PDA

View Full Version : Aluminium cutting



Bush Flyer
21-04-2014, 05:51 PM
I wonder if someone could check my setting for cutting aluminium as I keep breaking end mills. The last time I had this settings. The aluminium is 6082 T651 18mm thick I am just using this to test. I'm trying to pocket out a 25mm diameter hole only 6mm deep and I'm only getting to half way round the second pass.
The bit is a 1/8th single flute carbide bit, the depth of pass is 1mm RPM is 15000, chip load I have as 0.003 which I workout as 1142mm per minute feed rate plunge rate I have as 126mm per minute, the coolant I am using it duck oil its like WD40 but does not evaporate like WD40 and is a better lubricator.

Recap. Aluminium is 6082
Bit is 1/8th carbide single flute.
feed speed is 1142 mm/per/minute
plunge rate is 126 mm/per/minute
spindle speed is 15000 rpm
depth per cut is 1 mm
step over is 30% 0.952 mm
chip load is 0.003

There must be something in there where I have picked up wrong for working out feed and speed.
This is how I worked out my feed rate.
Feed Rate = RPM x number of flutes x Chip load.

Which gave me 45 I/P/M then to change to metric I divide that by 39.374 which gave me 1.142 metre which is 1142 mm. or multiply 45" by 25.4 which is 1143mm

Or is this all wrong.

Clive S
21-04-2014, 06:37 PM
Well take this with a pinch of salt but Gwizard tells me that at 15000rpm 1.4 doc 279 mm/min plunge 276 mm/min and 24000 rpm 446 mm/min.
I am not an expert by any means on using the calculator so please wait for another opinion. ..Clive

EddyCurrent
21-04-2014, 07:09 PM
I've only been cutting wood but from that experience I would say your spindle speed could be lowered and the feed rate is way too high. As it is it's trying to cut 3/4" a second which does not seem right.

Bush Flyer
21-04-2014, 09:22 PM
I have tried a slower feed rate but it blunt the end mill to a point it was not cutting but I cant remember the setting since then I have started to keep a note of what I have been trying. If I took the spindle speed down to 10000 rpm then the feed rate would be 30inch a minute or 762mm per minute, at a chip load of 0.003 but if my feed rate is to fast at 15000 rpm at 1142mm per minute should it not be the case that at 10000 rpm at a feed rate of 762mm per minute still be wrong. is there something wrong with the calculation that I have found or is it the chip load that is wrong for a 1/8th single flute end mill. also how slow can you take a water cooled 0.8kw spindle before it would stall when cutting.

Washout
21-04-2014, 10:00 PM
Hi Bushflyer,
.
Are you roughing or trying to get a decent finish - there's quite a difference between the two I've found.
.
For roughing I am using mostly a 6mm single flute carbide end mill using 16,439rpm and somewhere between 550 and 650 mm/min - when this is right and the tool is sharp its almost noiseless when roughing through 6082 T651. The lower feed rate seems to be better when the tool is slotting (6mm width) and higher when running at my normal 45% step-over. Also that's all at 2mm DoC - I've tried deeper at 3mm which is OK'ish and much deeper at 5mm but the latter was shrieking.
.
I'm using GWizard, which now has a gantry router setting and this is on either the 2nd or 3rd setting (highest kills tools and lowest is resulting in "rubbing" i.e. there's a lot of crap not being cut and being "pushed" out of the way.
.
Finishing paths are a different ball game as the very low "step overs" mean you can get chip thinning i.e. heat which needs getting rid of and also means high feed rates (3000mm/min+) and if that runs into a slot condition goes bad very quickly.
.
Hope that helps and I'm always on the lookout for experience in this, as getting in the "window" of feeds and speeds means the difference between nice, acceptable and ruined parts - especially with gantry routers.
.
Oh also a misting/flood system is a must IMHO for aluminium, as is paranoid blowing out of chips with compressed air - I have had everything cooked right before and snapped a tool just from clogged chips in a slot before.
.
Hope that helps.
.
.
Chris
.
PS. See my Youtube channel for some examples of pocketing 6082 T651.

Jonathan
21-04-2014, 10:51 PM
Your chipload is too high. For single flute tools, these are roughly the settings I use for cutting aluminium:

1/8", 24000rpm, 500mm/min
4mm, 18000rpm, 600mm/min
6mm, 12500rpm, 600mm/min
8mm, 9600rpm, 600-700mm/min

...then tweak the rpm until it 'sounds right'. That should get you close enough. With limited coolant I'd be inclined to lower the rpm and feedrate proportionately - soo keep the same chipload but run slower.


Well take this with a pinch of salt but Gwizard tells me that at 15000rpm 1.4 doc 279 mm/min plunge 276 mm/min and 24000 rpm 446 mm/min.
I am not an expert by any means on using the calculator so please wait for another opinion. ..Clive

Last time I checked, all Gwizard does to calculate the plunge feedrate is set it to the linear feedrate divided by the number of flutes - so for a single flute cutter it's the same. It's much kinder on the spindle not to ramp instead of plunge, or at least plunge a bit more slowly.

Here's a video of my machine cutting with the same tool (@2:14):


https://www.youtube.com/watch?v=hXxCQOqG8D4

JAZZCNC
21-04-2014, 11:15 PM
Chip load is wrong it should be more like 0.05 not 0.003. As a rule of thumb for chip load for roughing(50% stepover) divide the cutter diameter by 80. For slot cutting divide by 120.
15000rpm would give feed rate around 800mm/min with DOC 50% cutter diameter.

There are so many variables to working out speeds & feeds and the ridgidty of machine plays large factor so it's very difficult for anyone to work out F&S for someone else.
Also when getting into smaller cutters the material plays big part because while in theory the Grade of aluminiun should mean uniform hardness it doesn't and it's not uncommon for the same grade of aluminium to cut differant from batch to batch and even from same sheet.!! Only experience can help with this and unfortunatly this does mean wrecking a few cutters to learn.!

One thing you don't mention is how your entering the material.? You mention plunge rate and this makes be think your plunging straight down into the material.?
This is bad for tools and Esp single flute cutters so it WILL be knocking the edge off the cutter resulting in more heat.! . . . HEAT is the enemy and you want to aim for chips that are very hot but cool/warm material and cutter. When you have it corrrect you'll get a better idea of what I mean becuase the chips really burn when they hit you.
So when entering material either pre drill a hole and plunge into this. OR use ramping or spiral entry stratergy. Never plunge aluminium with a single flute cutter as it just kills them.

Loads of air and coolant are a must when slot cutting with small cutters and even when stepping over 45-50% they still need good chip clearing to prevent heat build up from chip re-cutting.

Edit: Bugger didn't see Jonathan had beat me to it but never hurts to get it said twice. .Lol . . . .. . Oh and I think Jonathan ment to say it's much kinder on spindle to Ramp rather than "Not Ramp".!

Bush Flyer
21-04-2014, 11:17 PM
Hi Chris,
I have just been trying to get a rough pass, I have never tried a 6mm carbide end mill as I don't have many and I'm sure the ones I have are only for wood, but I will order some and try, could you please tell me how to find you on YouTube, as I would like see your channel, I must have watched hours of cutting aluminium on YouTube and you can hear some of there end mills screaming. then you find one that it looks like it was cutting butter with a hot knife and that's where I want to be but am having a hard job finding the right information.
I have watched a Dennis martens cutting 6040 aluminium but there is no information about how he is doing it feed and speed plunge rate etc.

Jonathan
21-04-2014, 11:23 PM
Chip load is wrong it should be more like 0.05 not 0.003

Handy to specify the units here. Bushflyer is specifying the chip-load in inches per minute, so he's using 0.0762mm vs your suggestion of 0.05mm.

JAZZCNC
21-04-2014, 11:43 PM
Handy to specify the units here. Bushflyer is specifying the chip-load in inches per minute, so he's using 0.0762mm vs your suggestion of 0.05mm.

Ye you'd think I'd done this shit before wouldn't ya.!. .:joker:

Bush Flyer
22-04-2014, 12:00 AM
Hi Jonathan, and jazzcnc.
Jonathan many thanks for the info I hope this will get me in the ball park, Jazzcnc that's a big difference in chip load, where can I find more information on line about chip loads and calculations, I know about GWizard But I would rather have one with no cost or a one off payment as I mainly will cut ply and balsa and some small parts in aluminium. Once I can get near the correct settings I would have no or very little use of Gwizard calculator and yes I have been plunging into the aluminium but a very slow rate.

JAZZCNC
22-04-2014, 12:49 AM
Try this for a one off fee. http://www.mycncuk.com/forums/computer-software/7432-just-heads-up-anybody-thinking-buying-hsmadvisor-fswizard-25%25-off.html#post57489

Other than that then can't help as I tend to use rule of thumb and my ear or occasionally I'll use G-wizzard.
Google can be your friend sometimes.

To be honest your best approach is to setoff of slow and find your machines sweet spot and only way to do this is thru trial and error. Like I said doesn't mean my settings or anyone else's will work well for you or your machine so your best finding the limits of your own machine. Unfortunatly the price can be a few snapped cutters.

Best tip would be set your best guess for feedrate and spindle speeds then use feedrate over-ride to lower and setoff slow to judge how it's cutting. Between changing feedrate and spindle speeds it doesn't take long to find the machines sweet spot. Then start tweaking the DOC when you feel more confident and have a feel for the machine's/cutters limits.

Bush Flyer
22-04-2014, 11:29 AM
I have just tried the HSMadvisor free calculator and like it, easy to use. The G-wizard calculator is too expensive for all that I would use it. Anyway where are you buying your single flute carbide bits from? I have been buying from aliexpress.com and am beginning to think I should buy some better quality bits. the bits I have been using were listed as suitable for cutting acrylic, organic board material, Metal, Copper, Aluminium, but I have my doubts now.

Washout
22-04-2014, 11:37 AM
At the risk of a bit of shameless self-promotion here's my channel link on Youtube - https://www.youtube.com/user/CCWashout/videos
.
The 5th Video is probably the best one with the two 5mm deep pockets being cut - the noisiest thing in the room was the compressor, but I have made some horrendous noises previously when F&S have been wrong, misting not running properly etc. Oh the description for that vid is slightly wrong as the previous vid was an 8mm Carbide Single Flute and the 5th vid uses a 6mm End Mill @16439rpm, 2mm DoC, 539mm/min.
.
I'll back Jazz up and recommend ramping for single flute cutters - I've broken the tips off of a number of them by plunging and I tend to find if you have to plunge try and set that in your CAM software at ~30% of your normal feed rate.
.
One of the things I found frustrating is the CAM software I am using, as Vectric's Cut3D and 2D does not always consistently apply ramping and in the case of Cut3D doesn't give you a ramping option at all. I am mostly using Deskproto now which does apply ramping, but only if there's enough room on the first move, but at least I can force it to plunge if there isn't at 30% feed.
.
I'm still learning myself and will post more vids as I progress and if you want to see something really cool look at Jazz's video of his machine using iMachining trochoidal toolpaths - that stuff is amazing (one day I'll be able to afford that :-) ).

Washout
22-04-2014, 11:41 AM
For single flute cutters I'm using APT www.shop-apt.co.uk (http://www.shop-apt.co.uk) - they are more expensive than some of the ebay sellers, but I'm finding the quality and longevity much better - I wouldn't recommend it but I managed to cut my finger by clumsily taking the plastic cap off of an APT cutter and brushing the edge, whereas a batch of ebay cutters were no where near as sharp - I'm not sure that the correct way to test cutter sharpness however ;-)

Bush Flyer
22-04-2014, 01:29 PM
Hi Washout,
I liked your videos, Thumbs Up. The 5th video is perfect, That's how I want to be cutting aluminium. I don't think I will use your method for testing how sharp the end mill is, It's a bit messy. Can you tell me the plunge rate you have on the 5th video, and I take it as your using the full rate as you ramp down? and you only use the 30% if you were plunging a hole with an end mill instead of a drill bit.

corkcnc
24-04-2014, 10:36 PM
Just wondering why you didn't climb mill the 5mm pockets in the vid. Don't take this as a criticism as I bow down to your ability to self build such a nice looking machine. You would find yourself with a longer tool life though if you did all of the 5mm in one pass and cut the pocket using 30% step over. You could increase the feedrate then due to the chip thining so you would have a nice increase in material removal rate. I understand that you are not looking to lash off 1000 pieces so time probably isn't a bit deal but it would be better to let the whole tool wear a fraction than the bottom 2mm wear while the top section does no work.
Regarding speeds and feeds calculators I have a nice .xls file which I got from my tooling supplier. When I read the figures that came out first, I said no way, surely the tool can't handle it but they do. It gives you a range of speeds for carbide and hss tools, which is useful, as if you want to apply it to different brands of tools you can put in the lowest settings and still be in the ball park for things like stainless. Then you can speed up if the conditions allow. If anyone wants a copy just pm me and I'll send it on. One important point though is that I have a rigid NC bridgeport and home made machines wouldn't be expected to have the same rigidity so carbide tooling may not be suitable at high feed rates if vibration is an issue.
Regarding tool paths I'n keen to see how m_c gets on with generating trocoidal paths with cambam. If the software can do that for under 100 it sounds like a great deal. I use trocoidal all the time and cringe when I have to put a tool into a corner when the rads limit my options.
Rgds,
Noel.


At the risk of a bit of shameless self-promotion here's my channel link on Youtube - https://www.youtube.com/user/CCWashout/videos
.
The 5th Video is probably the best one with the two 5mm deep pockets being cut - the noisiest thing in the room was the compressor, but I have made some horrendous noises previously when F&S have been wrong, misting not running properly etc. Oh the description for that vid is slightly wrong as the previous vid was an 8mm Carbide Single Flute and the 5th vid uses a 6mm End Mill @16439rpm, 2mm DoC, 539mm/min.

JAZZCNC
25-04-2014, 12:17 AM
Regarding tool paths I'n keen to see how m_c gets on with generating trocoidal paths with cambam. If the software can do that for under 100 it sounds like a great deal. I use trocoidal all the time and cringe when I have to put a tool into a corner when the rads limit my options.
Rgds,
Noel.

Yes when you've used Trocoidal toolpaths you really don't want to go back to normal milling. Like Washout says I use i-machining (mostly for roughing) and it's unreal the material it shifts and time it saves even with my low powered spindle and DIY built machine. To watch it dance and chomp 6061 T6 @ 20mm depth between 2500 & 3000mm/min and do it with ease is amazing.

Washout
25-04-2014, 12:42 AM
Just wondering why you didn't climb mill the 5mm pockets in the vid. Don't take this as a criticism as I bow down to your ability to self build such a nice looking machine. You would find yourself with a longer tool life though if you did all of the 5mm in one pass and cut the pocket using 30% step over. You could increase the feedrate then due to the chip thining so you would have a nice increase in material removal rate. I understand that you are not looking to lash off 1000 pieces so time probably isn't a bit deal but it would be better to let the whole tool wear a fraction than the bottom 2mm wear while the top section does no work.
Regarding speeds and feeds calculators I have a nice .xls file which I got from my tooling supplier. When I read the figures that came out first, I said no way, surely the tool can't handle it but they do. It gives you a range of speeds for carbide and hss tools, which is useful, as if you want to apply it to different brands of tools you can put in the lowest settings and still be in the ball park for things like stainless. Then you can speed up if the conditions allow. If anyone wants a copy just pm me and I'll send it on. One important point though is that I have a rigid NC bridgeport and home made machines wouldn't be expected to have the same rigidity so carbide tooling may not be suitable at high feed rates if vibration is an issue.
Regarding tool paths I'n keen to see how m_c gets on with generating trocoidal paths with cambam. If the software can do that for under 100 it sounds like a great deal. I use trocoidal all the time and cringe when I have to put a tool into a corner when the rads limit my options.
Rgds,
Noel.

Hi Noel,

At that point I needed the parts off of the machine without mishap, as they had to go on the race car as one of the first bits of assembly, as they sit between the monocoque and the front sub-frame (replacing bonded ali and silly putty....I mean rubber OEM parts ;-) ). I also had limited amounts of 40mm 6082, so I needed safety and the machine was not long up and running at that stage. Conventional was quieter and I figured less stressful than climb, but I do use both these days and I hear you on the wear at the tip, but I have managed to tune my F&S's, using GWizard's help, to the point where (touching wood) I'm getting much better tool usage than I used to.

Washout
25-04-2014, 12:46 AM
Hi Washout,
I liked your videos, Thumbs Up. The 5th video is perfect, That's how I want to be cutting aluminium. I don't think I will use your method for testing how sharp the end mill is, It's a bit messy. Can you tell me the plunge rate you have on the 5th video, and I take it as your using the full rate as you ramp down? and you only use the 30% if you were plunging a hole with an end mill instead of a drill bit.

Correct chap - using full plunge when ramping and only 30% when actually plunging straight down, which I try not to do unless the CAM software forces me to do it.

GEOFFREY
25-04-2014, 10:20 AM
Probably slightly off topic, but related to material removal. About 3 years ago I visited a factory that had a number of CNC mills, one of which was making some ally boxes for race car electronic enclosures and they were specified as machined from solid billet. The way that the material was removed for "pocketing" was that the machine was programmed to plunge drill a series of holes about 50mm deep with something like a 20/25mm drill, each hole slightly overlapping the next such that it left a series of islands standing and serrations round the edge. The finish milling then simply meant removing the islands and cleaning up the edges. Of course this was a commercial machine, through tool cooling etc., but the factory owner told me that it was by far the quickest and cheapest way to remove material. I realize that this method is probably well known, but I thought it was interesting. G.

Bush Flyer
25-04-2014, 08:32 PM
I have just ordered a heap of aluminium and Five 1/8 single flute bits for cutting aluminium. When They arrive I will start at one setting and keep a note of exactly what the feed and speed is and go from there. The plan is I will take a slice right through the aluminium from one side to the other ie. mill a slot 1/8th wide.
The aluminium is 6082 T651 the end mill is 1/8th (3.175mm) carbide it is 38mm long 20mm will over hang the collet the cutting edge is 12mm long, the feed it will be 325mm per minute, plunge is 254mm per minute, the spindle rpm 12000, and the depth of cut will be 1mm.
Any advice about changing some of the settings will be welcome.

cropwell
01-05-2014, 02:19 AM
Worth a look
Sorotec - Werkzeuge (http://www.sorotec.de/shop/index.php/cat/c60_2-Flute-ALU-2-Flute-ALU.html) click the flag to translate it to English,
.
but with shipping costs you have to buy about 50 quids worth to make it worthwhile.

Bush Flyer
03-05-2014, 09:07 PM
Well that didn't work out well, cutting 6082 aluminium. The settings were. 12000rpm. Feed rate of 325mm per minute. Plunge rate of 254mm per minute, with a depth of cut 1mm. I used a 3.175mm single flute carbide bit, but as soon as the bit cut in to the side of the aluminium the bit broke, so I tried a cut depth 0.5 mm. The bit did cut through the aluminium of 60mm wide but by the time it was at the end there was a poor shaving curl and when I got down to 5.5mm deep it broke that end mill as well. I did use cutting oil and it was a wash with it, also there was no smoke coming from the bit so it was not getting hot. So what do I do now should I reduce the depth of cut a little more or speed up feed rate. Or is it that I am using to small a size end mill?

routercnc
03-05-2014, 11:17 PM
Hi Bush flyer,

I recently cut some elongated slots with a 3mm carbide bit without any problems. I don't use the 3mm cutter much (tend to use 6mm) so haven't experimented but the following settings worked OK:

DOC 0.3mm
rpm 12,000
300mm/min feedrate
30mm/min plunge rate

The 4 slots were 5mm wide, 15mm long, and 10mm deep (other side is pocketed 10mm). See photos below.
12324 12325

(I was actually surfacing the whole part in this photo - hence the 6mm cutter in the collet, not 3mm, but you can see the slots I was refering to)

I flooded the holes with duck oil as soon as cutting started. There was no smoke, no screeching, just a soup of very small chippings swirling around in the pocket as the cutter did it's job.

Bush Flyer
03-05-2014, 11:28 PM
Hi Routercnc,
Thanks for the quick reply, That's just what I wanted, your setting for slotting aluminium I will try again tomorrow with that settings. Would it be possible that you could also tell me the settings you are using with your 6mm single flute end mill as well I have 25mm thick aluminium to cut so am thinking I will get a few 6mm end mills.

EddyCurrent
03-05-2014, 11:38 PM
Hi Bush flyer,

I recently cut some elongated slots with a 3mm carbide bit without any problems.

What's the cutter details ? e.g. single flute, up spiral

Edit: This might seem a daft question but to me the thread is going round in a circle until Bush Flyer uses a cutter of the same type and most importantly, brand, that others are using when they suggest cutting parameters. The difference between a good cutter and a bad one is chalk and cheese.

magicniner
04-05-2014, 12:36 PM
I bought some cheap 3mm single flute cutters from Ebay, whilst the cutters themselves are good the initial edge applied to them is a little random, fortunately the single flute cutters are very easy to hand sharpen and and a quick touch-up on a diamond wheel is all they needed to get them cutting cleanly. They're not listed as suitable for Aluminium but I've used one on Brass, Bronze, Aluminium and Titanium and I'm still on the first one of a pack of 10 ;-)

- Nick

Bush Flyer
06-05-2014, 07:32 PM
We have success, :friendly_wink::friendly_wink: Using the settings from routercnc I was able to cut aluminium without breaking the end mill or blunting the end mill. Now just to fine tune, I used a zig zag plunge from zero Z axis height and it was too slow I think at the low plunge depth I will try it without the zig zag or increase the plunge rate and keep the zig zag, Now all I have got to do is the same for a 6mm end mill. Thanks again routercnc.

routercnc
06-05-2014, 09:46 PM
Glad it helped.

3mm bit was carbide 2 flute slot drill from 'bargain tooling' on e-bay:
3MM CARBIDE SLOT DRILL / CUTTER 2 FLUTE *NEW* | eBay (http://www.ebay.co.uk/itm/141159822132#ht_1464wt_1190)

I don't usually cut much aluminium, so am not an expert, but I have been cutting a fair bit recently for the upgrade parts. The setup I'm using is as below. This is what works on my machine, but no guarantee for yours:

e-bay again from bargain tooling. Can't find link to original part I bought but similar to this:
6MM CARBIDE SLOT DRILL / CUTTER 2 FLUTE *NEW* | eBay (http://www.ebay.co.uk/itm/130790907141?ssPageName=STRK:MEWNX:IT&_trksid=p3984.m1439.l2649#ht_1472wt_1190)
dia: 6mm
material: carbide
flutes: 2

feedrate: 800mm/min
(it feels like it could take 900-1000mm/min which is a better load, but running on 26V machine concerned about stalling/missing steps. Still waiting for new drivers . . .:grumpy: )

plunge rate: 150mm/min

DOC: 1mm
(tried 1.5mm today and tends to squeal / resonate - upgrade parts should improve things)

WOC: 6mm

spindle speed: 12000rpm

Bush Flyer
06-05-2014, 10:28 PM
That's great, just sent an order to ebay for some 6mm end mills. Thanks for recommending the seller routercnc, I appreciate your help and I will test it with the setting you have recommended.

AGTM
24-09-2014, 11:58 AM
Hi Bush Flyer

I am new here, but I went through the posts. Would you please tell me why you are using a single flute cutter for aluminium?
I have been working aluminium for years, but mostly with 3 flute cutters. You can plunge, slot and side milling with no problems.
Depends of the tool I am running the cutters around 8000 - 10000rpm.
For me is interesting why single flute, why not 2 or 3 flutes?

AGTM
24-09-2014, 12:22 PM
Hi All

I am reading here the discussion about the aluminium cutters. I also checked the links to eBay.
Yes, this price is good, but I would recommend something better. Check this out: http://www.agtmcarbide.co.nz/product/aue-0603/. These cutters are great, just as good as Iscar, but a lot more valuable. These tools can do DOC: 2.5D and WOC: 1D.
Not bad. Here is something more: http://www.agtmcarbide.co.nz/speed-tiger-cutting-tests/

JAZZCNC
24-09-2014, 01:28 PM
For me is interesting why single flute, why not 2 or 3 flutes?

Because of machine stiffness and feedrates at DIY level. With 3 flute you need much higher feed rates at lower DOC and most DIY machines can't cut at those feeds and are not strong enough or have powerful enough spindle to cut at correct DOC for 3 flute cutters.

I agree thou they are better than single flute and give nicer finish if you can use them.

AGTM
25-09-2014, 10:34 AM
Hi JazzCNC,

Thanks for the fast reply. Now I understand the situation. OK, here is what I would do if I have to use a single flute cutter for aluminium:
My rule specially for aluminium is Fz=D/100 or for example if you have 6mm diameter cutter your feed rate will be Fz=0.06mm/rev. And if you have available 10000 rpm, your feed rate will be F=600mm/min. I would not go more than DOC=1D
and WOC=1D.
Always helical plunging if it is possible as F=1/2 for the plunging. The single flute should go straight plunge (drilling) with no problems. Finally, It really depends of the carbide grade of the cutter. It might not be suitable for high speeds. Recently, I did a custom order for 3 flute uncoated cutters for aluminium. I made 12mm cutter with 45deg spiral. The tool has 24mm working length and 80mm total length. The carbide material of this cutter is WC25, a grade for stainless steel processing. This cutter works since four weeks, it is still in use and it works with S=10000rpm and F=3800mm/min.
So, if the single flute cutter brakes on the recommended cutting conditions, I am sure we can fix this problem with custom made tool. The good part is that the price is the same as the standard one, but there is a requirement for min 5 cutters.
I have one of those 12mm cutters left. If you want I will send you to try it or to some friend of you.

JAZZCNC
25-09-2014, 02:38 PM
Hi AGTM,

Problem most DIY users here wanting to cut Aluminium is spindle power or lack of it.! Most are using router based machines and spindles with high speeds but little torque with typical 2.2Kw.
So DOC=1xd on 6mm cutter with WOC=1xd is mostly impossible with the spindle torque they have available.! Then you have the stiffness of the machine. Again being router based most are flimsy in comparison to even the weakest milling machine so chatter and poor finish dictate using much lower feeds/DOC etc.

I may give your cutters a try but I mostly use smaller 4-8mm cutters. Again due to spindle power but also material saving when nesting parts.
I'm a big believer that when it comes to tooling cheaper cutters are uneconomical as they wear quickly and put more stress on the machine not to mention much poorer finish quality.

Also I feel most people use the wrong tool for the Job, like not using a ripper for roughing.? Often this is down to the fact they don't want to change tools so will use one tool to do the whole job. This again is False economy because with a cerated edge ripper you can cut far deeper and remove far more material in fraction of the time without wearing the tool away or stressing the machine/spindle.
Also they don't actually save time by not changing tools it actually costs them time and money because the smaller tool cutting at lower DOC takes much longer than any tool change. Plus the tool and machine are getting hammered because they are working much harder than they need to.
On top of this Finish quality is lowered because by the time they get to the end of the job the tool cutting edge is so worn finish is poor. They don't realise that by using rippers and then just doing a finish pass they actually save money because time is reduced and tools last much longer as they are cutting efficiently and they get a much better end result.!

That's my take on it. . .:beer:

AGTM
26-09-2014, 09:49 AM
Hi JAZZCNC,

I agree completely with you about the written above. You mentioned that you use 4-8mm cutters. I want to send you one Speed Tiger AUE to give it a try. Let me know what diameter would you prefer. You can go on the contact us page in my web site and give me your address.
Next week I will start a new thread named "Solid Carbide Cutting Tools - what we know and what we do not know about them"
There will be a few posts as I will start write first about the carbide grade of the tool.

Otherwise it is Friday here, a time for barbeque and beer.
:yahoo:
I'll see you next week here.
Have a great weekend. Cheers.

JAZZCNC
26-09-2014, 01:48 PM
Otherwise it is Friday here, a time for barbeque and beer.
:yahoo:

That's just cruel as it's pee-ing it down here.!!! . . . . But that's ok as it's offset with plenty of the finest Ale in the world. .:beer:

Boyan Silyavski
26-09-2014, 09:35 PM
I find that Fz=D/100 usually too much. Especially about aluminum. Not talking about roughing bits. Tools 0-2mm is one thing, 3mm is another thing, 4-6 mm another, and so on.

I have Gwizard trial installed but some how this program doesn't engage me, may be the price and subscription put me off.
Just found the free online FSWizard (http://zero-divide.net/index.php?page=fswizard) and actually the data it gives is quite near the manufacturer data and very very near at my actual cutting data. So i am quite convinced and maybe even will buy the payed version

The bits i use are mainly Kyocera, razor sharp and polished. Now looking at their data below, some conclusions about how things develop with sizing and type of operation can be drawn. This is quite more realistic than others i have seen.

http://www.mycncuk.com/attachment.php?attachmentid=13465&stc=1http://www.mycncuk.com/attachment.php?attachmentid=13466&stc=1http://www.mycncuk.com/attachment.php?attachmentid=13467&stc=1



Vc - cutting speed
f - chip load or feed per tooth
Fr- feed rate mm/min
D- diameter of carbide bit
U- nimber of teeth on cutter
p=3.14


Ae - side removal
Ap - face removal


1.
determine spindle speed rpm/min depending an operation/roughing, slotting, finishing/


RPM=(Vc*1000)/(p*D)


2.


Calculate feed rate mm/min:


Fr=f*U*RPM

AGTM
27-09-2014, 11:09 PM
Hi silyavski,

I checked carefully your post and the data which you provided. I completely agree with these parameters, but only if you do finishing. What I mean is that the roughing parameters provided in your table will be applied for finishing by me. I am working with Fz=D/100 and the tools (different range of diameters) sounds and works excellent. This is the tool: http://www.agtmcarbide.co.nz/product-category/agtm-tool-categories/aluminum-alloy-copper-alloy/endmill/aue-series/
In addition, this tool is designed for hard work and high MRR (material removal rate), but this cutter can be used for roughing and finishing as well. ST AUE has been designed for roughing, but it is doing a better finish than Kennametal.
I am attaching the manufacturer's cutting data for your reference. You will see there, that what I have recommended in my previous posts is actually low and safe. And it is because it is proven already by me.
I have sent a samples to JAZZCNC already, I will send you too to give it a try.
If you want to "make a step ahead", send me your address and let me know what diameter suits you.
Here are the cutting conditions:
http://www.mycncuk.com/attachment.php?attachmentid=13479&stc=1http://www.mycncuk.com/attachment.php?attachmentid=13480&stc=1

AGTM
27-09-2014, 11:16 PM
Hi JAZZCNC,

Your samples are on a way already. You should have them in a 4-9 days.

Cheers

Boyan Silyavski
28-09-2014, 12:32 AM
HI AGTM,

The data is for general 30 degree bits, not for 45 degree specific aluminum bits , that's why we are both right

AGTM
28-09-2014, 01:17 AM
Hi silyavski,

Yes, completely agree. If the bits are 30 deg I wouldn't do rough milling with them as you mentioned. They are mostly for finishing. AUE can do both.
Meanwhile, Kyocera have extremely good flat U-drills. They works pretty good on stainless.

Cheers.

AGTM
28-09-2014, 02:26 AM
Hi silyavski,

Here I made a picture of AUE1203. Take a look and let me know what do you think.
I will just mention that this tool has polished front and back cutting surfaces. To be honest yes, I am selling these tools, but I can assure you from the user point of view that these cutters are better than many world famous brands, which I will not mention here.
http://www.mycncuk.com/attachment.php?attachmentid=13484&stc=1

Boyan Silyavski
28-09-2014, 09:53 AM
These you show are 3 flutes and seem nice. But I believe here people/DIY, forums/ would be more interested in your AET series 2 flutes, cause they can be used also for plastic and wood, or at the long ones (http://carbide-tool.com.tw/pdf/400/400-025.pdf).



Now other thing is the price and place of origin.

Its difficult to convince people to buy something not made in USA or EU. At least me. Especially at similar prices. Thats the truth. I see many sellers /China, Taiwan, etc. / raise their prices and make them comparable to the famous brands. But reality is that a typical small business will search for discounted known brand,overstock sale, a deal or a clearance and will not buy 3rd brands.

Hell, i would not buy, even try other brand carbide router bit while Drillman sells Kyocera bits at ebay (http://stores.ebay.es/carbideplus/), especially at his price. I don't see how sb. could beat him especially for the DIY people market -plastic, wood and aluminum. 1-6mm. Kyocera also have representatives in Eu. Do you know why no body has ever heard of them? I will tell you. Cause they sell for 20euro the 6mm stub 2 flute that Drillman sells for 6$

AGTM
28-09-2014, 10:50 AM
Hi silyavski,

Thanks for the reply mate. This what you wrote above is completely fine and understandable. I will not continue arguing with you in any way as in the world there are many different people with different ideas and vision. That is completely fine.
Yes, there may be more interest about some other types of cutters and I might give a 6$ price for them too, who knows? These ones (AUE) are 9.86USD currently if you buy more than one. Whoever is interested is warmly welcome to contact me and to ask me. I will be happy to help him with any information. Let me tell you something very important, which appears you do not know clearly.
There is a big difference between China and Taiwan, I have been in Taiwan already on a visit in the ST factory. Their tools as I said are better than some of the world famous brands and there is no need to look for clearance, overstock sale and whatever.
I gave you a free offer, you did not accept, that is fine.
Whoever wants to try ST AUE is welcome to contact me. I have available AUE samples up to 10mm diameter.
The most important, which I want to finish with is that unfortunately you do not want to even try to make a step ahead.
You have my best wishes and success in your business.

Boyan Silyavski
28-09-2014, 11:16 AM
I was relatively speaking about the trying, i apologize, don't mean to spit on your business efforts :-) .

And the link to ebay was not to promote the other guy, but to point it to you , so you could look at what he sells, for how much and how his sales are going.

So compiling what is needed for the typical owner of CNC at home, you could offer it at one place, a good price, and have your cheaper sales, which once when you reach quantity will be very satisfying. Meanwhile you could sell locally at normal prices or just offer forum members different prices. As you know, this is not the only forum, however this is the highest quality forum i know of.

From what i have seen you have quite good price for the extra long reach aluminum ones, for example.

AGTM
28-09-2014, 12:01 PM
Hi silyavski,

I already have clients here in NZ. But I also have clients in Australia, EU and USA. The world is small at these days.
If hope you spotted already that there is a free delivery for orders over 200NZD. Well, if you know what you are buying and you are available to plan your job, there is no problem to select whatever you need even from NZ. I am not a local retailer, that's why I have good prices. I will start a new topic soon here. The thread will be "Solid Carbide Cutting Tools - what we know and what we don't know about them". Have a read if you have time as there I will try to explain in details the deference between value and price of the tool.

Cheers!

JAZZCNC
28-09-2014, 12:08 PM
The proof is in the eating.!! and I will soon be feasting on AGTM chips so we will see. Thank you.

But Boyan I have to disagree with you because I've tried many of the cheap cutters off Ebay and they are rubbish.!! . . . Cutters are not cheap when they go dull 2hrs into 6hr job or snap at 5hr58mins and wreck the job.!!
Drillman sells cheap endmils but are you 100% sure they are Kyocera or there rejects.? Maybe maybe not and it's this unknown that can't be trusted and when I'm cutting 300 piece of aluminium with 6hrs machine time I can't take that risk.

Even at DIY level I feel it's foolish to buy cheap endmills unless your first learning so still wrecking with wrong F & S or crashing into things (which I never do of course.:whistle:) as again lots of time and effort invested not to mention material can be wrecked for the sake of 3-5 more. Then you have machine stress to factor into the equation.!! . . . . Just not worth it to me.!!

Boyan Silyavski
28-09-2014, 12:39 PM
But Boyan I have to disagree with you because I've tried many of the cheap cutters off Ebay and they are rubbish.!! . . . Cutters are not cheap when they go dull 2hrs into 6hr job or snap at 5hr58mins and wreck the job.!!
Drillman sells cheap endmils but are you 100% sure they are Kyocera or there rejects.? Maybe maybe not and it's this unknown that can't be trusted and when I'm cutting 300 piece of aluminium with 6hrs machine time I can't take that risk.


Who could be 100% sure.

But:
Come in original sealed boxes. Look perfect, measure perfect. Outlast many times, like 20x times in wood - Bosch, Freud and similar , which are triple the price. Definitely ultra sharp and fine polished. I have seen only Onsrud and 10 times more expensive ones with better polish.

With the machine i build for my friend i tested 3 straight flute one where the flutes are 25mm long and the bit is 1/4 in diameter, typical wood bit, so i routed aluminum with astonishing glass like result, 1mm deep pass with 0.8kw spindle at 25ipm. The precision was 0.01mm.

I have very flimsy machine as you know maybe, belt driven, v bearings, not for aluminum at all. I have done many 10 hour aluminum scratching jobs with 3mm bit without problem. So on that machine I use 1/4 3 flute straight bit at diameter depth for like 25 times x 2 hour jobs in very nasty hard pine that does not cut well , without loosing edge. And it chatters a bit all the time due to the flimsiness of the machine. So i guess on a good machine it would last forever.


Anyway, yeah, i have small box with 1000 euro worth of Kyocera bits at Drilman prices, so yes, they are that good. He sells Destiny bits for aluminum. I like to look at the Kyocera bits like more multi functional ones. plastic, wood , aluminum with one sharp cheap bit, thats the DIYer dream.

When i finish my build and finally have new machine, will know better.

Kentobi
25-03-2015, 10:07 AM
some good advices here, thanks for posting

Boyan Silyavski
17-04-2015, 10:16 PM
Dean, did you ever test the bits?

JMaack
23-04-2015, 06:50 PM
If anybody needs speeds & feeds for Aluminium cutting I will be more than happy to help. Just let me know!

Chaz
12-05-2016, 09:22 PM
Dean, did you ever test the bits?

Also keen to know .....

magicniner
13-05-2016, 10:40 AM
I have a few of these - http://www.ebay.co.uk/itm/371406148992 - they are cheap and not advertised as anything special. I bought them initially for plastics, but then tried them on Aluminium and found they were great.
Last week I had some small parts to make in 304 Stainless from 12mm rolled stock and thought "What the heck!", loaded up a single flute (I did re-grind the tip to what I felt should be a slightly more robust form) and it proceeded to carve out my parts seamlessly.
I used air for cooling and chip clearance plus mist lubrication,

- Nick

Chaz
13-05-2016, 10:57 AM
I have a few of these - http://www.ebay.co.uk/itm/371406148992 - they are cheap and not advertised as anything special. I bought them initially for plastics, but then tried them on Aluminium and found they were great.
Last week I had some small parts to make in 304 Stainless from 12mm rolled stock and thought "What the heck!", loaded up a single flute (I did re-grind the tip to what I felt should be a slightly more robust form) and it proceeded to carve out my parts seamlessly.
I used air for cooling and chip clearance plus mist lubrication,

- Nick

Thanks. Im still hurting from breaking two fairly expensive roughing end mills. Mostly my own fault and not having enough spindle power. Having a some other options to mess around with will be good. Ill order a few of these and try them.

I am happy with the APT supplied end mills. I'm getting great finishes with the 10mm 3 flute endmill from them but they arent cheap. The roughing mills are expensive too (35ish for 10mm) but they work well (if you dont break them).