Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: mikel92 on August 09, 2018, 01:22:49 PM
-
I have just finished the initial setup of a CNC router at my place of work, and being a novice when it comes to configuring everything, I am wondering what the best tool would be for aluminum/composite metal applications? Current setup and use is as follows:
CNC Router: Accu-Cut XPS 6F12F (http://computerizedcutters.com/our-products/accu-cut-xp)
Application: Cutting signage from 1/4" alum. 6061 sheets, and 1/4" composite metal paneling (Omega-lite)
I believe the current tool was a 3/16" Dia x 2" L x 5/8" Flute Carbide Single Flute bit, but I ended up accidentally breaking it.
-
A 1/4" bit would be stronger. I'd use a single "O" flute bit.
Like an Amana 51401 or 51402.
-
Hi,
the trick to cutting aluminium is to clear the chips as they are cut. If the chips get recut
they are very VERY likely to get stuck to the bit, sometimes called 'built up edge' or BUP.
Its a certainty it will bugger up your job, and make real hard work for your spindle.
Using air or even flood coolant gets rid of most of the chips, if you can do it.
If you cant then slower surface speeds (200 m/min) are appropriate but if you can clear the chips
surface speeds of 500 m/min are OK.
So with a 3/16 tool:
diameter (mm) = 3/16 X 25.4
=4.76mm
circumference=4.76 x PI
=14.95mm
surface speed =rpm x circumference (in m)
=21000 x 0.01495
=314 m/min
which is in the zone for aluminum.
Even a 1/4 tool will have a surface speed of 418 m/min, which would be fine IF you can clear the chips.
Craig
-
Hi,
just a thought, my previous post assumes carbide tools. You'd want to reduce surface speeds a lot for HSS.
Craig
-
Hi,
a couple of other ideas to think about.
You may have seen a lot of carbide tools with coatings like Titanium Nitride, Titanium Carbo Nitride and so on.
They are very good when cutting steels but not with aluminium.
The coatings are very hard and aid lubricity so chips slide off and over the surface. Most of the coatings are variations of nitirides
which are trivalent. Aluminium is trivalent and the lubricity a coating might add for steel is actually 'sticky' for aluminium.
Consequently carbide tools sold for aluminium are often not coated at all. There are coatings that do work and work well including
C(hemical) V(apour)D(eposit) diamond (being essentially quad-valent) but are expensive and rare. Don't go there until you are 100% experienced and can get days
or even weeks without breaking a tool before you consider these exotics. There is one coating that is not common but not that expensive,
Titanium Diboride, and its just the bees knees for aluminium.
I use small, I mean very small endmills for making circuit boards, 0.4mm and 0.5mm (16-20 thou) and you only have to look cross-eyed at
them and they break. You are likely to have quite a few accidents before you get good at it. Cheap tools are OK when starting out but once you get
good enough to not break too many you should be using branded tools, they are more expensive, lots more expensive in cases but often are that much superior.
Harvey Tools have a vast range and all good. I tried some Raptor endmills from Destiny Tools and while expensive, in stainless and tough steels like 4340, just the best
I've ever used. I haven't tried their Viper DVH tools but are meant to be good for aluminium, 45 degree variable helix, with and without coatings.
I know a lot of sources say don't bother with coolant with carbide tools, I find though I get a huge performance lift when using flood coolant, I suspect more because
of flushing the chips out of the cut zone. When flood cooling works it will improve tool life by a factor of ten or better!
Craig
-
^ very interesting about the coating valency and its relevance to materials cutting. I'll bear that in mind.
I've had some pretty good carbide tools from AliExpress, the Chinese suppliers seem good at making these. Their HSS tools are a bit 3rd world but their carbide ones are well worth it and certainly a lot less intimidating cost-wise for a new guy.
-
Thanks for the information! It is saving me many hours of times/headaches since I am attempting to to set up our table from scratch with no manual or anything. I really appreciate it.
I have one more question regarding bit type, downcut vs upcut, which would be better suited for my application? I'm assuming downcut leaves a better finished edge (a lot of the sign work would require this), and upcut is better at removing and clear material, is this correct?
-
You should get similar edge finish with either one. I'd use an upcut with aluminum, because the chips have nowhere to go with a downcut.
-
Hi,
downcut is useful if the materials really soft and you want to prevent the tool from lifting the cut edge. If the cut is not right
through the chips have nowhere to go and can't be used. As a consequence the vast majority of tools are regular upcut.
I've had some pretty good carbide tools from AliExpress, the Chinese suppliers seem good at making these
I used to think so.....until I started using Harvey Tools, Destiny Tools, Kyocera Tycom, Kennametal and Iscar.
Craig
-
I just ran a cut, and did a mix of inside cuts and outside cuts. the tool went clockwise, but counterclockwise on the out side. Is going counterclockwise worse for the bit?
-
Hi,
the tool rotates in one direction, the vast majority are Right Hand.
As to the direction around the perimeter that you traverse the cut is the difference between 'conventional
milling' and 'climb milling'. With older mills which have backlash you must use conventional milling only whereas
CNC mills with no backlash can use either. For various reasons climb milling is preferred IF your mill has the rigidity
and ZERO backlash.
Most CAM programs allow you to chose either conventional or climb milling toolpaths.
There is plenty on the net about climb/conventional milling.
Craig
-
Could you explain what backlash is? I've found some information on the internet, but I'm not sure I understand it completely.
How would I know if my machine has a backlash system?
-
Hi,
on a conventional lathe or a mill with ordinary hand wheels if you wind the wheel clockwise the axis
will move to the right, say. If you now wind the wheel counter-clockwise there will be a small zone
where the axis does not move until the 'backlash' is taken up and then starts to move to the left.
If you like backlash is the slack in the thread of the leadscrew. Just about all conventional machines
have it, more as they wear.
Modern CNC machines with preloaded ballscrews can be called zero-backlash, although an engineer might question
your definition, and as such have no measurable slack between the axis moving right or left. Such machines
often use 'climb milling' toolpaths.
Craig
-
Ok, I think I have that figured out on my machine.
After a few cuts I noticed that I am getting a pretty thick bur on the edges of my cuts (1/16"), I used a baseline feedrate/rpm calc sheet to start, but being that the material I am using is somewhat unique I'm not sure what to be using.
Currently, I have my IPM = 45 and RPM = 21,000 - The material I am cutting is a mix of an aluminum backer (0.013" THK), corrugated polypropylene plastic 0.2" THK), and an aluminum face (0.031" THK). I am using convention milling as well.
I did a mixed calc with Gwizard, and it gave me 23,000 RPM @ 34 IPM for both the backer and face aluminum, and 24,000 @ 121 IPM for the plastic core. Is it switching feedrates and rpms logical for this situation?
-
Hi,
unless you can be sure that the only cutting that will be done in any pass is the plastic core then keep the speed the same.
If for instance you up the speed but part way through the pass the tool engages with some of the aluminum. either top or
bottom, the tool will break.
If I understand the way you have proposed your question you are doing multiple passes to cut through the composite.
That will mean that only the very tip of the tool will be doing the cutting. When the tip of the tool is blunt it will have
to be replaced but the rest of it is perfect.
May I suggest trying to cut through the entire thing in one pass. The two layers of aluminum constitute a thickness of only 1/16 and
the plastic core is that soft it doesn't really matter. You'll have to cut more slowly, probably very slowly to start until you get a feel for what
can be achieved but even at only 15ipm would still be the same total time as three passes at 45ipm. At least this way you would see that more of the
tool is engaged and cutting.
Craig
-
Hi,
I came across this when I was making my mill.
I went to the scrap yard and got some big cast iron weights that had been used in a lift. It was a cheap source of big cast iron lumps.
What I did not know was that the cast iron was pretty rubbishy, I mean all they have to be is heavy, they don't have to be that good.
When I started milling them in the Bridgeport at work I found that the iron had quite a few inclusions which were very hard on the HSS tools
I was using. In my inexperience I tried to take light and shallow cuts to make the tools last. That was a mistake, it means that the tip of the
tool does all the work and the flanks of the tool do nothing. Re-spharpening is possible but as I was paying a company to do it it was dubious that
I was saving any money.
I found instead the best way to proceed was to take deep cuts, 1/2 to 3/4 inch deep but only 20-50 thousandths laterally. The old mill has HEAPS
of backlash, nearly 0.2 inch, the yoke must just about be worn right through, and so after my one mistake, I had to use conventional milling
sometimes called down milling. At least when the tool was worn out I'd got the best out of it.
If you are unsure about climb/conventional milling get yourself to the controls of an old Bridgeport with plenty of backlash. Put in a 1/2 endmill and some
steel in the vice and try climb milling. Make sure you are wearing a face shield!. When the mill 'climbs' into the cutzone and shatters the tool and/or dislodges
the steel in the vice you will understand the difference and what that can mean. You can read 100 books or look at 10 videos but 5 minutes at the controls
of a mill will teach in a manner that you'll never forget!
Craig
-
Worth noting that if you're cutting grotty metal like odd castings and steel with mill scale on it, conventional milling saves the edges of the bit to an extent. if the cut starts in the meaty bit of the metal it doesn't impact on the scale or the casting's crusty shell. Climb milling has the teeth of the bit cutting through the nasty bits every time and it fouls it up quite fast.
@joe Chinese steel has this sometimes including structural sections, big pockets of carbon or slag, horrible stuff.
-
at 21000rpm @ 13 IPM, with 0.17" per pass and its cutting like a charm, thanks for the advice.
What's a good indication that a bit is dull or bad?
-
Hi,
first indication is cut quality, followed by built-up-edge, followed by breakage.
The last two occur within seconds.
Craig
-
Hi,
the real killer for aluminum cutting tools is heat.....and I don't mean necessarily heat of the tool or workpiece. Its more about
the heat of the chips.
There are some excellent videos on you-tube about chip formation, every mechanical engineer has to be intimately familiar with this process
AND the calculations that result. I'm only very fair with the calculations myself.
Amongst the objectives of forming a chip is to have the energy of the shearing work to enter the chip rather than the workpiece or the tool. You'd
say that the chip is 'hot'. You will of course have seen 'blue' hot steel chips forming when drilling steel. The same thing happens with aluminum but
without the change in color. Also the melting point of aluminum is only about 780 C whereas steel is about 1480 C.
If by a combination of heat and pressure aluminum chips adhere to the edge of the tool the energy (heat) required for the now blunt tool, by virtue
of the rounded built up edge, to create fresh chips increases dramatically. This results in now very very hot aluminum chips and will have a great propensity
to stick to the already built up edge. Breakage is now imminent.
It is a similar line of reasoning that recutting chips must be avoided. When an aluminum chip is formed it gets hot, lets say 400C. Should that same chip
get recut by the next flute it will get hotter again....lets say 700 C. At that elevated temperature the likelihood of it sticking to the tool goes up hugely.
Thus if you use means like flood cooling or air to remove the chip from the cutzone, it will still get hot, 400 C, air or coolant doesn't change the physics
of chip formation, but air/flood will prevent the chip from getting recut. If you haven't given some thought to trying flood cooling, think again, and if you
decide you can't do it, think a third time until you do it.
Flood coolant or air will have significance for tool life. Lets say that a new and sharp tool will produce chips of 300 C at normal cutting parameters. As the tool
wears and becomes less sharp the temperature of the chips will go up, lets say to 500 C, at which point they adhere to the tool and that tool is now worn out.
If you have flood cooling or compressed air in operation you may be able to cool the chips to the extent that they do not adhere and can carry on using the tool,
extending its life.
I use very small (0.5mm) and tender two flute carbide endmills to cut a thick (0.42mm) copper layer on a circuit board. Without flood cooling I get about 1/2 hour
life for a tool with decreasing cut quality, burrs etc. WITH flood cooling I get about 10 hours, and MUCH BETTER cut quality.
I have had similar experience in aluminum. At 500m/min surface speed my 3mm two flute endmills will last a few minutes before BUE (built up edge) and
subsequent breakage. WITH flood cooling the same endmills last for hours and NO BUE!!
I know a lot of highly authoritative sources say don't use coolant on aluminum but I have found an immense increase in performance if I do.
Craig
-
I have been wondering if its worthwhile for me to try and figure out the coolant system on our setup, as I have no idea how to configure the airline relays. Is conventional milling something I would be OK using a 3/16" O-flute on 1/4" 6061 alum sheets?
Also, this is a separate concern, but I cannot tell if the spindle is sinning at the RPMs shown on screen or if it's full bore at all times. I have it set tp a 18+ dc unregulated pin, and it doesn't seem to sound different at different RPM - FROM 1000RPM - 21000 RPM the motor seems to be spinning the same. Should I be setting this up with step and dir outputs?
-
Hi,
Is conventional milling something I would be OK using a 3/16" O-flute on 1/4" 6061 alum sheets?
If your machine is sufficiently rigid and without backlash the climb milling is preferred. There is extensive discussion on the net as to why
that is the case.
Should I be setting this up with step and dir outputs?
Does the spindle have a step/direction drive? From what you have described I don't think so. what make and model is the spindle motor?
What sort of spindle controller do you have? Can you post some pics?
Craig
-
The Spindle is a Perske - not sure about the model because the tag is covered by a block.
BoB is a Sound Logic PC-2--> (https://www.scribd.com/document/217900646/Pc-2-Route-for-Mach-Rev-1-9)
-
Hi,
Perske is a very good brand, so is Yaskawa and they are both very expensive.
The VFD is for an asynchronous motor and step/direction is not possible, that requires a servo type motor.
The VFD and spindle are very good indeed, I suspect that if yo set to 20000 rpm it will do it whether you
believe it of not.
You could put an index sensor on the spindle and have Mach count it out to confirm what speed its doing.
I am inclined to think that your PWM to DC converter is not linear.
For the work you are doing and the size tools (bits are for woodworkers) you are using just set it to run at maximum
and leave it be.
Quite frankly I think trying to buggerize with that spindle is wasting your time, you could very much more profitably
work on a flood coolant or air cooling solution.
Craig
-
Thanks for the info - I am starting to cut 6061 1/4" alum. sheets now, what would you recommend as a starting point for IPM, RPM, and depth per pass. I configured my coolant mister so this should help.
Current tool (https://www.amanatool.com/51408-solid-carbide-cnc-spiral-o-flute-aluminum-cutting-3-16-dia-x-1-2-x-1-4-inch-shank-up-cut.html?ff=1&fp=11947)
The provided feed and speeds from the mfg. seem really high to me, I did a test run with the recommended rates and the tool deflected quite a bit.
-
Hi,
why use single flute?
Download a demo copy of HSMAdvisor.
The surface speed for 6061 with uncoated carbide is in the region of 200-500 m/min. What you can actually achieve will depend to a large extent
on the rigidity of your machine and whether you can avoid recutting the chips. If you recut chips ALL BETS ARE OFF.
Craig
-
Someone on here suggested an O flute for aluminum. I tried cutting at 18,000 RPM 90 IPM @ .005 Depth per pass, and it gave a pretty good cut, the downside being 54 passes per piece.
What does it mean when I am creating dust instead of chips? Is this good or bad?
-
Your depth per pass is way too low. Having said that, the actual depth you use depends on the rigidity of the machine.
You should be cutting at least .05 - .125 per pass.
-
Hi,
I'd be trying to cut the panel in one pass, ie top layer aluminum, the core and the bottom layer aluminum all in one go.
Craig
-
He said 1/4" aluminum? There's no core or layers?
-
Hi Gerry,
OP is also cutting cored aluminum panel.
Craig
-
I've switched over to 1/4" Aluminum, I think I said that in a previous post, sorry if that wasn't clear.
-
Hi,
well that does make a difference.
The temptation is to take a lot of very shallow cuts but it is a mistake. That would mean that the only
part of the tool that sees any work is the very tip, once it gets blunt you throw it out despite the rest of the
flanks of the tool being good.
Take fairly deep cuts, maybe 1/8 inch or more. Then use your speeds and feeds calculator to work out how fast
to cut. You are hoping that you will load the tool up so that the spindle is producing some real power.....thats
when the tool is at its most cost effective. Sure you can make it last longer by pussy footing around with it
but when you bore in, approaching its strength limit, you will do a lot more cutting before it wears out.
Under those circumstances cooling, or more importantly, chip evacuation and lubrication become important.
I personally have had great success with flood cooling despite the extra complication and mess. rcaffin, a regular
on this forum uses M(inimum) Q(uantity) L(ubrication), a mixture of kerosene and olive oil with compressed air.
He uses vanishingly small quantities with great results and has all but convinced me to try it too.
We were discussing it on CNCZone but feel sure he'd be willing to post some pictures of his setup, its remarkably
simple.
Craig