. Pocket from center out, use climb, use a morph "spiral" toolpath if HSM to cut down on decelleration time. We cut 7075 and 6061 all the time using this approach. OSG Blizzard 1/2", .0125 IPT, .2-.25 doc and Stellram aluminum routers (3/4 & 1" dia) at ~140ipm and 10,000rpm. Good luck. -Chuck

Other than a few odd balls here and there, this place is great. Still trying to figure out the weird connection so many Mastercammers seem to have with "Winnie the Pooh". That and putting "teh" letters in the wrong order on purpose but hey... whatever floats the boat. That's all I can complain about right now so I'm doing pretty damn good. lol Best not to take things too seriously on the internet. I agree with you though... people are real quick to correct but keep in mind that it aint exclusive to this forum. It's a netwide phenomonon and probably more so from the youngins than anyone else. Hell, I'm just happy when I can read through something one time and get it! I could care less about a few misspelled words here and there. Best to follow the advice Dale Carnegie gave so many years ago on dealing with people. Just expect them to be at some degree of egotism and defensiveness... not to mention, everyone wants to be important. So, handle with kid gloves. lol Take care, ChuckM

Ahh, "small" and "large" are all a matter of perspective. The company I use to work for machined features as small as .015 wide on a regular basis. Now everything I work with is 3/8" and up. Doesn't really matter one way or the other... other than issues with TIR and getting enough sfm to be productive. Charlie Pierson makes a real good point about his findings with TIR. If you do a lot of small tool milling, might be worth looking into a toolholder like Lyndex's "Bullseye" etc and nip that stuff in the bud. I am of the school of machining which would suggest the largest depth of cut possible in this case. Don't think horsepower will be an issue. If you run .010 doc, you're gonna need to go 36 ipm to equal the metal removal rate you could get at .030 doc and 12 IPM. So it's always important to look at MMR when estimating the productivity of an operation. I do this a lot when looking at different milling operations.... quite revealing. If you can get away with 1xD in doc like Degmc has had success with... do it! I would take a serious look at the reduction in cycle time versus the cost of replacing the tool. It may very well save you money to change the tool after every part. Never know til you crunch the numbers. Good luck. -Chuck [ 12-29-2004, 08:03 PM: Message edited by: ChuckM ]

Use a coated carbide... TiN at a minimum and TiCN or TiAlN depending on the type of cut. You'll likely want as much rpm as you can get. At something like 10000 rpm, you're 3/32 end mill is only achieving ~245 sfm. If you can achieve 300+ sfm for carbide, that will help boost your productivity. +1 to the 3-flute recommendation and using a short LOC. Robbjack makes a very economical 3-flute "Tuffy" end mill and other companies offer something similar. I would run a chip load somewhere around .0004-.0005 per tooth, 20-30% of diameter in axial depth of cut. Use your best tool holders (least TIR) and high pressure coolant or cold air. Good luck. -Chuck

Sp3 is a good call as is the Exocarb Diamond lineup from OSG. Been very happy with both. -Chuck

Definitely look at Mitsubishi's MZS for a through coolant spindle. You can run 375-400 sfm all day long with the MZS in 4140, no pecking and well filtered coolant. +2 on checking the runout. Good luck, Chuck

+1 to Storkman on RCTF... That's a lengthy calculation when you're wanting instant answers. Buy yourself a Casio graphing calculator (~$30), write a program and forget about the math. Only need to do it once that way. Does dumb you down a little bit though. lol -Chuck

Nah, I'm laughing at all of them that can't do it but it's a lighthearted laugh so no need to take offense Thad. Esprit (which I'm currently using) tries to do multiple undos but you never know what you'll get. Humorous and frustrating at the same time. -Chuck

Use what the manufacturer recommends. OSG, SGS, Robbjack... they all give very specific recommendations for chipload and sfm starting points. Robbjack even has a nifty calculator on their website based on their cutters. I have my favorites but one thing I can't deny is the fact that our local SGS guy is really up on his cutting tools. If I have a question, he has an answer. If it's something he's never dealt with personally, he'll buy a chunk of material and experiment with it to establish a knowledge base. That's pretty cool in my book. I'm still not totally sold on SGS, as I feel their are better cutters for some applications but that just goes to show that a good rep can be a valuable source of information. -Chuck

Good luck with your pursuit Mick. Choosing a CAM package can be a daunting task but you're right... if you ever got stumped, you couldn't hope to find a better answe than you'll get right here on this forum. Post your problem-file up, let everyone take a look-see and get a quick answer to your questions. What more could you ask for. I understand that Gibbs finally got around to building a forum. It was a hot topic of discussion here a couple of years ago at the annual users meeting. Now if they could just fix the software for more than one "undo". One other slick feature Gibbs had that I never really got around to setting up was its "hole wizard". You could set up multiple parameters and equations that would automatically create tools per given hole "type". Say you needed to make 20 5/16-24 tapped holes... it'd pull a center drill, letter "I" drill and a chamfer tool to create all the holes based on specifications you set up for that particular type of operation. Pretty slick, but like I said... I just never got around to using it as it was a rather dedicated effort in setting all the parameters and I never devoted the time. Have a good x-mas. -Chuck

CMR, Give Stellram a look. http://www.stellram.com/Company/Library/Videos/5702.mov Just finished up a big 7075 aluminum job using their "routing" cutters. 3/4 & 1" diameters, .2-.3" doc 10,000 rpm and .007 ipt on new 40 taper Haas. These things really fly. The Mitsu BXD might be the cutter you're after. They move aluminum real nice too. -Chuck

Man this forum moves fast! Thanks for the information Rob. I personally love every Mitsubishi cutter I've used and you can't beat the warranty policy. CMR, the materials will be A2 tool steel (we cut A2 frequently), 4140 and lots of carbon steels like 1050. We work in a very large variety of materials.... some I hate with a passion, but that's another subject. Gotta make quick work of this stuff and need to do it reliably. Have used the Iscar Feedmill and it is fast but the insert life is not so predictable. The Mits cut nice, don't put alot of heat into the workpiece and insert life is very predictable. Looks like they're going on our 40 tapers here real soon. Thanks again guys. -Chuck

The Urmas are nice but my personal favorite is Walhaupter. Might want to give them a look before you buy. Had a nice article in the latest Cutting Tool Engineering Magazine (I believe). If you're interested I can scan and send. -Chuck

Yep, all the wrong people making the decisions.. doncha just love it? 1st CAM ackage I worked with was Gibbs. We went through maybe 10 demos and my personal choice was Mastercam (I was to be "Lead programmer") but I was vetoed by the head of our engineering department. A guy who'd never written a single line of NC code, lol. Gibbs is not a bad CAM package. I like it alot better than some others that's for sure, but one thing that will irritate you real quick is it's rendering engine. Try a rotation and she starts all over just like Mike said. And forget about gauging surface finish from the render... doesn't matter if you have .00001 cusp height it still looks like hammered dog doodoo in tight. No real options for lead-ins and lead-outs. Ok, what line length and radius do you want cause that's all you get unless you geometry it in. No "smoothing" at the ends of surface cuts. Little stupid stuff that will drive you crazy til you figure it out like..... say you rough a pocket with a 1" x .125R bullnose end mill, then you want that tool to "start" .050 above that floor surface for a finish cut. You'll get a big surprise when it cuts your vertical walls. It's now cutting into them .125! No biggie if you know to start more than the radius above that finish floor. .126 or better yields a good toolpath, lol. Now that one had me scratching my head for a while 1st time 'round. No tool library as mentioned above but you can save "processes" that you use all the time easily enough. Overall it's a good CAM package. It's intuitive and easy to create parts with but at the same time it lacks options and for us control freak programmers that can be frustrating. MC is by far the more powerful software, especially when it comes to surface cutting. I'd go with MC and be done with it... it's up to any task you can throw at it. Let your experience be a limiter (you can work that part out), not your software. Good luck. -Chuck

Hello gentlemen. I've used the AJX on a 50 taper Mori and the thing worked beautifully but I'm now working with Haas VF2s and 40 taper tooling on Haas' spindles. So, is anyone using these "high feed" cutters (1.25-2" diameter) with success on their ~25hp machining centers? Have a job coming up where I could really utilize one and although I like the Haas mills fine so far, I'm use to working with beefier machines than these. Your input is always appreciated. -Chuck [ 12-12-2004, 08:58 PM: Message edited by: ChuckM ]

Almost everything I wanted to ask was in Budgie's reply. I feel you'll answer your own questions on this matter when you look at the capabilities your shop really needs. As far as solids design goes, I choose Solidworks any day of the week and twice on Sunday. I've done solids in a multitude of CAD packages and I was plenty happy to give up designing them with Boolean functions and setting up new workplanes for every feature. Anyone who says they can do solids faster this way has got to be smoking some good ganja... either that, or they aren't anywhere near proficient enough with their Solidworks, ProE, etc.. Fixture design with multiple components is also a real breeze in Solidworks as you can utilize mating functions to place your tooling. If you have a modular tooling system and have a library of these components, things get even better. Build your fixture in SW, print out a setup for your operators, import the assemblyt into your CAM package (Parasolids are fine) and machine your part knowing exactly where every component is located. I do 90% of my programming this way utilizing modular components. All goes back to the type of work your shop does. Good luck. -Chuck

I agree, RPM aint the problem. We just finished up a job drilling hundreds of .078" diameter holes in 1018 steel at 40,000 rpm with one of Air Turbine's spindles. Run-out will destroy small tools, especially carbide. Until you fix it, you can expect a lot of tool failure. Nail that down, go with the much more rigid circuit-board-style drill mentioned and you should be fine. -Chuck

Hardmill, We use Haas VF2, 3 and 4 machining centers. The 2 and 3 have the 20hp delta spindles (10,000rpm) and the 4's have the optional 2-spd/high-torque gear boxes on them. All are CAT40. I come from a shop that was all Mori, Makino and OKK but so far these Haas haven't dissapointed me too much. Especially when you look at their sale slips. I should also mention that the deepest full-tool cut on any of these parts would be 1/4" max as none of the pockets are any deeper than that. They'd also be very rigidly fixtured. A couple are actually vise/block-stock jobs. Thanks for any help in advance. -Chuck

quote: Welcome to the forum ChuckHey, thanks for the welcome Hardmill! Take care, Chuck

Hello gentlemen! Ok, this is one of those materials I'd never even heard of until we were asked to provide a quote to one of our prospective customers. Stuff's heavy in cobalt (~48%) and I haven't found much info on machining it other than a 25-35 sfm recommendation (double that for carbide). So give me a shout if you have anything to say about Hiperco 50A, I could sure borrow on someone elses experiences here. 95% of this quote will be mill work. Thanks, Chuck