Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: HimyKabibble on January 17, 2010, 12:21:17 AM
-
I tried to machine some 6061-T651 wrought plate today, with rather disastrous results - four broken/dulled endmills later, I'm stumped. If I go fast, the tools load up and break in seconds. If I slow down enough to not get chip welding, the tool edges get destroyed VERY quickly - I ruined two brand-new high-quality HSS endmills in less than 24" of cutting each. All the cutting edges were absolutely destroyed. How the heck do you machine this cr@p?
Regards,
Ray L.
-
Ray, I've used 2 flute Carbide with flood coolant and gotten pretty good results. Coated carbide does a little better. Can't remember using an HSS. What kind of feeds and speeds are you running? Cutter type, diam. and number of flutes? Make sure nothing is vibrating.
Brett
-
Ray, I've used 2 flute Carbide with flood coolant and gotten pretty good results. Coated carbide does a little better. Can't remember using an HSS. What kind of feeds and speeds are you running? Cutter type, diam. and number of flutes? Make sure nothing is vibrating.
Brett
Brett,
I started with a 1/2" 3-flute carbide, 5000 RPM, 0.325" DOC 30 IPM, heavy mist coolant. It loaded up and broke almost instantly. I then went to a 1/2" HSS uncoated 2-flute, 3100 RPM, 0.175" DOC, 10IPM, very heavy mist coolant. It didn't load up, but the cut quality was awful, and after cutting about 24", the tool was destroyed.
Regards,
Ray L.
-
What's odd is, I cut some smaller features, using 1/8" and 3/6" uncoated HSS 2-flutes, 8K RPM, 10 IPM, and they came out OK - Not great, but OK, and the cutters didn't seem to be damaged.
Regards,
Ray L.
-
Hey Ray, I get 4584 RPM for the 1/2 HSS 3 flute at 41.26 IPM.
See if this link helps you any.
http://precisionchaos1.com/support.htm
Brett
-
Hey Ray, I get 4584 RPM for the 1/2 HSS 3 flute at 41.26 IPM.
See if this link helps you any.
http://precisionchaos1.com/support.htm
Brett
Brett,
The HSS tool is a 2-flute.
Regards,
Ray L.
-
Wasn't the titanic made of that? 5140???
-
:o 5000 Rpm? O>MG
-
Might be the type of coolant your using. I have NEVER gotten satisfactory results using anything other than an oil soluble coolant with aluminum. Looks like motor oil, then milk when mixed. Usually, I can get pretty aggressive with the cut, too. Coolant like koolmist or similar water based coolant is pretty much horrendous. Maybe I've always went about it all wrong, but that's my limited experience with cutting aluminum. I've never tried 5K. Might need more of a flood than a mist, additionally. I'm no expert with aluminum, so take all above with a grain of salt.
-
Kool Mist is not good in my experience. I have tried a couple of lubes, but keep coming back to tapmatic tapping fluid. They now have an aqueous version that is not specd to be diluted, but I cut it about 3:1 with water and put it in a spray bottle with very good results, but for anything heavy, I still have to fall back to the tapping fluid.
Cutting tools . . . think in terms of chip load and not IPM. I have just completed my new mill and have not cut anything with it yet, but with my previous mill, all I could get was .001 per tooth before trouble started.
HSS if fine is the tools are excellent quality and have a smooth bright finish and are razor sharp. My experience with el-cheapo import cutters (Grizzly, etc) is exactly as you describe. Using a brand name cutter makes a huge difference.
There are some cutters that are made especially for aluminum with a higher helix and special coatings that prevent the dreaded build up on the tool. Once the aluminum melts and attached to the cutter you have only seconds before the tool snaps, so you usually wont get the chance to stop and clean the cutter.
Bottom line is you have to have sharp tools and keep them cool. Blow air on the cutter constantly to keep it cool, with or without mist. The MOST important thing is chip load. If you get that right, then the vast majority of the heat will go overboard with the chip. If you get it wrong, the heat goes into the workpiece and the cutter.
Oh yeah and the two most important words in aluminum cutting: climb mill.
-
Have only ever machined 5083 due to the work I do (marine) but have always used flood coolant and its fine, bought a mister to try and cut down on the mess but found it a waste of time even when using the same water soluble coolant in it that I was using with the flood.
Hood.
-
6061 ranges from T-0 (soft and gooey) to T-651 in this case (tough and gummy) and flood coolant is what we use along with the appropriate speed and feed or cutters are quickly coated with smears of aluminum that attract more aluminum. Although it (6061) is one of the most used aluminum, we try to stay away from it for machined parts on machines without flood coolant, or a constant stream of a light lubricant such as WD40 is needed - smokey! Heavy mist will work but a short period of starved liquid will become a disaster.
7075 can be cut dry in any hardness and it's similar to mild steel in strength.
-
Ray ,
2 flute, slow it down , and flood it.
-
7075 can be cut dry in any hardness and it's similar to mild steel in strength.
2011 (bar) and 2024 also cut nicely. Like 7075, these very nice to cut after figting with 6061 or 5052 (which is even worse), although that joy comes at twice the price of the 'every day' grades.
2 flute cutters definitely help if you have the power and rigidity to make a big chip. If you look up cutting speed for aluminum in any text older than a few years you will see what is today a very low number. Aluminum is routinely cut many times faster than that today, and one should get their cutting speeds from the toolmaker and also not forget to multiply that by the appropriate number if using cobalt, carbide or coated tools. You will find an indication for 3x to 10x faster speeds. I run my 5/16" and 3/8" three and four flute cutters at 7,500 RPM . . . . only because that is as fast as my spindle would go. My new mill is set up for 8,500. 1/4" cutters are the 'crossover point' below which I go to my die grinder spindle with speed set appropriately up to 28,000 for the really small cutters.
Of course, the faster you go, the more heat problem you have and you start to get into water cooled spindles and stuff like that.
-
7075 can be cut dry in any hardness and it's similar to mild steel in strength.
2011 (bar) and 2024 also cut nicely. Like 7075, these very nice to cut after figting with 6061 or 5052 (which is even worse), although that joy comes at twice the price of the 'every day' grades.
2 flute cutters definitely help if you have the power and rigidity to make a big chip. If you look up cutting speed for aluminum in any text older than a few years you will see what is today a very low number. Aluminum is routinely cut many times faster than that today, and one should get their cutting speeds from the toolmaker and also not forget to multiply that by the appropriate number if using cobalt, carbide or coated tools. You will find an indication for 3x to 10x faster speeds. I run my 5/16" and 3/8" three and four flute cutters at 7,500 RPM . . . . only because that is as fast as my spindle would go. My new mill is set up for 8,500. 1/4" cutters are the 'crossover point' below which I go to my die grinder spindle with speed set appropriately up to 28,000 for the really small cutters.
Of course, the faster you go, the more heat problem you have and you start to get into water cooled spindles and stuff like that.
I was wondering if trying more "high-speed machining" techniques might help. I find it interesting that small cutters (1/8" and 3/16") seem to work fine, at the same RPM, DOC and feed I normally use, but the 1/2", both HSS and carbide, seem absolutely unforgiving, even at greatly reduced feed and DOC. I'm tempted to try a 1/2" endmill running max RPM (8200), shallow DOC (maybe 0.050"), and high feed rate (probably 30-50 IPM?).
Regards,
Ray L.
-
If the chip load per tooth is not exceeded and the cutter is the proper helix for aluminum and lubricated, theoretically there is no top speed.
-
As described, the problem as I see it requires an analysis that is somewhat beyond bobby level, but here it is anyway. For calculating production, you think in terms of the cu.in. of metal removed per minute. Each material has a factor indicating the volume of the material that can be removed per available spindle HP.
Here is an important consideration to keep in mind when deciding on your parameters; SFPM can be all over the map and will effect surface finish and production time, but there is a very wide range that you can use successfully. The same is not true for chip load per tooth. There is a definite 'sweet spot' where the heat goes overboard and the cutter runs smoothly. This is a very narrow range and you will have no success on either side of it. The beauty of CNC is that you don't need to go thru a ton of calculations to arrive at the proper IPM. You just set your feedrate in terms of feed per rev based on the chip load and number of flutes and then run the spindle as fast as your machine will allow (for aluminum). The IPM will automatically be optimized for ANY spindle speed.
Moving on the the analysis; in general terms it goes something like this; lets say you have 'X' spindle power available. You can remove 'X' volume of 6061-T6 per minute. SFPM of the cutting tool indicates a max RPM of 'X'. With that, you calculate the chip load per tooth required to remove the prescribed volume of metal per time. DOC obviously dictates the VOLUME of the chip at the same per tooth feed, and a 4flute cutter can run at twice IPM of a 2 flute for the same tooth load . . . . BUT, that requires a lot more power and if you don't have the available power (or rigidity), then the solution is not to lower the IPM, which I think most hobbyist's tend to do, which will make the chip too thin, but to use less flutes (for the same DOC), or less DOC so that you can maintain the proper chip load.
Quick word about DOC; the deeper the cut, the more of the tool edge you use and therefor the longer it will last per cu.in. of material removed, but reducing the feedrate to get more depth is not a good trade off if it reduces the chip load beyond the 'sweet spot'.
That being said, it should be simple to combine these factors into 'volume per tooth' thinking. This is the basic idea behind roughing cutters. Obviously a 1/2" cutter is going to make a very much larger volume chip that a 1/4" cutter at the same feed per tooth, the effect of which is what is being observed, methinks. In practical terms, on my little X2 I could not drive a 3/8" cutter at a feedrate (per tooth) that was acceptable, so I went to a roughing cutter in that size.
Just my 2 cent's worth . . .
-
Heres what we use 10 hours a day, cutters last months.
Okuma 4VA, big ridgid tool making cnc.
6000 rpm, thats as fast as it goes. Always climb milling.
Ultra synthet (with water) lubricant, we used to use soluble oil/water emulsion. Always flood coolant.
Nearly always solid carbide uncoated tools. Sometimes brazed carbide router bits for special profiles.
Roughing with 16mm rmr, three flute, Sandvick, tagutec, or hanita, stelram. feed 2500mmpm, cut about 8mm deep, full width.
Facing with sandvick 8 tip, dia 125mm, aluminium wiper inserts, 2500rpm, 2500mmpm.
Finish with 2 flute carbide end mill, 6000rpm, 1000mmpm (40ipm), 0.2mm stock finish cut, 5mm step depth for profiling.
Some cutters seem to work better than others. We find 6061-T6 or 6061-T651 to machine quite well. 5005 is horible, 5083 OK and 7075 good.
HSS tools do work at 1/3 of the rpm of carbide but need to be short to be stiff enough.
We always use the shortest tools practical and on deep parts we often use a short tool then a long one for the deep parts at lower feed rate and depth of cut.
Good luck.
-
Simpson,
You're absoutely correct. My mistake seems to have been in mis-interpreting the tool manufacturers chipload recommendations. My assumption was they provide recommended chiploads, but I now think they are more like minimums, and you need to go up from there, and see what you can get away with. I have been running for a long time on values derived by calculating RPM based on SFPM, using the manufacturers chipload to calculate feed rate, then testing to see how deep I could go. But yesterday I instead started with a shallow cut, and greatly increased chipload. I found running MUCH higher feedrate did the trick with the icky material. I can run the same DOC (0.175"), but at a 30-50 IPM feedrate, and get an acceptable result, even without coolant. I need to do more experimentation to come up with optimal values.
Regards,
Ray L.
-
I must be on the ignore list...
-
I machined some 6061-T651 plate on the weekend.
1/4" 2 flute HSS at 4800rpm, 12ipm, flood coolant.
1/4" deep and full width cut.
Ran all day and still had a mirror like finish on the last piece.
Timothy
-
Being a hobby user I use just about any materials at hand, some good some really horrible and have found that the biggest difference is flood coolant and climb milling.
I do try to use highish feed rates.
Mostly carbide tools, some of which are totally inappropriate, 4 or even 6 flute, and the only problems I've had have been when the coolant ran low and stopped, instant clogging and a snapped 10mm carbide bit.
Now that was a loud bang!
Steve
-
I don't need an excuse like "too fast" or "no coolant", I just drop my carbide on the floor or the table and break the edges off....
-
I don't need an excuse like "too fast" or "no coolant", I just drop my carbide on the floor or the table and break the edges off....
Dropping on the floor is so low-tech, and manual. I just let Mach3/SmoothStepper jam the tool through my touchplate, or ram it into the side of the workpiece when probing. :-)
Regards,
Ray L.
-
Amateurs . . ::)
Real pros buy name brand coated carbide cutters . . position them carefully . . . get them up to max RPM . . . and then jog at full speed directly into the hardened vice jaws 8)
-
Here Ya go Ray, the way it's done.....
-
Hey Bill, that looks more like friction stir welding than milling. :)
Russ ;D
-
'friction stir welding', hmmm, could we have developed a brand new and exciting process? Problem is these random results.
-
Oh...its been around a while. But like you say, maintaining consistency with a milling machine would be a problem. ::)
Russ :)
-
Here Ya go Ray, the way it's done.....
Now that's impressive! How did you manage to NOT break it?
Regards,
Ray L.
-
Here Ya go Ray, the way it's done.....
Now that's impressive! How did you manage to NOT break it?
Regards,
Ray L.
Quick on the big red button! We only lost coolant for a few seconds when this happened - 6061 - T6.
You would think that those tendrils of aluminum extruding off the end mill would be delicate - they're harder than the piece that was being cut.
-
That thing looks obscene :P
-
Only experience can give you results like that. Your good Bill. ;D
Brett
-
Hi all i got a nice speed and feed calculator from cnc cookbook .com its in beta testing ive been using it for a while works real well and it also has a lot of other useful gadgets on it and its free.I run production runs in 6061 exclusively and this calculator has worked fine for chip load calc. and feed rates might be worth a try gives you a great starting point and seems to do very well with end mills .I use accupro end mills and i usually use three flute end mills carbide coated on 6061 it gives a better finish smaller chips and no welding i use flood rustlic coolant works great in aluminum .
-
Hi all i got a nice speed and feed calculator from cnc cookbook .com its in beta testing ive been using it for a while works real well and it also has a lot of other useful gadgets on it and its free.I run production runs in 6061 exclusively and this calculator has worked fine for chip load calc. and feed rates might be worth a try gives you a great starting point and seems to do very well with end mills .I use accupro end mills and i usually use three flute end mills carbide coated on 6061 it gives a better finish smaller chips and no welding i use flood rustlic coolant works great in aluminum .
Yeah, I'm using G-Wizard to validate my own numbers. It's a VERY nice tool. I'm now cutting the "gooey" T651 at 100IPM, *without* coolant, and getting a pretty nice finish!
Regards,
Ray L.
-
I don't know what you mean when you say "coated carbide", but I've learned that the usual coatings like TiCN, while good for extended tool life, interfere with the flute sharpness. Any coated tool I've seen had a less sharp edge than that of an uncoated tool. For aluminum you certainly want the flut to be as sharp and smooth as possible to reduce the friction and heat. Thus not coated mills are better for aluminum.
Here is a good article http://www.moldmakingtechnology.com/articles/030401.html , see second paragraph from the bottom.
May be you mean other coatings, designed specially for aluminum? That make the surface smooth?
Daniel
-
I don't know what you mean when you say "coated carbide", but I've learned that the usual coatings like TiCN, while good for extended tool life, interfere with the flute sharpness. Any coated tool I've seen had a less sharp edge than that of an uncoated tool. For aluminum you certainly want the flut to be as sharp and smooth as possible to reduce the friction and heat. Thus not coated mills are better for aluminum.
Here is a good article http://www.moldmakingtechnology.com/articles/030401.html , see second paragraph from the bottom.
May be you mean other coatings, designed specially for aluminum? That make the surface smooth?
Daniel
That depends on whether you're looking for ultimate surface finish, albeit with limited tool life and/or machining rates, or good surface finish with longer tool life, and/or faster machining rates. Coated tools can last much longer than uncoated tools, and often enable MUCH higher feedrates. In a production envinronment, time is money, and tools are money, so surface finish will often take a back seat to tool life and throughput.
Regards,
Ray L.
-
I'm not sure I buy the sharpness argument, as these coatings are literally a few molecules thick.
That said, I agree that sharpness and surface smoothness is key to successful soft aluminum cutting, as I commented previously. The primary reason I like the coated cutters is not for higher speed or production longevity, since I can't cut at what would be considered 'high speed' by today's standards and I do prototypes and not production as a rule.
For those of us who don't have or want a flood system, certain coatings offer a measure of 'anti pick-up' to the tool. So aluminum behaves more like an egg in a 'teflon' coated pan rather than a steak on the grill, often allowing dry machining with only compressed air for cooling and chip evac. Uncoated cutters always need lube of one kind or other, in my experience. For those with flood cooling, the debate is somewhat academic. Many moons ago I had a bridgeport with flood cooling and you really didn't even have conversations about material 'welding' itself to the cutters . . . on the other hand, I wan't cutting any soft aluminum back then.
The caveat with uncoated cutters on aluminum is that you *might* get away with a dry cut . . . . and you might not. The trouble is the way you find out that you didn't . . . which can get expensive in a hurry. I may as well add once again that in my view, mist 'coolants' like Kool Mist that I have tried are no better than dry cutting for soft grades of aluminum, however, something that I find very effective for band saw blades is 'grinder's paste'. This stuff is pretty miraculous at keeping aluminum from sticking to saw blades and grinding belts . . . . . just don't use it for final finishing if you plan to paint the part afterward.
-
I'm not sure I buy the sharpness argument, as these coatings are literally a few molecules thick.
May be, but one thing I know is that when you come to metal plating you usually want to avoid sharp corners because the coating doesn't hold on a sharp corner... sure true for anodizing, not sure about other coatings.... ??? could be something to do with this...
But please do compare a coated and uncoated edge for sharpness. I think there is a noticeable difference.
That said, I agree that sharpness and surface smoothness is key to successful soft aluminum cutting, as I commented previously. The primary reason I like the coated cutters is not for higher speed or production longevity, since I can't cut at what would be considered 'high speed' by today's standards and I do prototypes and not production as a rule.
So what is the primary reason you like coated cutters for aluminum?
The caveat with uncoated cutters on aluminum is that you *might* get away with a dry cut . . . . and you might not. The trouble is the way you find out that you didn't . . . which can get expensive in a hurry.
That's true ;)
something that I find very effective for band saw blades is 'grinder's paste'. This stuff is pretty miraculous at keeping aluminum from sticking to saw blades and grinding belts . . . . . just don't use it for final finishing if you plan to paint the part afterward.
My almuminum supplier always use this pasty thing on their band saws... so you say it's a grinder's paste...
Daniel
-
I don't want to get into a science discussion on a hobby forum, but if you are curious about the coatings, you need to look into how cutting works on a microscopic level. The reason a lot of inserts are not sharp is because they don't need to be. The material actually 'tears' off and the very tip does not even contact the material.
The problems occur just aft of the tip where the metal chip is scraping past the tool surface after it is torn from the parent material. If you run inserts as fast as they are designed to run, the wear point is a crater behind the tip. This erosion failure of the cutter surface and is why coatings to improve abrasion resistance are effective.
Look at the part of your end mills where the chip is curled around after the actual cut. The sliding motion here creates intense heat which is the devil in aluminum and other gummy low melting point materials. In this case, abrasion is not so much the problem as heat and 'pick-up' and a coating that reduces friction or imparts a 'lubricity' in these surfaces of the cutting tool are effective in sort of a similar way to flood cooling.
That's as far into it as I want to get, but it is a fascinating subject with lots of technical information available for those with an interest.
As to grinding paste, there are no doubt lots of different ones. I was doing some consulting recently that netted me a sample of Boeing's 'Bio-Lube' product in paste form. It works well enough that I bought their gel version (have not tried it yet). Normally I use Eastwood's stuff. They call theirs 'grease' for some reason, but both these are more accurately described as 'sticks', methinks.
http://www.eastwood.com/ew-grinders-grease-8-oz.html
-
We always used Bio-Lube when a nonpolluting coolant was required while working with composite materials such as fiberglass or graphite. It works very, very well indeed. That is a great product.
As far as band sawing aluminum, the best way to destroy a blade it to saw the material without the 'stick of wax'. I've seen machinists dab the stuff onto an endmill when a short run part was being cut in aluminum - the 'gooey' stuff.
-
I enjoy reading your posts, Simpson.
I don't want to get into a science discussion on a hobby forum, but if you are curious about the coatings, you need to look into how cutting works on a microscopic level.
That's as far into it as I want to get, but it is a fascinating subject with lots of technical information available for those with an interest.
Do you have some link to refer me to, where I could read about all this stuff in more detail?
BTW, I called my tool supplier and asked if they had some cutters with coating for aluminum. The guy there said he never heard of coated cutters for aluminum... he said that the best results in aluminum are achieved with uncoated cutters and flood cooling.
Daniel
-
"BTW, I called my tool supplier and asked if they had some cutters with coating for aluminum. The guy there said he never heard of coated cutters for aluminum... he said that the best results in aluminum are achieved with uncoated cutters and flood cooling." - You need to find a better tool supplier. Look at any manufacturers current catalog for endmills made specifically for cutting aluminum. The vast majority of them will be coated, most probably with ZrN.
Regards,
Ray L.
-
OK, ok...I'm not that old. But a fellow I once worked with was.
I'd used the stick type lubes before, bandsawing and hand tapping where fluids were not practical.
This old gent had a little tub of tallow that he kept handy. I was amazed that it didn't rot but it never did and it worked quite well.
I'm surprised the wiki doesnt mention using tallow as cutting oil as it was used widely in machining. BUt for solder flux ? ? Bet that made you hungry for lunch. :)
http://en.wikipedia.org/wiki/Tallow
OK, back to the future McFly.
I use Stick-Kut from MSC.
Russ
-
I had a funny conversation about coatings with a PhD metallurgist working for Kennametal one time. She was working on endmill coatings, and some guy in marketing wanted her to take a bunch of endmills around to shops and ask them which ones they liked better. So they did a big study about it. She figured they'd be real scientific and try each cutter on their materials and then tell them which one worked best. She was surprised to learn that almost all of them just wanted "gold" cutters because they "looked cool." LOL!
So now marketing tries to make them find coatings in cool colors, and if they don't start out a "cool color" they try to reformulate it to get the color even if it slightly reduces the performance.
You gotta love the power of positive marketing!
Cheers,
BW
-
As far as paste for band sawing aluminum , I always use parrifin wax , the same stuff they use for canning.
Works for me. :D
-
OK, ok...I'm not that old. But a fellow I once worked with was.
I'd used the stick type lubes before, bandsawing and hand tapping where fluids were not practical.
This old gent had a little tub of tallow that he kept handy. I was amazed that it didn't rot but it never did and it worked quite well.
I'm surprised the wiki doesnt mention using tallow as cutting oil as it was used widely in machining. BUt for solder flux ? ? Bet that made you hungry for lunch. :)
http://en.wikipedia.org/wiki/Tallow
OK, back to the future McFly.
I use Stick-Kut from MSC.
Russ
I guess I'm pretty old. I have poured liquid tallow mixed with paraffin wax into the stuffing box on boats as a seal on the prop shaft. Never thought about using it as a machining lube. Any animal fat would work but I believe mutton tallow was used because it is one of few fats that flies don't particularly like. Some of that mix did smell pretty good though...We sold blocks of it to DIY boat owners.
-
I race grasstrack motorcycles and they use the same engines as speedway bike. These have normally run on castor oil.
I use the old oil as cutting oil and it's really good, no idea why but much better than others I've tried.
Works on band saws, lathe, milling machine and drilling and tapping.
Steve
-
Caster oil? It was even used as a laxative. Pretty expensive cutting lube!
You can separate caster oil out of other mineral oils and fuels by burning off the lighter oils since caster oil will not burn - with a burning permit!
-
Any of you guys ever use kerosene for working Alum. ?
Brett
-
Actually yes Brett. But K1 is the most stinky of the heavier fuel oils. It is even hard to wash the smell off.... WD40 is bad enough for stink and smoke. Kero smoke is nasty and the flash point is too low for safe use on the mill. That's it for you....
We used to use the Aladin Blue Flame Heater to heat areas that we worked and they never smelled. Now the heaters stink of raw kerosene. Very bad for the lungs!
Sorry - off topic.... MACHINE ..... - on topic... :-[
-
Good question Brett. I do know that kero is used quiet extensively on aluminum punches and presses. I have also heard of it being used for wet sanding aluminum. Some have praised it for that, others hate it. My first initial thoughts on it are, that it cleans AND lubricates, making it a "jack of all trades, master of none" kinda thing. I'm also interested in hearing some educated experiences with kero.
-
Screw this
-
Screw this
???
Not sure what you mean?
RICH
-
No self respecting machine shop or anyone else for that matter would use kerosene as a coolant! The discussion of using it is ludicrous. I would venture to say that if a machine shop did use kerosene as their machining coolant, they would be noted for the horrific fire that their machine shop went up in. The flash point is too low, it stinks, it is a carcinogen to the skin and lungs, it's expensive and it's lubricity is similar but a bit better than gasoline. Oh yes gasoline, let's discuss using it as a coolant too - it evaporates fast therefore it must be good as a coolant. Concentrated levels in confined spaces of kerosene fumes are highly explosive. If it weren't for wick style heaters and lamps, it would no longer be available, and that is probability not too far off in the future.
Add a soluble soap or oil as appropriate to water for your coolant, keep your sanity and property - no fire and no smoke.
There you go Sam, a professional, and 'educated' opinion.
-
Hey Steve, I used to use racing castor too but mixed it with the fuel for 2 cycle use. Did you use it in the gear case ?
Bill, I lube all of my casters with grease.
Sam, are you referring to punching, pressing and sanding so fast that a coolant is required ?
I have used kero for hand sanding machined fillet welds in aluminum and it did a good job. Just don't go too fast !
Russ
-
Bclemens, now i know what you mean. Whats wrong is sometimes folks take liberty in what they read.
You will find mention of Kero for cutting back oil in the Machinist Handbook. I guess i have also heard
or read of it's use in many mixtures, not to say they are safe. These days, MSDS sheets are mandatory and review of any material is done. ( heck i brought some marking stuff onto a site once and was almost fired!)
Some of the old timers used some nasty stuff. You should see what's in some old books on firearms and the chemical concoctions that were used.
RICH
-
The castor oil is for the engine Russ, normal gearbox oil in the gearbox but some people do use castor oil in the gearbox.
Just to clarify, this is oils such as Castrol R, I use Morris MLR40 at £30.00/5ltrs but it only gets used for one meeting then drained out so it makes a good cutting oil, to thick for spraying though so I use a brush and an old hand cream bottle with the press down top.
Other than that I flood coolant with soluble oil on my Alu cutting and I follow my uncles advise and tend to run low surface speeds and high feeds(compaired to modern practice), my mill only has a top speed of 2600rpm anyway so for anything less than a10mm carbide cutter I'm way down on the surface speed.
Steve
-
First off....let me apologize to Himy for taking this off topic.
My goodness, you'd think I had just shot somebody's favorite dog! Clemens, I do believe you are far to easy to take offense in the slightest thing you don't agree with. That's a shame, as this is a public forum and all (productive) comments should be welcome. In no form, or fashion, was my reply aimed negatively toward you, or any other person. Maybe I should have reworded it, such as...."I'm also interested in hearing some educated experiences with kero, in addition to BClemmens professional experience." I suppose I can see where you might have taken that I insinuated that you were not a professional, however, I do think you are the only person that took it that way, and I'm definitely not going to worry about every single phrase I make, in fear of the chance I might be offending somebody. None of us are here to offend, only to help and expand our knowledge. Nobody here knows everything, and no single answer to any discussion should be the "be all-end all, case closed".
There you go Sam, a professional, and 'educated' opinion.
Do I take offense to your reply? Of course I do. You definitely went out of your way to post that last part, to make it known to me that it is meant to be offensive. I won't loose any sleep over it though, I've got thick skin.
Yeah using straight kero as a flood coolant on a milling machine would definitely not be a good idea, and I don't really see how anyone could interpret from the responses here, that it would be, but that don't mean there is no place at all for the chemical in metal working. As I clearly stated, it is indeed used extensively in punches and dies. Actually, a nearby steel foundry uses kero with their aluminum dies. These dies stroke so fast they are a blur. This foundry uses kero, has never burned down, and they deal with molten metal daily.
Sam, are you referring to punching, pressing and sanding so fast that a coolant is required ?
As far as the punching and pressing goes, I don't know the "why" part of the kero usage. My first guess was that it acts like a light cutting oil, and a good solvent, both of which aids against the formation of gum, which would be disastrous (and expensive) in a very short time. It seems as though there would be a more suitable chemical. I was hoping to maybe get some people that have indeed used it in industry to further the discussion. Doubtful anybody will chime in now, though.
As far as sanding goes, it keeps the paper clean (unclogged), and aids in cutting. When wet sanding aluminum, you can really go through sandpaper quick. You can use detergent added into water, but it don't work nearly as good as a solvent.
-
LOL Bill, I introduced the forbidden word Kerosene in a topic on coolant because another fellow like yourself swore by it. I thought he was crazy too. His way was the only way and ready to fight if anyone had a different idea. I would love to get you 2 together. ;D
That's it for you....
What is that supposed to mean?
Brett
-
First off....let me apologize to Himy for taking this off topic.
My goodness, you'd think I had just shot somebody's favorite dog! Clemens, I do believe you are far to easy to take offense in the slightest thing you don't agree with. That's a shame, as this is a public forum and all (productive) comments should be welcome. In no form, or fashion, was my reply aimed negatively toward you, or any other person. Maybe I should have reworded it, such as...."I'm also interested in hearing some educated experiences with kero, in addition to BClemmens professional experience." I suppose I can see where you might have taken that I insinuated that you were not a professional, however, I do think you are the only person that took it that way, and I'm definitely not going to worry about every single phrase I make, in fear of the chance I might be offending somebody. None of us are here to offend, only to help and expand our knowledge. Nobody here knows everything, and no single answer to any discussion should be the "be all-end all, case closed".
There you go Sam, a professional, and 'educated' opinion.
Do I take offense to your reply? Of course I do. You definitely went out of your way to post that last part, to make it known to me that it is meant to be offensive. I won't loose any sleep over it though, I've got thick skin.
Yeah using straight kero as a flood coolant on a milling machine would definitely not be a good idea, and I don't really see how anyone could interpret from the responses here, that it would be, but that don't mean there is no place at all for the chemical in metal working. As I clearly stated, it is indeed used extensively in punches and dies. Actually, a nearby steel foundry uses kero with their aluminum dies. These dies stroke so fast they are a blur. This foundry uses kero, has never burned down, and they deal with molten metal daily.
Sam, are you referring to punching, pressing and sanding so fast that a coolant is required ?
As far as the punching and pressing goes, I don't know the "why" part of the kero usage. My first guess was that it acts like a light cutting oil, and a good solvent, both of which aids against the formation of gum, which would be disastrous (and expensive) in a very short time. It seems as though there would be a more suitable chemical. I was hoping to maybe get some people that have indeed used it in industry to further the discussion. Doubtful anybody will chime in now, though.
As far as sanding goes, it keeps the paper clean (unclogged), and aids in cutting. When wet sanding aluminum, you can really go through sandpaper quick. You can use detergent added into water, but it don't work nearly as good as a solvent.
Thick skinned and long winded! You are the one to be offensive and I answered you - without the offense. But you read it your way.....whatever....
Kind-of clannish bunch aren't you.....and I'm very aware that I'm not in the click here.
-
Kind-of clannish bunch aren't you.....and I'm very aware that I'm not in the click here.
For the most part folks are additive or question for understanding and will help until the end is found.
Remarks relative to posted info are just replies, but, content that insinuates ill meaning to a group or individual are not appreciated.
The only "clicks" i have found in my time here, are a bunch of folks who "click together" to assist another user or address a problem. Sometimes that ain't easy and requires a clan to accomplish it. ;)
RICH
-
As my Father used to say when we were causing trouble and Mom wanted him to intervene, "fight nice"
I read a lot of these posts and and I am amazed at the tensions and animosity that result.
I am actually reading this post to learn about Rays problem as I believe him to be a pretty sharp guy when it comes to Mach3 and its use. I didn't come here to read these posts to listen to people get all upset about what may or may not have been someones meaning.
AS far as clicks are concerned the only one I belong to is the DSPMC users which is by far in the minority. I forgot the other "Click" is the Mach3 users click in which if you are a user of Mach3 or even know about Mach3 your are welcomed in.
Back to the topic at hand. I can't imagine the use of kero on a daily basis. The smell makes me sick and I would be very concerned about the fire hazard. I do remember reading somewhere that it works well for drilling cast iron but I could be mistaken.
I also can recommend against the extensive use of WD40 in a mist lubricator. I had read that it works well for aluminum and it did a good job of keeping the cutter from clogging up but I had breathing troubles for a few days after a long machining session.
I have gone to water mixed coolant and I am very very happy with the result. Mu only real concern is the evaporation and carry off of the coolant. To minimize the carry off I have taken to washing the parts in clean water and then using this water to mix new coolant with. Since this water already has a percentage of coolant in it from washing the finished parts, I reduce the carry off some what.
So far I have not had any smell from the sump and the machine will sit for days and sometimes weeks without odor build up. I have even converted my bandsaw too use this as I like the all in one type solutions.
While I am sure that it is not the perfect coolant for every job, it has so far stood me in good stead.
>:D Mike >:D
-
I hope this doesn't start a fight, but it's "clique". ;)
-
Thanks Gerry for the spelling lesson.
Mike
-
All I intended to do was discourage the use of kerosene as a coolant in some raw newcomers shop and burn his shop/house down. Even suggesting its use might be enough to send someone up to the local service station to buy himself some 'coolant'. The MSDS on the stuff is enough to discourage the average person, but some just may not get the total implications and danger of using it. To request more information on its use as a coolant other than has been presented in as plain and to-the-point way is a possible come-on to some who may misunderstand. That' all I was trying to do. If SAM wants to get up in my face for the way I did it then that's SAM's problem. I'm not fighting anyone, wasn't my intent and never was. Pointing a finger in a kindly way with words only has always been tough for me but requesting more information on the use of kerosene as a coolant sent me on a campaign to discourage it completely. You took me wrong SAM!!!
'Clique', even looks better than 'click'. Looks special...
-
??? ;D Please excuse me for getting off thread, maybe this will provide some insight. ;D
RICH
-
What do you mean "getting off thread"? Ray L. probably has given up by now!
Spele chyck? Hey, 'click' was spelled correctly!
-
Never use spell check... I like to think I can spell better. :)
-
Quote
That's it for you....
What is that supposed to mean?
Brett
Joking Brett! As if you spilled your beer..
-
All I intended to do was discourage the use of kerosene as a coolant in some raw newcomers shop and burn his shop/house down.
And right you are.
-
The only problem with spell check and dictionaries is...... you have to be able to spell to know it's the right spelling of the word!
Having said that I use it all the time :)
Steve
Sign maker who can't spell.
-
Ohh and I stick by my old castor oils as a hand applied coolant, complete with methanol and other nasties.
Most soluble oils these days have something in them to stop the growth of the bug that caused coolant to smell, much nicer smelling now than when I were a lad.
Steve
-
Nah, I got the funny feeling that 10,000 plus members are following this thread and more Kero responses are yet to come. Hmm.....Ray will probably program something into Mach such that you will be prompted
for coolant type and if you select Kero mach will shutdown.
Now back on thread.
Some of the water based coolant will stain Al if left to dry and can be a cause for rejection of the work.
The grind shops refused to grind the plates ( 6' square x 3" thick plates ). The plates had to be re-machined / surfaced.
RICH
-
Awww come on, do we have to...???!!!
-
Ray L.
Sorry to end your discussion, didn't intend to. Just got a reminder of a heart felt and desperate incident with the stuff...
Besides, regarding you and kerosene; RICH has it; we're in no danger!
thanks,
-
;D
RICH
-
Quote
That's it for you....
What is that supposed to mean?
Brett
Joking Brett! As if you spilled your beer..
Shoooooooooooooooo............ thought there for a minute I was being put in time out or something. ;D
Spilling beer is almost as crazy as using Kero for coolant but I have heard of it. ;D I don't recommend either though.
Sorry to end your discussion, didn't intend to. Just got a reminder of a heart felt and desperate incident with the stuff...
I understand that Bill. Kinda like running up the road with arms waving to warn other drivers the bridge just around the corner is out. That is a noble thing. :) If that doesn't work the next step is to pull out your gun and shoot their tires out I suppose.
The point is............... sometimes some hot air has to be expelled to avoid a bad situation. I think were all big enough to appreciate the fact that although this hasn't been the warmest topic it will defiantly be the lesser of two evils if it in any way helps to keep a single person from a crash and burn. The Bridge is fixed now. It was a tough one to cross but were on the other side now. Lets get on down the road.
Brett
-
Just check this post ,LOL , and as far as kerosene goes , now days we have better stuff .
But years ago , well , many years ago , we did use kerosene for machining alum on the big planner , and theres no speed involved on a planner . It was driven with a flat belt. We just brushed it on , But never used it on a mill. And , it worked great.
As far as milling alum , FLOOD.
Ed
-
Just who are you 'laughing out loud' at there Ed? My band wagon? (I still feel bad about the way Ray L's thread got stomped on...(but he's probably Tubal Cain incognito))
-
Sorry to jump in here so late. It's been very interesting though.
When you refer to 6061 T651(1) "Wrought Plate" I assume you are talking about something other than your common 6061 everyday aluminum plate? Maybe someone can explain. I would have assumed 6061 T6511 would all be the same given the numbers pretty much dictate it's characteristics - no (?)
Thanks
Sage
-
6061 T651
Machinability and tensile the same. Wrought plate is double the price
-
And more than double the trouble by the sound of it because I've never had any trouble whatsoever machining the "regular" stuff. So the question is, why is the wrought stuff so difficult.
Sage
-
Sorry to jump in here so late. It's been very interesting though.
When you refer to 6061 T651(1) "Wrought Plate" I assume you are talking about something other than your common 6061 everyday aluminum plate? Maybe someone can explain. I would have assumed 6061 T6511 would all be the same given the numbers pretty much dictate it's characteristics - no (?)
Thanks
Sage
T651 and T6511 are not the same thing. T561 is rolled, stretched, then surfaced, rather than being simply extruded. I can't explain why the real-world machining characteristics of this stuff is so different from the extruded 6061 I've used tons of in the past, but it sure is. However, increasing the chipload/feedrate by about 2X has resolved my problem. It now machines just fine, at 30 IPM with a 1/2" HSS 2-flute, and 75 IPM with a 1/2" carbide 3-flute, even with no coolant.
Regards,
Ray L.
-
SO all the digits are important to note. I'll have to investigate that more.
Thanks for that. I hope I never need to machine it.
SAge
-
According to the Aluminum Associations standards and data:
T_51 Applies to plate and rolled or cold-finished rod or bar, die or ring forgings and rolled rings when stretched the indicated amounts after solution heat treatment or after cooling from an elevated temperature shaping process. The products receive no further straightening after stretching.
Plate 1 1/2 % to 3 % permanent set
Rolled or Cold-Finished Rod or Bar 1 % to 3 % permanent set
Die or Ring Forgings and Rolled Rings 1 % to 5 % permanent set
T_511 Applies to extruded rod, bar, profiles (shapes) and tube and to drawn tube when stretched the indicated amounts after solution heat treatment or after cooling from an elevated temperature shaping process. These products may receive minor straightening after stretching to comply with standard tolerances.
Extruded Rod, Bar, Profiles (Shapes) and Tube 1 % to 3 % permanent set
Drawn Tube 1/2 % to 3 % permanent set
-
Hmmm. They look almost the same except for the rolling vs extruding. Amazing that rolling the aluminum can can make that much difference in the machining characteristics of the finished product.
Sage
-
Hmmm. They look almost the same except for the rolling vs extruding. Amazing that rolling the aluminum can can make that much difference in the machining characteristics of the finished product.
Sage
Well, when machined *properly* there doesn't seem to be a huge difference. I can now use the same (revised) parameters for both with good results. What I was using before worked well for T6511, but not for T651. It appears to me the T651 just gets gummy at a significantly lower temperature. The difference is just a much heavier chipload.
Regards,
Ray L.
-
It now machines just fine, at 30 IPM with a 1/2" HSS 2-flute, and 75 IPM with a 1/2" carbide 3-flute, even with no coolant.
Regards,
Ray L.
Can you tell us the RPM's you are running?
Maybe what kind of cut depths you are running?
It will probably help some of us a lot if we run into a similar
situation.
Thank You,
Scott
-
It now machines just fine, at 30 IPM with a 1/2" HSS 2-flute, and 75 IPM with a 1/2" carbide 3-flute, even with no coolant.
Regards,
Ray L.
Can you tell us the RPM's you are running?
Maybe what kind of cut depths you are running?
It will probably help some of us a lot if we run into a similar
situation.
Thank You,
Scott
For a 1/2" HSS 2-flute, 3100 RPM, 0.150" DOC, 30 IPM works well. For a 1/2" Carbide 3-flute, 6100 RPM, 0.150" DOC, 75 IPM works well.
For a 1/2" HSS 2-flute, 3100 RPM, 0.500" DOC, 12 IPM.
I'm still playing with settings to find the optimum for deeper cuts. I tried the HSS at 0.225" DOC, 18 IPM, but that didn't work terribly well - chipload was too high.
Regards,
Ray L.