[bala955]

would like to machine block of 316ss machining parameters 1-1/8"deep 1/2"endmill 4fl 1-1/4"flute as truemill what feed and speed to use fadal4020 cat40 machine

[davereagan]

I have never gotten good life from carbide in stainless. I'd rough it out with some coated cobalt roughers at 750 rpm, good soluble oil flood coolant and .002-.003" feed per tooth. Then finish the last .010" on the side with your Power Feed at 2500 rpm and .002-.003" feed per tooth depending on the finish you need. Dry on the finish. 316 is 304 with the addition of 2% Molybdenum, so it work hardens very quickly and is hell to drill. Never just rub or feed too lightly.

[Jason S]

would like to machine block of 316ss machining parameters 1-1/8"deep 1/2"endmill 4fl 1-1/4"flute as truemill what feed and speed to use fadal4020 cat40 machine

You can go on Surfware website and see some of their case studys and kinda determine what you want to run. Rule of thumb from what I been told is double your SFM, triple your IPT. Also depending on your part setup rigidity and air blast. All else fails, contact your reseller the will help the most.

[lkenney]

I don't do much Stainless but I would start with a 1/2 TiALN coated carbide endmill at about 6000 rpm and 50 ipm, NO coolant but air on the cutter. Any Coolant will shorten the life of the TiALN Carbide end mill very quickly. I even blow off coolant left from drilling before starting the truemill cycle.

I would take the depth in two passes with a finish wall cut 0.005" with Truemill. If the floor needs to be smooth, I would hold off about 0.010" and finish with a normal pocket cut.

I would adjust from this point. You could very well end up at 9000 rpm and 100 ipm. I usually don't cut deeper the 1.5x diameter in a single pass.

Look at your chips they should be coming off gold to blue in color. Don't let the chips build up in a pocket, they hold heat and recutting will lessen the life of the endmill.

If you use a SwiftCarb True-Mill endmill you can plunge faster and push for the higher end of things. Swift can give you more info. Let us know what works for you.

Lowell

[Maguillacutty]

I don't do much Stainless but I would start with a 1/2 TiALN coated carbide endmill at about 6000 rpm and 50 ipm, NO coolant but air on the cutter. Any Coolant will shorten the life of the TiALN Carbide end mill very quickly. I even blow off coolant left from drilling before starting the truemill cycle.

I would take the depth in two passes with a finish wall cut 0.005" with Truemill. If the floor needs to be smooth, I would hold off about 0.010" and finish with a normal pocket cut.

I would adjust from this point. You could very well end up at 9000 rpm and 100 ipm. I usually don't cut deeper the 1.5x diameter in a single pass.

Look at your chips they should be coming off gold to blue in color. Don't let the chips build up in a pocket, they hold heat and recutting will lessen the life of the endmill.

If you use a SwiftCarb True-Mill endmill you can plunge faster and push for the higher end of things. Swift can give you more info. Let us know what works for you.

Lowell

Nice, thanks for the tip.

Maybe you can help me out with this one.
I seem to be blowing threw inserts every 4 parts. I am machining Alloy 88. This material is new to me. I am using surfcam velocity 4 b189. I am treating the material as Low Carbon Steel 5-20rc. Using a simple Face mill toolpath..
I have .610 worth of material to remove. I am using a 3 inch shell mill taking .075 depth of cut, S1200 F22.ipm These inserts blow balls I think, they are ingersoll brand Grade IN1030 whatever that means. Not sure about these inserts.. Boss man handed em to me.. He doesn't know much about machining that is for sure lol..

Hoping you can recommend what kind of inserts I need for this application. Speeds, Feeds, depth of cuts etc would also help. This really blows lol

[davereagan]

lkenney: At the risk of sounding rude, are you out of your mind? The speeds you recommended are double the starting parameters SGS gives for mild steel, which is twice as fast as stainless should run. I see a lot of guys on here recommending 500, 600 even 700 sfm in mild steel with TiALN cutters, but I have to see one say they are doing more than tickling the part with a million lines of code. Taking a full slot one full diameter deep, I run 400 sfm in 1018 steel and get good tool life. I would probably run in 304 stainless at 200 sfm in heavy cutting and 300 for finishing.

[lkenney]

Maguillacutty, I have not done much insert cutters, my work is usually small so I am afraind that I can't help there much, sorry.

davereagan
I made a suggestion, admitted that I don't cut much stainless but what i have done and what I see from others using Truemill this is doable. Truemill never buries the whole end mill in the cut and we do tickle the work with a million lines of code and laugh all the way to the bank with faster production and longer tool life.

Over on the Haas forum there is a good discussion about this style of milling and some insert info was given there, GEOF started it and it called "now I belive ---"

Lowell

[davereagan]

Lowell, Maybe I envy those with nice CAM systems, but I do wonder how long a machine lasts when you make hundreds or even thousands of reversals on the ways and ballscrews just to get one slot when a variable helix endmill run correctly could do it in one or two passes.

[lkenney]

Dave, I have wondered that also but my load meters never go over 50%, the machine sounds and cuts smoother than i have ever had it and I am using an old 1992 VF-0 Haas and cutting steel with ease that I was not able to with other methods. Also I don't use Truemill for everything and often finish the bottom of a pocket with a shallow pocket routine as that leaves a better floor finish. It is a tool that works for us. On steels I use nothing but carbides but often they are just run of the mill no-name tooling. I even have a couple of vendors on E-Bay that I buy from. Tooling and packaging is the same as what I pay local tooling houses 1/3 more for. It is not how long a tool lasts but how many parts can the tool make.

I had to unlearn a lot of gospel before I could really make it work. With 64K of RAM I sometimes have to drip feed it.

We never program on the machine, I have seen away too many crashes from that and I like to visually check my paths by running the model. I am only running an 2-D version of SurfCam with the Lathe module. We have had the softwear since 2001.

TrueMill open a lot of business for me that i would not have bid on before as well as allow us to manufacture products for our own production that we could not produce without it.

I do not see how a machine shop can compete in this tight market without a good CAM package. I Think that you can buy 2D SurfCam for about 2 weeks of a single CNC Mill's time and than annual maintenance is less than 3 days.

Sometimes when we are runnig full scale I will bring in some one to put and pull material on the mill while I program but I often do both. My office is just a few feet from the mill and I can hear it very well.

We are an R&D shop so our runs are short and always changing. I visited a shop the other day that had one VF-2 making one part 2 shifts a day 6 days a week and had been for several years. that is a vastly different business than i operate under.

Truemill does require more time blowing chips out of pockets but I am trying to get time to install a airpipe that will keep the cutter clear when cutting.


With the changes in the market I believe this is a time to review all our processes and find out what is new and what will improve our production. There are new tooling, different holders, new softwear, coolants, fixtures that need to be reviewd and processes changed to make us more effiecient if we are to survive.

That is my soapbox for today.
everyone have a good week.

Lowell

[davereagan]

It's interesting how we all adapt. For some of the simpler jobs I do, I kind of laugh to myself with this scenario: In another shop, a guy is just coming over to the machine after programming the part on a CAM station and he's ready to cut. In a split screen, I am taking the finished part out of my machine. This would be for a part with a few holes and a couple of slots. The Imco Power Feed mill is made for heavy slotting. I do believe your machine could do it, although I've never run a Haas. I am positive your Haas could atleast handle a 3/8" endmill cutting a 3/8" deep slot and I think it could cut a 1/2" deep slot with a 1/2" endmill. I've watched a few videos and read a lot of posts and it frustrates me when people swim halfway across the English Channel and decide they can't make it so they swim back. What I mean by that is they get the awesome endmill and then hang it out a mile in a 2.5" or even 4" gage length holder. The inner diameter of the spindle of a lighter 40 taper machine is 60mm (2.362") Why would you want to be 1.5 diameters away from the top of your tool? Then you are over 2 diameters (in terms of spindle diameter) from the cutting edge to the bearing. Of course it will sound awful if you aren't tickling the part. US Shop Tools has holders with 1.38" gage length at really good prices. They also have an ER32 collet chuck made by Techniks that has a 1.13" gage length. Now, even a light machine can cut. I learned these things because my machine has a light head and sings in one particular quadrant when I am interpolating. When I first bought my machine, I had standard 4" length holders and I couldn't take the depths of cut I had been taking on my Bridgeport knockoff with a 3 flute face mill.
So Lowell, what holders do you use? Have you tried full slotting with one of these variable endmills dry in steel? I worked up to it in steps. I had a 3/8" SGS Z carb and I even called them and said "I'm about to try exactly what you brochure says. Are you going to take the tool back if it breaks?" They said yes. I ran the 3/8" endmill .187" deep in 1018 CRS at 4000 rpm and .0015" feed per tooth. It ran great. Then i ran a full .375" deep slot. Ran great. By the way, if you run under .0012" it will sound like it's about to break. It quiets down when you feed it right. Then I ran a .550" deep slot with that 3/8" endmill at .0012" and it ran fine. That was enough for me to see I was safe running 3/8" slots all day. Below is the IMCO catalog. Page 9 gives feeds and speeds for the Power Feed. Notice it says 350sfm for heavy slotting in steel. 275 for stainless which I still think is high. I don't think they would put these endmills out with full diameter slotting recommended if a Haas machine couldn't handle it. Haas outnumbers just about everything these days.

Dave

http://www.imcousa.com/catalog/downl...talog_2007.pdf

[lkenney]

Dave,
I am running a mix of new and old holders, about half are Bison, ER16, ER25 & ER 32 with a few fixed dia tool holds. Most are fairly short, you could find at least one of oll the rest of American tool holders in the rest. Top RPM is 7500 and the spindle motor is a 5HP rated at 7 1/3hp for 30 minutes. Modern Machine Shop did a story on our shop in this April's issue.

We make a lot of M1913 (Picatinny) rails in 1018 steel. This drove me nuts and was very expensive. Another firearms manufactuer told me what they used. I could not believe it. It was my first fast and full cut without coolant.
The recipe went like this. An TiALN Coated Iscar 3 flute 3/16" Dia Carbide with 3/8" LOC running at 4000 RPM and 20-30 IPM no coolant at 0.125 deep, one cut. It Cut like butter,

I went to carbide inserts on a Dual 90 degree 3" cutter 3 inserts running dry and fast and a 1/2 TiALN carbide to trim width with and cut my production time to 1" per minute on 1" Square stock, a 1/3 of time it was taking my contract shops to produce. I am changing end mills about every 8-10 feet of bar. we make about 30 grooves per foot of rail. Load meter stays at 25% until the end mill is shot then jumps to about 30% and that is when I change.

I understand that thise who program at the machine often can do so very quickly, but I also have seen some very expensive crashes when a number is keyed in wrong. In fact my lathe machinist just crashed a $400. tool and knock the turrent out of alignment when a number was transposed as a correction in the program. It took us a day to get it back aligned and we are waiting for a new tool to show up so we can redo that job. I can't fire her as we have been married 39 years as of yesterday. I don't have it in me to train another one. LOL

Lowell

[davereagan]

That sounds painful. Check out these videos....

Watch this whole thing. They eventually go 2 full diameters deep and they are even going against my mantra of a short tool holder. Must be a super rigid machine.

[ame="http://www.youtube.com/watch?v=Vb_pwFm6W9A"]YouTube - LMT DHC Variable Helix End-Mill[/ame]

[ame="http://www.youtube.com/watch?v=H1J5XauCw74&NR=1"]YouTube - 1018, 1045, 4140 24 HRC NX-FP 708 SFM Fraisa end mill[/ame]

[lkenney]

Here is a video by Helical tools in 316 SS at higher feeds and speeds that I recomended.

[ame="http://www.youtube.com/watch?v=5apL5FhW2Wk"]YouTube - Helical Solutions Video 316 Stainless Running at 150 IPM[/ame]

Your videos were interesting also.

Lowell

[lkenney]

Maguillacutty,

Alloy 88 seems to be more like stainless below is info that I found, not sure that this is the same aas you are using. Most sights say the Alloy 88 has a lot of nickel in it. That may be why you are balling up.

Lowell


Machining Recommendations for WM88 Alloy
Waukesha 88 is characteristically a soft, short chipping, material. It dissipates heat poorly and abrades tool materials rapidly. WM88 has low thermal conductivity and requires careful tool selection. When machined it behaves somewhat like grey cast iron, with edge wear the primary mode of tool failure, while producing short and discontinuous chips.

The Waukesha alloy differs from cast iron in that more rapid tool wear will occur and surface footage should be less than that of cast iron of similar hardness.

Tool Materials - Generally, cast iron grades of carbide are the best tool materials. C2 carbides work well on interrupted cuts and for roughing. C3 carbides work well for light finishing cuts. Coated carbides to date have not been cost effective. Honed edges produce poor surface finishes and grades evaluated are no better than uncoated C2. High-speed tool steel is often successful; however, with rapid tool wear common.

Coolants - Waukesha 88 can be machined with or without coolant. If coolant is used, an ample supply must be available and applied directly into the cutting zone. Most water-soluble coolants are adequate.

Specific Processes - For turning and milling, use C2carbide, negative rake tooling. Start at 300 - 450 surface feet per minute. Set a feed rate of 0.008 - 0.015 inches per revolution for roughing and 0.003 - 0.006 inches for finishing. Single point threading is recommended for threading and tapping. Use carbide tipped drills whenever possible for drilling.

NOTE: The Waukesha 23Bi, and 54C alloys exhibit somewhat similar machining characteristics. For specific recommendations, please contact Waukesha Foundry.

[davereagan]

I know how nasty 316 is and therefore, your video is far more impressive than mine were. Both the cutter and machine are awesome. If they had gotten rid of that slow plunge rate on the outside the video would have flowed better, but that just makes us all start thinking of how we could knock another 30 seconds off. Because stainless work hardens, I think this radial cutting, high feed method is better justified. Cutting a full width in even 304 makes the cutter and material red even at a third of the speeds shown. The endmill needs a cooling break and an interrupted cut. A while back, I noticed in Machinery's handbook that generally stainless has half the thermal conditivity of regular carbon steel. I think this accounts for a lot of the problem with heavy engagement in stainless. The heat builds up at the cutting edge like a thermos. Add to that the work hardening from the 2% molybdenum in 316. Anyone doing this kind of thing with 6Al-4V Titanium?

[lkenney]

Dave,

here you go

[ame="http://www.youtube.com/watch?v=xr_km46BbJo"]YouTube - Surfcam - TrueMill - High Speed Titanium Machining[/ame]

Lowell

[lkenney]

My operational goal is to be able to keep the spindle running nearly all day long. In my vision (trying to match Dave's here)

I see me finishing a job, uploading the next one that was created during the previous run, changing the vise soft jaws, replacing tools resetting zeros and running a test piece, checking the specs making finals and then setting up in a short production run, while I create the next gcode program, order some tooling, check on some bids, while picking and putting parts in the Mill.

1st and 5th go to qc for checking then every 10th is check by my QC person (wife) who is an expert at finding things that I do wrong. only now it pays!

She will also pick and put as she has time between the lathe and the QC work. I do check her production just so two sets of eyes have measured the parts.

One bad part is that I am hard of hearing so I have to issolate myself when I am on the phone to be able to hear.

Hope everyone had a great weekend.

Lowell

[Maguillacutty]

Maguillacutty,

Alloy 88 seems to be more like stainless below is info that I found, not sure that this is the same aas you are using. Most sights say the Alloy 88 has a lot of nickel in it. That may be why you are balling up.

Lowell


Machining Recommendations for WM88 Alloy
Waukesha 88 is characteristically a soft, short chipping, material. It dissipates heat poorly and abrades tool materials rapidly. WM88 has low thermal conductivity and requires careful tool selection. When machined it behaves somewhat like grey cast iron, with edge wear the primary mode of tool failure, while producing short and discontinuous chips.

The Waukesha alloy differs from cast iron in that more rapid tool wear will occur and surface footage should be less than that of cast iron of similar hardness.

Tool Materials - Generally, cast iron grades of carbide are the best tool materials. C2 carbides work well on interrupted cuts and for roughing. C3 carbides work well for light finishing cuts. Coated carbides to date have not been cost effective. Honed edges produce poor surface finishes and grades evaluated are no better than uncoated C2. High-speed tool steel is often successful; however, with rapid tool wear common.

Coolants - Waukesha 88 can be machined with or without coolant. If coolant is used, an ample supply must be available and applied directly into the cutting zone. Most water-soluble coolants are adequate.

Specific Processes - For turning and milling, use C2carbide, negative rake tooling. Start at 300 - 450 surface feet per minute. Set a feed rate of 0.008 - 0.015 inches per revolution for roughing and 0.003 - 0.006 inches for finishing. Single point threading is recommended for threading and tapping. Use carbide tipped drills whenever possible for drilling.

NOTE: The Waukesha 23Bi, and 54C alloys exhibit somewhat similar machining characteristics. For specific recommendations, please contact Waukesha Foundry.

Yep that is exactly where the material comes from waukesha.. Lots of nickle. thanks Lowell. I just got off the phone with one of the fellas over there.. They dont seem to know much about machining tho lol, just about there material and the tooling listed.. Not much help. I am using a Cobalt 2 inch Hogger for ruffing the inside of the casting after the 2inch Shell mill clears a majority of the material..
these are some nasty castings. man this **** is just killing my inserts.. I have been messing around with it all weekend.. Got it a little better.. But this 105 deg heat outside don't help either.. Hehehe I like using Truemill for my ruffing.. I keep the tool engagement at 50 deg. with .075 depth of cuts Using a 2.0 shell mill for ruffing out material, S1200 RPM F25. seems to kick ass but only for 3 parts. I guess thats cool being I am removing .610 worth of material. Might try some coated carbide EMs for finishing just not sure what kind of coating would suit my needs best.