Tool Life Expectations?

Evening Gents,
.
As I'm still on the toolpath/feeds & speeds/machine enhancements learning curve and having done a few jobs now, with varying results (and a number of worn out tools) I'm wondering what the kind of ball park tool life expectancy is in general?
.
I am pretty sure the answer is "it depends" and on a number of variables such as those on the learning curve in the previous sentence, so I'll give a few parameters to see if you guys have similar experience and how long your cutters remain sharp enough, as I am finding I am going through an 8mm HSS cutter every 2-3 hours of cutting and a little longer for Carbide (3-3.5 hours), but not that much longer.
.
My current rough parameters are:
.
Material: 6082 T651 Aluminium
Cutter: 8mm HSS and/or Carbide
Flutes: Single for the Carbide and 2 for the HSS
RPM: 10,000
Feed: 800mm/min (plunge using 600mm/min but ramping this over 10mm)
DOC: 1-2mm (I had an accidental 5mm cut once, but that was a shrieking mess, but at least didn't break the tool)
Step-over generally 40-45% but also some slotting, which actually seemed to help with chatter (at least whilst the tool was sharp)
.
I have had a few loose bolts & misaligned ballscrew issues on the machine, which I've resolved over Christmas and also have just got hold of a 50litre compressor, which is way, way better than the asthmatic gnat compressor I had previously, so clogged chips should no longer be an issue as well, which didn't help tool life previously.
.
The main reason for this post is to get a reference point for tool life, which will help with a benchmark to aim for in terms of tweaking parameters and also whether I'm going to be charging customers for a new cutter as standard when I quote for a job, not that I like charging for essentially learning on the job......
.
Oh and whilst I remember, I have noticed the behaviour seems to be that the HSS cutters run fairly noisy to start with and gradually get worse until chatter etc. gets too bad and force a tool change, whilst Carbide (especially the single flutes) are almost noiseless but when they do go blunt, seem to drop off a plateau and deteriorate rapidly. I'm wondering if that is normal for the cutter types?
.
Later and also Happy New Year all......
.
.
Chris

PS. I have been buying cutters from APT and RDG (ebay) but also see some what seem to be very cheap cutter from a seller called Supermario-au - anybody bought from this seller? (looks to be Chinese and I havenothing against going that route for the price , but its always a punt on what you get).

I have the 6mm single flute carbide cutters from Supermario and they are fine for the cost.

You probably know about these anyway, they do a reasonable job at 'tickling' an edge, though you'd struggle on spiral bits :whistle:

DMT Mini Whetstones - Diamond Stones - Sharpening - Hand Tools | Axminster.co.uk

Thanks Eddy,
.
They are much prettier than my old oil/whetstone - might have to get one just to lighten the workshop up :) I also have my sights set on a bench grinder/sharpener (if Arceurotrade ever get the one I want back in stock - Bench Grinders - Arc Euro Trade) as I need something for my HSS lathe tools.
.
I'll definitely go for some of the Supermario ebay cutters as well, as they are way cheaper (and probably the same thing) as the APT single flute cutters I have been using - thanks Goblin.
.
Perhaps we should have a "trusted suppliers" sticky at the beginning of most of the sections on here, like the CAD/CAM one, to save a lot of googling etc.
.
BTW - how long do your cutters last chaps - I have this image of Jazz or Jonathon putting 5 year old and never sharpened HSS cutters in their collets and mocking my cutter's lack of longevity (or rather my lack of machining knowledge leading to their early demise) :friendly_wink:

Quote:

---

Originally Posted by Washout

I also have my sights set on a bench grinder/sharpener (if Arceurotrade ever get the one I want back in stock - Bench Grinders - Arc Euro Trade) as I need something for my HSS lathe tools.

---

Nice looking grinders, the seas must be rough from China at the moment.

Quote:

---

Originally Posted by Washout

I'll definitely go for some of the Supermario ebay cutters as well, as they are way cheaper (and probably the same thing) as the APT single flute cutters I have been using - thanks Goblin.

---

Is that the one in Australia ?

Quote:

---

Originally Posted by Washout

BTW - how long do your cutters last chaps - I have this image of Jazz or Jonathon putting 5 year old and never sharpened HSS cutters in their collets and mocking my cutter's lack of longevity (or rather my lack of machining knowledge leading to their early demise) :friendly_wink:

---

I'm only cutting hardwood wood and I'm finding they don't last very long, the Axminster seem to do quite well and Tilgear Viper cutters came out tops once in a magazine test.
If I need something quick and disposable when the jobs done I go for something like this.

Toolstation > Power Tool Accessories > Router Bits > Kitchen Fitters Router Bit Set

Currently about 3-4hrs from a 2 flute 6mm APT carbide end mill churning it's way through steel, however I reckon I'd get a bit longer the mill that on wasn't so underpowered and could take a decent cut!

Eddy - I am pretty sure the description for the Supermario-au seller was that the cutters were coming form China - will doublecheck....
.
Yep - definitely China but also some from the same shop from Hong Kong, but that's not unusual for stuff from that neck of the woods http://www.ebay.co.uk/itm/5x6mm-Germ...item1e667696d2

These are the ones I use : 5x 6mm Carbide CNC Router Bits Single Flute Tools 25mm | eBay

Quote:

---

Originally Posted by Web Goblin

These are the ones I use : 5x 6mm Carbide CNC Router Bits Single Flute Tools 25mm | eBay

---

That's why I couldn't find supermario on uk ebay it's supermario-au

Well not 5yrs but certainly longer than 2hrs from HSS. I want at least 6-8hrs from HSS and I get couple of days cutting from carbide, obviously depends on the finish your looking for to when you call them knackerd. I always finish with a 0.2mm finish pass.

Now The secret to great tool life is to use 3F Carbide roughing cutters then finish with HSS or Carbide tools. This way cutters last ages and the serated edge roughing cutters allow 3-5mm pass's with no problem. I also nearly always use 6mm tooling with 8mm being the max.

Cheap cutters are pointless I find and waste of money but I have had the Mario cutters before and they are ok and gave decent life I think, certainly no worse than others I've used.

Cool - that gives me a target for now in terms of tool life from where I am now.

I'm certainly expecting the better compressor to help, as I'll not have slots full of cut chips - although they'll all be stuck in what's left of my hair I expect ;-)

I'll buy some serated edge cutters to play with - they are often called rippers?

I've shied away from 3 flute cutters due to the previous frustrations and lack of feed-rate I could get, but will have a go again now my machine is a lot smoother than it was due to Christmas hols maintenance and the new controller board, which I should have up and running tomorrow.

Luckily the parts I'm cutting for a customer can be left at the rough stage, as they are for a sub-frame to chassis mount and hence buried in the bowels of an engine bay away from public view. He is well happy with the 2 I have shipped already (especially as I can sell them cheaper than the OEM) :-) even if I need to charge a cutter for each part, which with extended tool life over what I have currently I shouldn't have to do. Of course there are many parts which are not so hidden I need the finishing pass on......

BTW - is that tool life using "normal" toolpaths or iMachining/HSM? There are some stunning youtube vids of the latter in steels albeit on what must be very rigid moving bed mills rather than the gantry type and they are claim 70%+ better tool life - shame the continental company that makes the software is not more Google/Trimble rather than Autodesk in terms of price point ;)

Quote:

---

Originally Posted by Washout

BTW - is that tool life using "normal" toolpaths or iMachining/HSM? There are some stunning youtube vids of the latter in steels albeit on what must be very rigid moving bed mills rather than the gantry type and they are claim 70%+ better tool life - shame the continental company that makes the software is not more Google/Trimble rather than Autodesk in terms of price point ;)

---

No that's conventional cutting and yes the I-machining does indeed improve tool life massively but like you say it's resoanably hard on the machine if run at the higher settings but it can still be fine on even larger gantry machine like mine.
Here's a rough shaky video of my machine doing a little, these are just roughing passes, was finished with 4mm and conventional wall & floor paths. This was level 2 and theres 8 levels plus turbo mode.!! The DOC is 7.5mm but only because flute length was only 10mm other wise it would have done it full depth 15mm just has easy and at same feed etc. CNC Stepper spacers using i-machinine toolpaths - YouTube

This is the finished part just off the machine.

Awesome - the material removal rate is fantastic compared to the raster/offset paths I'm using out of Vetric and there's something very "right" about chips and the way they come off of the cutter.

2000mm/min doesn't sound too aggressive (I assume that's the rough maximum as iMachining varies the feed) - I was expecting 3-4000mm/min max, but as you say its No. 2 out of 8+ settings.

If you arrange an intermittent drip feed of cutting lube (I use a 20/40 mix of 30 weight oil/paraffin) into your chip clearing airstream you'll increase cutter life.
I introduce the lube with a separate pipe overhanging the air nozzle by 5mm or so to ensure a coarse droplet size that settles quickly and avoids aerosol lube in the workshop air,

- Nick

Thanks - I've been thinking about a replacement nozzle for the airbrush I'm using (would like the airbrush doing what I bought it for ;-) ) so that's giving me some more ideas.

Now if I can just work out why my new Optoport V3 isn't turning my steppers (can't seem to find out what pin Enable is supposed to be configured for in MACH3) I'll be able to test it.

Quote:

---

Originally Posted by Washout

Thanks - I've been thinking about a replacement nozzle for the airbrush I'm using (would like the airbrush doing what I bought it for ;-) ) so that's giving me some more ideas.

Now if I can just work out why my new Optoport V3 isn't turning my steppers (can't seem to find out what pin Enable is supposed to be configured for in MACH3) I'll be able to test it.

---

Chargepump enable output is pin1, if you cant get MACH3 outputting a chargepump signal to pin 1 jumper J13 on the board overrides...

Ah thanks Irving - I did wonder but the manual is a little cryptic - I'll give that a go now.

Quote:

---

Originally Posted by Washout

2000mm/min doesn't sound too aggressive (I assume that's the rough maximum as iMachining varies the feed) - I was expecting 3-4000mm/min max, but as you say its No. 2 out of 8+ settings.

---

Well it doesn't so much change the Feed but more it adjusts the stepover when you go to higher settings.

How it works is by varying between a Minimum and Max stepover and feed rate in differant areas to maintain a constant chip load and positive tool engagement.

To give an example of going one setting higher. 8mm Carbide 11mm flute length cut depth 15mm done in 2 passes [email protected] DOC 2nd @ 6.6224mm

#2 setting
Min Step over 0.160mm Max 1.050mm feed 2411mm/min Spindle speed 13,571Rpm x 2 steps . . . . Cut time per part 3.27mins
#3 setting
Min Step 0.560 Max 1.710 Feed 2498mm/min 14,667Rpm x 2 steps . . . . Cut time per part 2.10 mins!!

My machine would have handled this and possibly higher but didn't want to push it.!

Just for giggles.
#8 Min step 2.880mm Max 3.310 Feed 3902mm/min 16.213Rpm x 2 steps . . . . Cut time per part 0.52 Mins.!!!!

This would rattle my machine into pile of nut n bolts and melt down the spindle. . Lol

Funny enough Same but with flute length to allow full 15mm DOC so only 1 x pass isn't that much quicker due to lower STO & feeds.
#2 Cut time per part 3.08 min
#3 Cut time per part 1.54 min
#8 Cut time per part 0.42 Min

Edit: Oh by the way just checked code and that video was done on setting #1 not #2 and thats why feeds are lower at around 2mtr/min. Total time for 3 parts was around 15mins I seem to remember.?

Even on setting #1 that's still a very impressive performance.

I seem to have hijacked my own thread ;-)