Printable View
Hi All
Up until now I have only routed wooden plastic etc, but wanted to make a custom set of car peddles in aluminum. Nothing fancy it's a very old mini and wanted to make some round peddles with the Leyland logo on, and just wondered if anyone had any advice on things to do different to routing wood plastic etc, like faster or slower spindle speed and x and y axis speeds.
Many thanks
:) Don
assuming your going to use a brush to clear the chips, plenty of WD40 and at a speed you can keep the chips clearQuote:
Originally Posted by don_jarr
some alli will soon clog and snap your tool if you dont keep it clear
i tend to go a tad easier on the feed with alli than i do in acetal with 1mm depth of cut if im feeling brave and 0.5mm if im not
I was cutting about 0.5mm depth at 750mm/m with maximum spindle speed. I used a LOT of Wd40 and it got very hot.
I ran out of wd40 and clogged my tool before i was finished!
I'm using a 1.5kw spindle, using a 6mm end mill. 4 flute.
Bloody hell no wonder it got hot at 7.5mtr/min thats miles too fast for cutting Ali with a 4 flute cuttter. Wouldn't go much above 2.5mtr/min.!! Actually I wouldn't be using a 4 flute cutter full stop on Ali. Single flute cutters are far superior for cutting Ali.Quote:
Originally Posted by jcb121
My advise based on the fact I 95% cut Ali is.
No1 use single flute cutters on Ali, twin if cant get single but try stay away from multiflute.
No2 Don't be shy on the DOC you want a decent chipload so 1.5mm @ 650-700mm/min 12-13K rpm this will give a nice chipload the chips should be very hot but work piece only slightly warm. The goal is to get the heat to leave with the chips not stay in the work piece or tool, incorrect chipload is what causes chip sticking due to overheat.
To be honest it's trial and error to some degree and every machines sweet spot will be slightly different depending on how well built etc. . .BUt it's common for folks cutting Ali for first time to go too conservative on feeds and speeds, and esp DOC. Taking too little DOC actually heats the cutter quicker and causes sticking and wears tool away faster.
WD40 works good for coolant but better still is blown air with the odd squirt of WD40 has it clears the chips so your not recutting chips giving poor finish.
Also for best finish always finish off profiles with a slower 0.1mm full depth finish pass. The chips will look like little needles.!!
Looking forward to an alu cutting demonstration in the near future! ice.
Hi All
many thanks for the info, I will get a couple of bits of alloy sheet and have a play and if the results turn out ok post some pictures.
Many thanks again
:) Don
When you say sheet what do you have in mind.? . . . Reason I ask is, if thin sheet 3-4mm then most tends to be low grade 1050 stuff and very shity sticky stuff. The grade of aluminium makes a big difference to cut quality. I mainly work with 6 series, 5 series if I have too but not keen unless harder grade 5083 H32 has lesser grades can be sticky with hard spots.!!Quote:
Originally Posted by don_jarr
Hi m8
I have no idea the grade, its 4mm thick from where my dad used to work and when they shut down it was being chucked out, so I grabbed it all, (like you do when no one is looking lol). Its quite hard to drill, but they used to make displays cabinates, so guessing its not going to be high grade stuff seeing as it was only for shelves signs and odd stuff like that.
:) Don
Chances are it is.!! . . But You'll know soon has you start cutting. . It gums up the cutter and gives a really bad finish if the feeds and speeds are not perfect.
When you have it wrong it tends to leave a torn like finish, mainly because thats whats happening. Because it's soft it's getting torn rather than cut away if the feeds and speeds arn't correct. . . . . Unfortunatly can't help much here has it's trial and error more often than not finding the right cutting conditions for this shity stuff.!!
The one thing I will say is don't take your eye of it for a minute because when it does start to gum up the cutter it happens very quick and with only a slight audible warning.!!
Cutting this stuff is the one time I do recommend you use absolutly loads of cutting fluid other wise it will gum up for sure.!!
Hi All
Well had a bash and adjusted the speeds as recommended to start from, and only had a 2 flute cutters but they were all new so nice and sharp and apart from altering the cut depth to make it a bit shallower which meant it took longer to do, they came out ok. Bit of clean up along the top edges, but by the time there polished and painted they will look ok. Pedals done, now onto the gear gate.
Will post pictures asap, and many thanks again.
:) Don
Thanks for this post , I was also having problems cutting the thin 3mm stuff, just clogs up no matter what I tried, still haven't found a good feed & speed for this . Guy in Ali shop told me it was 6061. I downloaded trial of G-wizard but that still wouldn't give me good numbers. Does anyone have some suggestions of numbers I could try for this shitty 1050 3mm.
Cheers
Riche
Sent from my iPhone using Tapatalk
From my experience with cutting aluminium I believe coolant and amount of coolant is very important. It is not only cooling factor, but chips removal and lubrication as well.
I use plain diesel, strait from petrol station as a coolant. It's cheap, available, does not cause corrosion and it is not likely to get bad. In fact it protects my machine against rust.
As an example, to cut my aluminium plate for my PC cooling system I used 4 flute HSS 3mm dia end mill available from UK online shop. There was no clogging and broken end mills at all. I don't remember feed rate and DOC( it was few yars back), but most certainly I wasn't creating alu dust.
Obviously using two or single flute carbide bit would be advantageous, but milling in a way I did proves significance and necessity of coolant.
I have to take my hat off to you lot, I'm amazed you can cut it at all with a router, I have trouble milling the stuff.Quote:
Originally Posted by riche543
Not the same trouble mind you, My problem is holding it down because the tool tries to lift it and it doesn't resist much.
I think it is practically pure aluminium, not enough magnesium, you could probably stretch it into a Coke can but that means the tool can push it out the way rather than cut it. Any interruption of the suds and the tool clags up, stops cutting and starts extruding.
Yep you can't beat GOOD flood coolant but it's not practicle for most router based machines and here lies the problem.?Quote:
Originally Posted by wiatroda
Unless you have high flood cooling so the chips are getting washed away constantly then using a coolant how most do it by just brushing or spraying a bit of WM40 etc soley is more trouble than it's worth.? . . . It clogs the slot and makes the chips stick to the material rather than wash away, this results in chip recutting and actually creats more heat than cools. It also leaves a very poor finish and kills cutters prematurely.
Blown air with a slight mist is by far the best method for cutting ALi on a NONE Full flood coolant machine, mill or router based. (It's messy thou)
I use a dedicated air mister now but for years just used to blow the chips away with the odd occasional squirt of maintenance spray and just doing this gives far better tool life and finish than brushing coolant on.
To get good results and tool life in any material you need the heat away with the chips but in Ali it's even more important due to the sticky nature of the stuff and this can be achieved dry with good chipload and IME dry cutting with the correct chipload is far better than brushing the odd bit of coolant on.
Try kerosene(heater fuel) it's far cheaper and works just has good.Quote:
Originally Posted by wiatroda
Robin If I had a pound for every body I've spoke to about building machines and when asked what they are doing about material clamping it never even entered there minds.!! . . . .Clamping must be the least thought about aspects of DIYCNC and yet one thats very challenging to get right and very frustrating at times resulting in many a few hours lost due to material lift or moving.!!Quote:
Originally Posted by Robin Hewitt
Yep thats exactly what happens with the 1050 stuff it just deforms and gets pushed or torn out the way eventually wrapping it's self around the cutter like chewing gum.!!. . . .I hate the bloody stuff, I'd rather cut it with pair scissors. .LolQuote:
Originally Posted by Robin Hewitt
Got some 5083 4mm plate today , was told its hard & expensive too get 6061 that thin? . Also think my remaining 3mm carbide cutters are now dull ,from trying to cut crappy 3mm 1050 ,ally guy said the 3mm I had previous tried too cut was not 1050 was 5005 ?. Anyway Now have 5083 tried recommended feeds & speeds from g-wizard started good but then snapped after a minute or so. They didn't gum up just clean snap is this due too the bits being dull?
There isn't really a good supplier of end mills here in Australia so have too order from the US , which takes few weeks too arrive so wasting Bits gets frustrating.
Cheers
Riche
Sent from my iPhone using Tapatalk
Quote:
Originally Posted by Robin Hewitt
JAZZ , My wet router is nothing special, going from bottom up it is steel frame + 18mm mdf board from wickes, painted thick layer of 2k paint + another plywood board( mounting one to which I screw all sheets and pieces) + waste 2-3mm mdf or cardboard. Recently, after maybe 2-3years, I replaced the mounting sheet - It's due too many holes in the old one. Plus there are steel and wooden border to keep liquid contained. Old swimming pool filter + cheapest 3 speed CH pump. Whole bed is slightly slanted to allow for nice return of coolant Does its job.Quote:
Originally Posted by JAZZCNC
Kerosene is cheaper( I thing 1/2 price of diesel) but whole effort to find supplier - not worth it when petrol station is behind the corner
Robin, I use simple way of clamping - drywall screws with big washers. First I mount material from outside then mill all inside profile+holes, after this mount material from inside or through holes, remove outside screws then mill outsides.
Amateurish?? YES , but does its job
Sounds good I like the KISS approach and you obviously prepared for using coolant but most DIY builds don't and has you know unprotected MDF is useless if so much has show it cup of coffee.!!Quote:
Originally Posted by wiatroda
I used to have similiar setup untill last year when I changed to Ali bed and must say I do like it a lot better now but for some jobs it's not has easy as the MDF/screw method and I do actually still use MDF. The difference being I only use small offcut pieces that I throw away after several use's and only for certain jobs.
The main reason I shifted from the MDF bed was the constant movement so could never relay on it being flat or true, always having to surface it flat when jobs required it.!! . . Now it's the other way round I always have a flat and true surface to work from. When cutting jobs that are non surface critical and require thru cutting then I use MDF has a spoil board.
I also use HDPE for accurate spoil boards, HDPE is a nice stable unform thickness so can be relied upon not to change shape and stay resonably flat. It's also easy to screw into and doesn't blunt cutters like MDF.
Because my bed is quite large tend to devide it into segmants and use fixture boards located at a known positions on the bed then use fixture offsets in G-code so I can cut several different jobs on table.
The beauty of this means I can mount different materials on the table while one job is cutting then when it's finished that job it will move to the other fixture and start on the that material and I can remove the fixture plate with just completed job. . . . I also keep one area free that I can work direct off the bed.
Another plus to doing this means I can make better use of expensive offcut material like ALI or Brass.? So long has I know it's large enough to get the job out of and I position it in the correct place on the fixtures then I can cut several parts from scraps at the same time at any location on the bed I choose.
Basicly I draw the part with the X0-Y0-Z0 relative to the corner of the board then select G54,55,56 fixture offset for the selected area on my bed and assign it to this job. Each job has it's own offset code and when finished moves to the next offset and starts again at X0-Y-0 which is relative to the corner of the fixture board.
Doing it like this means I can set several jobs off in different materials in one go and walk away. . :yahoo:
Hi Jazzcnc,
Reading your answers on this thread is very helpful....IE speeds and feed rates. I have the 2kw Chinese spindle now, about to use it this week hopefully. I have ordered several 6mm single flute cutters. What about drilling through ali ? would it be the same setup and the same cutter ? what drilling method is best ?
Depends on the size of the holes. Up to about 4mm you can get away with good quality HSS drills, but any more than that is difficult because of the limited power these spindles output at low rpm's. Instead you have to use carbide drills, or mill the holes if they're big enough. Using a carbide drill worked extremely well for my bed hole array. I'm not sure if the flood coolant was required, probably could have got away with applying coolant manually if it wasn't so many holes:Quote:
Originally Posted by dudz
http://www.mycncuk.com/forums/router...html#post38578