First short video of machining aluminium. Still very new to this so any tips would be appreciated. I was playing with feeds and speeds during the test.
Started off with feed rate:
Attachment 24253
2mm DOC
https://youtu.be/MAfQFzEzogA
Printable View
First short video of machining aluminium. Still very new to this so any tips would be appreciated. I was playing with feeds and speeds during the test.
Started off with feed rate:
Attachment 24253
2mm DOC
https://youtu.be/MAfQFzEzogA
Air to clear chips and a bit of lube to reduce chip welding and increase cutter life.
There is so much variation from machine to machine that you either need data from someone who has done the same thing on the same machine or you start with about 50% of the recommended feed and see how it goes. You'll get a feel for what your machine will do before spitting the dummy in this way.
Keep a Workshop Log of good working feed/speed/depth/cutter figures, that way you build up a reference of settings for future jobs,
- Nick
Watched the video, lube would likely improve things a bit but if the finish is good, the size is good and tool life is good then it's good.
The camera man desisting from waving the camera about like a flag would improve things! ;-)
Haha thank you. I've got a knock off go pro that I might mount to the machine.
Thank you for the feedback really helps. I've bought some cutting paste and a uncoated endmill to try.Sent from my SM-N910F using TapatalkQuote:
Originally Posted by magicniner
70% Paraffin to 20% 30 weight oil is ideal for aluminium, WD40 works well too.
It is difficult to say anything regarding that video since I don't know how your machine looks like. To me it seems far too slow, but perhaps it is not possible to speed up more. Personally I'd prefer much faster speeds, like spindle speed 18krpm and feed rate 2700mm/min or maybe more. Here is a short video I made some time ago, milling at higher speed.Quote:
Originally Posted by dfox1787
https://youtu.be/LFFyb2XtpkE
Note that I am using 4 flute bits, to me they work better. I don't use any lubricants, only the vac with dust shoe. That is enough, nothing gets hot if I don't slow down the feed rate too much and rub the bit.
Does seem like a very slow feed, but as above with no details on your machine it's hard to know... sounds like the tool is chattering a lot. Is it really only 5k rpm?
You can reduce your tool stick out a lot there... ideally you only want enough of the tool sticking out to clear any fixings and get as deep as the bottom of your work piece. Obviously you don't want to insert it into the collet deeper than the shank but consider using shorter tools where appropriate as this will reduce tool flex, reduce chatter and minimise any runout issues.
I use mist coolant and air blast when machining alu and that works great for me.
You are also using adaptive there but you don't show your axial engagement (it's on the 4th tab). You can reduce this to suit the rigidity of your machine while also upping the Depth of cut to get more of the cutter length engaged.
Thank you. My spindle isn't at 5000 sorry. It was at 18000 and I was adjusting it as the cut went on. I use air blasting but no mist as I'm machine on top of mdf.Quote:
Originally Posted by Zeeflyboy
I've got a Chinese 3040 not great i know. I was using a 3 flute tian coated endmill.
Sent from my SM-N910F using Tapatalk
Feed is way too slow for that RPM imo.
Try a feed of 1000mm/min with around 12,000 rpm and an axial engagement (again, found in the 4th tab) of 0.8mm... these chinese machines are a little ropey so play around with the rpm to find one that sounds better and doesn't cause resonance in the machine.
Don't use TIAIN coated end mills in aluminium... the aluminium nitride causes the aluminium you are cutting to weld to the cutting edge. You can probably see where the coating has turned silvery already - that's your alu ending itself to the cutter.
Much better just to use uncoated carbide and a good mist coolant.
Yep, too slow. Need max RPM and increased feedrate.
For a 4mm (on a larger machine), id cut 24K RPM and probably 1000-1500 mm/min, if the machine can cope.
Here I am doing 4000 mm/min with a 6mm endmill (4KW spindle).
https://www.youtube.com/watch?v=QAv-q9P4FjA
Thank you. Ill have a play with the settings. Here are my settings for the current part i was practising on.Quote:
Originally Posted by Zeeflyboy
Attachment 24259
Yeah so I would reduce that optimal load down to something around 0.8mm and increase your maximum step down to the tool diameter to start with (so 4mm here). This will engage more of the cutter length but reduce the amount it's trying to move into the part on each pass. The way you have it set up currently it's the bottom 0.5mm of the tool that will be doing all the cutting and you'll wear it out much more quickly.Quote:
Originally Posted by dfox1787
Keep the optimal load low as this will help with your lack of rigidity. I rarely use anything more than 1mm on my machine which is a 6040 with linear rails.
If doing slot type clearing like in your video, try selecting "both ways" from the milling direction drop down. It means you aren't wasting time with a travel move each time it goes across the slot and can save a lot of time on those sort of operations. Just make sure you are leaving eg 0.2mm stock in the radial direction and then run a clean up contour to finish the edge.