Many things went wrong.
For the diameter bit you are using, you need more RPM, less depth of cut, and slower feed rate.
I would try 15k rpms, 0.5mm depth of cut, and 15ipm
Hello,
I have purchased Solid Carbide Spiral 'O' Single Flute, Aluminum Cutting 1/8 Dia x 5/16 Cut Height x 1/8 Shank x 1-1/2 Inch Long Up-Cut Router Bit with*Mirror Finish today for the first time I tried to use it, to cut aluminum plate (6061). unfortunately it's broke immediately after I started cutting ... I used this parameters: (metric units)
Spindle speed : 10,000 rpm
Feed rate : 30 ipm = 12.7 mm/s
Plate thickness : 6mm
Step down (Pass depth) : 1.5mm, 4 passes totally.
When I start the g-code, The bit inserted into the aluminium plate (depth 1.5mm) moved 1cm horizontally and broke into pieces.... What could be the reason ?! I post the g-code I tried & I will appreciate your help if you can run the g-code and find something wrong in it and let me know ( I'm a newbie) ... The g-code job size is 20cmx17cm.
Also I attached 2 picture for the aluminium plate .
Thanks
Murad assadi
Link to g-code https://drive.google.com/file/d/0B34...p=docslist_api
Similar Threads:
Last edited by assadi; 12-19-2015 at 11:38 AM.
Many things went wrong.
For the diameter bit you are using, you need more RPM, less depth of cut, and slower feed rate.
I would try 15k rpms, 0.5mm depth of cut, and 15ipm
If you are plunge cutting, I would reduce the feedrate for that, but it would be best to ramp or helix into the cut.
I used this parameters based on video tools today post (same bit),
what kind of machine are you using?
It's a CNC Routers homemade with 2.2 kW spindle, LAM technologies motors & drivers (nema 34 6.8Nm motors, X axis dual drive) DS1078 drivers, pmdx-107 spindle controller & pmdx-126 BOB, Invertek VFD Optidrive E2 - 2.2kW 230V 1ph to 3ph - AC Inverter Drive Speed Controller... Hiwin Rails... All extrusion aluminium
I will add some pictures for the machine if that will help...
Looks stiff enough, I would try to start out around 0.001" per tooth, and increase from there.
I think your original settings were around 0.003" per tooth, which is pretty aggressive for a 1/8" cutter.
Thank you Alan, I will try that when I get another bit and I already sent amana tools an e-mail asking them about that... I just asking because I want to learn and sometimes it's better to ask before just try and broke a lot of bits ...
Appreciate your help
Hi i agree mainly Wirth the other Posters but remember if cooling Stopps it bresks use high Feed Speed because the Chips Tend to glue on the cutting edges so less depths high Speed and extrem cooling saves your day ..,
Gesendet von iPhone mit Tapatalk
Sorry 1/8 i translate to 3mm the depths you are trying will never work on a machine you have (swinging ) i spend around 400 € in Routers to learn that the hard way and my machine is a heiz 400 T
So if you use 3mm never go deeper than 0,5 mm per pass when it breaks use less depth ,.. make sure the rpm fits to the federate the cutter is designed to (it is an different if you use single flute or 4 flutes )
i use 6mm flutes like you pictured (but from swizerland for 30€ per piece !!) where i can do max 2mm per pass but 30mm /s but 18k rpm and i cool like hell if cooling stops it breaks less than a second
but 3mm is too less material so you have to slow down and every little wobble of your machine (every machine wobbles ) will result in resonances which to my experience never work in your favor so breaking moe easier occur
thomas
Hi
Tkamsker is spot on there. I always use a helical interpolation (.35 Pitch) when using single tooth 1/8 carbide even for 4mm though holes ,although for holes slow the feed rate down to a crawl as my machines will try and shake themselves to bits. ( Multicam 5000 & Multicam MG both high gantry )I have a spindle speed of 18500 and feed at 500mm pm . If you are using a mister then you shouldn`t have too many issues but if not then WD40 before you start cutting on the tip then as it enters the stock give it another squirt every so often, you can hear when it`s starting to gum up. It`s a pain but with the spindle speed and feed rates you `re using then you should definitely be using some lube.
Thank you Thomas, I realised that I'm going to break a lot of bits until I learn , I have contacted the bit manufacture and they are amazing they refunds me the cost of the bits I broke which I didn't ask for ... And they told me
"To prevent you from breaking any other bits we suggest that you use the following starting points for your application with the use of the bit
6 Inches/Minute @10,000 RPM
11 Inches/Minute @18,000 RPM
It is strongly recommended to start at 70% of the recommended feed and increase it during work.
Note: For optimal results and extended tool life use mist lubricant system or air cooling.
All these spindle speeds to me sound massively high, i would be using around 8000 rpm with that bit at 1.2m/min.
Aluminum you want your bit as deep in the collet as possible.
Last edited by Jon.N.CNC; 12-23-2015 at 11:27 AM.
John what Kind of machine so You have ? I have Seen much differences in behaviour depending on machines on my Thojomech Vertical Mill i use Same alu and Miller Different ..
Gesendet von iPhone mit Tapatalk
It's an 8x4 diy router lol it is very rigid with aluminum moving gantry wieghing just under a 1/4ton but a vertical mill you should get even larger chip loads.
I know single flutes you use faster Rpms but I was using a 1.5mm single flute the other day at 12000 rpm 400mm/min.
If I were to try 18500 rpm @ 500mm/min with a 1/8th bit too would clog and break almost instantly. Flood cooling would slow it but like I say at the correct speed and feed it shouldn't clog your bit the second cooling stops. It should infact be fine up until the point the bit wears and blunts.
I agree happy Christmas
Gesendet von iPhone mit Tapatalk