PDA

View Full Version : Single flute carbide cutters



Jonathan
26-07-2011, 12:49 AM
I was wondering if anyone has used these single flute carbide cutters:

http://www.ebay.co.uk/itm/5x-6mm-Carbide-CNC-Router-Bits-Single-Flute-Tools-22mm-/130520720413?pt=UK_Home_Garden_PowerTools_SM&hash=item1e63a4241d#ht_2706wt_905

They're a lot cheaper than anything I can find in England ... but will they be any good quality?

I've chosen single flute for the obvious reason - more space to clear the swarf.

I'm intending to use them with 18mm plywood and probably aluminium. I've been using the 6mm router bits from Toolstation recently but not having much luck. It's quite a lot to spend if they turn out to be no good ... can get 19 of the 6mm carbide tipped cutters from tool-station for that price so it's only worth it if they last at least 4 times as long.

AdCNC
26-07-2011, 01:30 AM
Ive also been looking at these, i have used some similar before and have had good results. for what its worth i think i might give these ago. if you are wanting to cut ply then i would suggest you use a straight fluted cutter, there are a few on the market.. but having used a fair few i have found that the geometry on the cheaper ones like the ryobi and silverline to be really poor and this is shown with the cutting, they seem to resonate more so than cut, now swap to a trend, freud or titman and you will have alot better results.. thats if your cutting woods anyway.

Jonathan
26-07-2011, 12:14 PM
I heard that straight flutes are better for ply as it's less likely to lift. Or even better apparently are compression cutters since they squash the material together on both sides... expensive though.

The finish I was getting with the silverline 6mm, 6mm per pass, was fine ... Problem was it snapped (twice). I'm hoping it's just a matter of getting the feedrate etc correct for them to last... the good brands you mention do cost a lot more.

Shall I buy them and we can share? (annoying that's it's an odd number)

AdCNC
26-07-2011, 01:10 PM
Shall I buy them and we can share? (annoying that's it's an odd number)


Sure if you want to.. how do you want to do it tho. you have 3 and ill have 2?

John S
26-07-2011, 01:18 PM
The finish I was getting with the silverline 6mm, 6mm per pass, was fine ...

If it snapped twice, back off a bit on cut, 100% of depth per diameter is a bit much on 6mm.

Jonathan
26-07-2011, 01:38 PM
Sure if you want to.. how do you want to do it tho. you have 3 and ill have 2?

Sounds good to me. I was going to say I'll have 3 but didn't want to sound greedy :lol: I can buy them today - no doubt they will take forever to arrive. They shouldn't cost much to post. There's also 25mm long for 4 more ... not sure which to get as the 22mm will be stronger, but 25mm might be useful...


If it snapped twice, back off a bit on cut, 100% of depth per diameter is a bit much on 6mm.

Ok then, I've just checked the Gcode and it was actually 5mm per pass, not 6mm as I thought. I'll try less next time.
I was using 2500mm/min and 18,000rpm ... that makes the chip load very low which I suspect was what caused it to break. It broke when I lowered the feedrate to 2000mm/min. I think I'll try something like lower rpm but keep the same feed next time to reduce the heat.

AdCNC
26-07-2011, 01:45 PM
Another thing that i you need to pay attention to is the resonance, these cutters can give off a "screaming sound" this is bad as what you are hearing is the cutter resonating. this will almost definitely cause the cutter to fail. Id experiment like you say keep you feed the same 2.5M/M and reduce or increase you RPM until the screaming goes, you should hear a nice cutting sound, I if get 5 mins ill do a vid for you.

Jonathan
26-07-2011, 06:03 PM
I think I would describe the sound as 'screaming' ... not the normal sort of 'hissing' sound. I'll experiment tomorrow and do a vid...I bought a heap of cutters from toolstation yesterday, 3 each of 6mm, 1/4", 8mm and 10mm so plenty to experiment with though I'd prefer not to break them all! Before I made the recent changes to the router I can't remember ever breaking a cutter ... it was just too slow. I can use much more than 2.5m/min if neccecary - I tried a 1/2" cutter yesterday cutting 1/2" deep and it was fine at 6m/min.

Robin Hewitt
27-07-2011, 11:08 AM
I bought a couple of these cutters in 2 and 3mm from J & L to try with aluminium. Haven't spun one up yet, but I reckoned that half fishtail point should be good for a fine horizontal finish. Wonder how it copes with a vertical plunge, I always prefer to add some horizontal movement when I sink a fishtail, but that might just be my poor old brain seeing problems that do not exist :whistling:

blackburn mark
27-07-2011, 10:23 PM
iv bought 30 of the 3.175mm version... iv only managed to wear one out in alli, they seem to last for ever in acetal though (snapped one or two)

im lazy with my g-code and plunge straight in... if they costed more and i was wearing lots of them out id consider ramping

Jonathan
30-07-2011, 02:00 AM
I'm thinking that they may not be as effective as a 2-flute cutter at plunging since with only one flute cutting (instead of one and a bit) the direction of the resultant force in the X/Y plane is going round in circles. Whereas with 2-flute I imagine the the forces are almost equal, and they are opposite ... so they should at least partially cancel out. That does not take into account swarf ejection though...

We used carbide 2-flute cutters (2mm and up) on the little router at school all the time with various plastics. They lasted a long time.

Karl
30-07-2011, 11:25 PM
So do these single flute carbide cutters on ebay have a centre cut for plunging?

blackburn mark
31-07-2011, 03:36 PM
So do these single flute carbide cutters on ebay have a centre cut for plunging?

the cut passes the centre and because of the rake and clearence etc if you plunge a blind hole you end up with a small dome at its base

make sure you measure the radius of your cutter when you buy them !!!!
mine sold as 3.175mm however the cutter was much closer to 3mm and the shaft was 3.175mm..... took me ages to work out why some of my parts were under/over sized:whistling:

packmansdaddy
08-08-2011, 03:26 PM
I have tried several of these single flute cutters and results vary relative to the quality. You can buy them in solid carbide from US$ 4 to US$ 60, in HSS from US$1 to US$ 10. This price is for a 6mm cutter.
As blackburn mark mentions, measure the exact diameter. Especially the cheaper ones vary slightly (some up to 0.1mm).
I can plunge even the cheap ones in aluminium at twice the speed than 2 flute milling cutters without any vibration. I have cut solid hardwood, MDF and acrylic with great results and performance in aluminium is even better. And it does not die if it takes a chunk out of your vice either. I use them on my router and my mill.

If you thought your router would be not solid enough to cut aluminium, give these a try. You could be up for a nice surprise.
On my home made router I cut 16mm MDF in one cut at 400mm/min @ 12000rpm.

Jonathan
12-08-2011, 11:46 PM
The cutters arrived ... and they're excellent! Not measured the diameter yet as my sister has borrowed my micrometer (long story).

I've only used one so far, and on aluminium. Cut some lots of parts from 4mm aluminium sheet with 0.5mm depth of cut and no coolant at 550mm/min ... no problems and left a good finish. I used a spiral path, so no plunging.

Also used one to cut two spindle mounts from 5/8" aluminium, again pretty good finish this time with 0.7mm depth of cut and cutting fluid. The swarf is ejected much better as expected.

blackburn mark
13-08-2011, 10:57 AM
0.5mm depth of cut

that doesnt sound like you jonathan !!

in acetal (like butter to cut) ill go up to 3mm depth with the 3.175mm cutter at 200mm feed and adjust spindle speed untill the chips are nice chunky curl and do a 0.5mm finish at full depth (upto 20mm)
i use a fish tank type air pump to blow the chips away... its a tiny amount of air but with the nature of acetal chips it doesnt take much to clear them even in a slot

they are quite good in abs as well, with the reports i had heard i was exspecting meling problems but i didnt get any of that, im guessing my spindle speed was aprox 2000rpm

iv snapped a couple of small single flute cutters in plastic when braking out of slots that arent perpendicular to the exit face, when the cutter exits the material it can pull itself out of the exit and try to walk around the corner .... pi**es me right off when its a fresh cutter, im guessing a lower feed or higher spindle speed would stop this but it seems to happen at what i would cosider the sweet spot (i might be overly aggressive:whistling:)

luke11cnc
14-08-2011, 01:13 PM
I think I'm going to buy some as I have no cutters for aluminium any guidance on sizes would be greatly received or should i buy a kit?? and add to it as and when I need it

James

Jonathan
14-08-2011, 01:46 PM
Bigger diameter cutters are *much* more rigid, so you want to use the biggest you can for a particular part. Within reason though as clearly a bigger diameter cutter will remove a greater volume of material, so the cutting force is higher for a given depth of cut. It's a balance ... I thought 6mm was good in general, but if you're only cutting say 5mm sheet then 4mm would probably be fine. I wouldn't advise anything bigger than 6mm for a router.

I've got some 0.5mm, 3mm and 4mm on the way, though they are two flute (oops).

luke11cnc
14-08-2011, 01:56 PM
what about plunge cuts of flat bottom hole ??

James

Robin Hewitt
14-08-2011, 02:52 PM
I've got some 0.5mm on the way

Blimey, you're brave :eek:

OTOH maybe you are cutting cheese or these are in stub length :naughty:

Jonathan
14-08-2011, 02:56 PM
Blimey, you're brave :eek:

OTOH maybe you are cutting cheese or these are in stub length :naughty:

PCBs ... so more like cheese on toast.
I've used 0.8mm on the router with aluminium - it didn't break!


what about plunge cuts of flat bottom hole ??

Using a spiral toolpath works well for that.

packmansdaddy
21-08-2011, 02:07 AM
what about plunge cuts of flat bottom hole ??

James

as has been mentioned before, you will end up with a small dome in the center. These cutters plunge much easier than two flute cutters.

My 6mm single flute is actually 5.95mm. With the right data the cutting is very accurate.

I used 1mm two flute cutters in the past on aluminium and acrylic with very little success. But the single flute 1mm cutter did a fine job and is still in one piece after about 3 hours work in aluminium.

Jonathan
22-08-2011, 05:53 PM
I accidently chipped one of the single flute cutters, but it turns out they are easy to regrind ... works just as well as new now. I was thinking I should buy some more in case these break... but it looks like they're immortal.

Just tried the same cutter on plywood, 14000rpm, 2800mm/min (so quite a high chipload) with 4mm depth of cut on spiral toolpaths. The cutter was quiet, left a good finish on the sides (but ripped the top not surprisingly) and did not heat up much so I'm sure it will go faster!

I did I video which I'll upload at some point.



as has been mentioned before, you will end up with a small dome in the center.

Strictly speaking they leave a small right circular cone in the center.

blackburn mark
22-08-2011, 08:03 PM
Strictly speaking they leave a small right circular cone in the center.

thats a dome to amyone with eyes over 30 :smile:



I accidently chipped one of the single flute cutters, but it turns out they are easy to regrind


now then..... i hadnt thought about that :) i need to dig to the bottom of my tool tray and start doing some grinding :smile:

Jonathan
22-08-2011, 08:06 PM
now then..... i hadnt thought about that :) i need to dig to the bottom of my tool tray and start doing some grinding :smile:

Hmm, if I hadn't said that I could have got myself a load of broken tools to regrind :lol:

blackburn mark
22-08-2011, 08:16 PM
hahahaha!!!! you dirty rotter !!!

i have this habit of collecting shit with the feeling that one day it will all make sense, there should be a medical term for it

at my age now i have a magic box of shit and whenever i need a stange item or a thingymibob i have a root in my magic box and nine times out of ten i find just the thing :)

packmansdaddy
25-08-2011, 03:16 PM
In the past I used two flute HSS and carbide cutters for my aluminium work. On my Syil X4 usually I did cut 2mm deep at between 5 to 8"/min (120 to 200mm/min).
With these single flute carbide cutters I can now cut 6mm (1/4") deep in one go. On my bigger X6 I can cut 1/2" in one go @ 100mm/min (4"/min). Plunging is a breeze.

Now, with these single flute carbide cutters I can cut much more efficient. And on my home made router I can now take 3mm (1/8") deep cuts in aluminium without problems. No more melting of acrylic either and 16mm cuts in MDF are a breeze... .
I uploaded two video's to YouTube

http://www.youtube.com/watch?v=re0IDJ8tzWw
http://www.youtube.com/watch?v=tC0rNbW9oV4

Compare these to a video I made some months ago and you will see why I am so happy. To add to the fun is the price of these single flute cutters. Cheap as chips.

http://www.youtube.com/watch?v=_2CHbSVJ8JY&feature=related

Originally I made these video's for my machine supplier, personally I have no connection to Syil or to Titan. i also have a Sieg KX3 (excellent small mill) and a 3'x3 1/2' table router I made myself as well as a 5'x12' Forfun router from China. Yep, I am an addict...

luke11cnc
25-08-2011, 03:24 PM
i tried to watch the first two video's but they are private ??

so I can't view them

James

m.marino
25-08-2011, 03:25 PM
You set the video to private and can not view it.

packmansdaddy
25-08-2011, 04:03 PM
sorry for that, have no idea really about this "modern stuff" but managed to change it. Hope you enjoy.

luke11cnc
25-08-2011, 05:54 PM
I can now view it thank you

cool machine you have there

James

luke11cnc
26-08-2011, 11:04 AM
I have ordered some today ready for when I'm up and running

James

Karl
26-08-2011, 01:32 PM
OK, let's just recap here. Are single flute cutters to be preferred over 2 flute (or more) cutters when it comes to working with hard woods such as oak?

We mostly do detailed (depth 5-10mm) v-carving and flat bottom clearance in small areas and therefore the feed rate rarely seems to get up to max' rate because of the stepper motor acceleration and de-acceleration times; feed rate typically 300-500mm/min.

packmansdaddy
27-08-2011, 04:05 AM
Hi Karl,

I am certainly no expert on cutters, just an ordinary user. I do earn a bit of money cutting stuff, mainly aluminium but also wood, MDF and plastics. I bought this single flute cutter because of its "good looks" and when I actually tried it (many weeks later) I was stunned about its performance.
As I take a lot of knowledge from the forum I thought I give a bit of info back as I am sure that some will profit using these cutters. As mentioned, I now can easily cut aluminium on my home made router as before, with whatever I tried, the results were not impressive.
You will have to try one for your application to see how it works. I made a nice holder for my collets in a "hardish" Australian timber, some kind of a redwood. And it worked fantastic.

I buy these direct in China as I visit there quite often
http://www.aliexpress.com/store/903014?tracolog=minisite_CP
but am not sure if they sell direct to outside China or what is the minimum quantity. There are also a few shops with the product on EBay and yes, there are high quality ones for a lot more money too. I regard the cheap ones as throw away's but never actually did throw one away yet. So far I made around 200 liters of chips with just a 4mm and a 6mm one.

I published the video's as I realized that I make big words and needed to back it up. I will make another one cutting off a 1/2" aluminium plate with a 6mm cutter in one go at 100mm/min (4"/min). All I can say is that I could not do this with any other cutter I have tried and I paid top dollars for famous brands. Not even close. Just give them a go and I am confident it will work just fine or you can use it for something else.

packmansdaddy
09-09-2011, 12:47 AM
Added one more video, cutting 10mm (3/8) aluminium bar stock with 6mm cutter at 100mm/min (4"/min). I do not want to risk to break the cutter so I cut quite slow. Did cut some parts in 1/2" aluminium in one go at 4"/min, no problem at all. Surfacing leaves a beautiful texture because of the center dome.

http://www.youtube.com/watch?v=fZVT8ORdQu0

I have excellent results in acrylic, MDF and ply. Just finished my new vacuum table for my small router (2'x3') and will try to make a video with the different materials.

packmansdaddy
09-09-2011, 06:04 PM
just added a small video cutting 12mm ply.

http://www.youtube.com/watch?v=n1QcqRAIDl4

This is the same cutter as I used to cut aluminium on my Syil X6. The finish is amazingly clean despite the high cutting speed. I usually do not cut this fast, only about half the speed you see on the video.

Jonathan
18-10-2011, 07:39 PM
Here's a video of the 6mm single flute on my router:

http://www.youtube.com/watch?v=bWmsunez7sw&feature=youtube_gdata

I think that was 1mm depth of cut... I now use a bit more at the same feedrate.

blackburn mark
18-10-2011, 07:50 PM
sweet :smile:

are you cutting dry ??

Jonathan
18-10-2011, 08:31 PM
are you cutting dry ??

In that video yes I think so. Now I tend to put a bit of coolant in the slot after each pass as it helps, especially on a small part where the heat otherwise just builds up.

blackburn mark
19-10-2011, 11:01 AM
In that video yes I think so. Now I tend to put a bit of coolant in the slot after each pass as it helps, especially on a small part where the heat otherwise just builds up.

i find it a bit of a dilema when cutting small slots... adding coolant tend to make the chips stick in the slot so theres a lot of re-cutting of chips going on or cut dry and clear the chips with a bit of air

i cut acetal dry and use WD40 in alli like you say, a couple of dabs on each pass..... watching your vid has me thinking that it may be worth me trying to cut alli dry more aggressive than i do so the chips clear themselves and forgo the coolant, it might be interesting to see how long one of these cutters will last cutting alli dry

the voice in my head tells me it will all end in tears but without a bit of science i guess we would still be eating bananas :smile:

Jonathan
19-10-2011, 02:19 PM
i find it a bit of a dilema when cutting small slots... adding coolant tend to make the chips stick in the slot so theres a lot of re-cutting of chips going on or cut dry and clear the chips with a bit of air

I use both methods when I care about the finish (either that or use a smaller cutter / cut wider slot). After the first few passes put coolant in the slot with pippete, wait for it to go round then blast the chips out of the slot with compressed air then put coolant back in slot and wait... repeat. Depends on the depth and size of the part you may not have to do this for every pass. If it's small part you do as otherwise the billet heats up a lot, then the chips start sticking.

Obviously the best way it to pump the coolant directly over the cutter, but that's not going to end well with an MDF bed!


and use WD40 in alli like you say, a couple of dabs on each pass

I use the white soluble oil coolant from the lathe.

cooliced
07-11-2011, 09:08 PM
This discussion has got me very interested.

I have a sherline mill, ive currently got hss 4 flute roughing end mill and i can safely goto 0.3 DOC at 350 mm/min. so cutting ally takes forever and the finish is shit tbh...

Do you think a single flute carbide cutter will be good for me??

Edit: i use WD40

JAZZCNC
07-11-2011, 11:00 PM
This discussion has got me very interested.

I have a sherline mill, ive currently got hss 4 flute roughing end mill and i can safely goto 0.3 DOC at 350 mm/min. so cutting ally takes forever and the finish is shit tbh...

Do you think a single flute carbide cutter will be good for me??

Edit: i use WD40

Yes they will perform far better in Ali than 4Flute hogger. . . . Also don't be afraid to go higher on the FR and DOC.
Depending on Max spindle speed you should easily double those figures.! (If machines upto it.?). . . Chipload is the key to cutting Ali (And most other materials) send the heat away with the chip and you'll be surprised just how deep and fast you can cut in Ali.!
Most of my work is cutting Ali and find blown air to clear chips mixed with the odd squirt of WD40 type fluid works best.

cooliced
07-11-2011, 11:18 PM
my spindle is 2700rpm max

if thats the case i will buy some.

will it give better finish to the work too?

JAZZCNC
07-11-2011, 11:46 PM
will it give better finish to the work too?

Well with out knowing what finish you get it's hard to say but I dont have any complaints. I very rarely cut less than 1mm Doc often it's 1.75mm @ 1100mm/min 10-12000rpm and still get a nice finish. Even when I'm being greedy and cutting upto 3mm Doc the finish is ok but it does wear the cutters quicker so found the best balance is around 1.5-1.75mm mark.
If I need fine finish then I just use a finish pass of 0.2mm and moderate feed rate.

Really you will need to play with your machine for the best balance regards ideal cutting speeds as every machine is differant but don't be affraid to let rip.!. . . You'll know when you've hit the sweet spot by the sound and the nice stream of chips flowing off the cutter.! . . . When a single flute is cutting sweet it's like taking a piss after you've been busting for hours.!! . . . Strong flow and nice Arghh sound. :rofl:

Jonathan
07-11-2011, 11:56 PM
4 flute end mill doesn't leave much space for chips at all, so they're going to get re-cut / rub etc causing the poor finish you describe. 0.3 DOC at 350 mm/min is pretty pathetic ... as Jazz said you should be able to get a lot more than that.
On my router, which compared to a mill isn't very rigid, I've been using 1.2mm DOC (sometimes 2mm for short periods) at 700mm/min and 12000rpm. Clear the slot of chips and put some cutting fluid in it before the cutter gets round.
Since your max spindle speed is 2700rpm, not 12000rpm, you want to reduce the feedrate roughly proportionately for the single flute cutter to get the same chip load and increase the depth of cut.

The video I posted earlier in the thread should give a reasonable idea of what it looks/sounds like. Finish is generally good - here's an example where I didn't do a finishing pass as such. 23mm thick if I recall correctly:
483348344836

And another with a different grade of aluminium (showing how grade can make a big difference):
4837

cooliced
08-11-2011, 12:29 AM
Thanks for the replies guys. ive hated watching the slow shitty speeds ive been running.

Gonna get some on order

cooliced
08-11-2011, 12:41 AM
http://i200.photobucket.com/albums/aa292/ubley/2011-11-04143625.jpg

that took about hour n half

HankMcSpank
08-11-2011, 10:17 AM
. . . When a single flute is cutting sweet it's like taking a piss after you've been busting for hours.!! . . . Strong flow and nice Arghh sound. :rofl:

I often wondered what the mist setting in Mach3 was for ;-)

cooliced
11-11-2011, 03:45 PM
dont suppose anybody has one of these spare i can buy, china are gonna take forever to get here and i wanna get cracking on!

PM me

Jonathan
11-11-2011, 04:25 PM
dont suppose anybody has one of these spare i can buy, china are gonna take forever to get here and i wanna get cracking on!

PM me

I can send you one at cost (eBay price divided by number in listing plus postage) - will PM you.
You'll soon be wanting more.

cooliced
11-11-2011, 04:51 PM
thank you very much

Stu

JAZZCNC
11-11-2011, 06:48 PM
Yep I just bought 5 will PM Ya.