Fine People fo Open Builds... My weekend plans have gone slightly amiss dues to having to take my daughter to A&E, the right of passage I think... Anyhow as everyone is ok and just a bit bruised I thought I would pick up my calibration block. I have modelled this based on Ryan's video on Ooznest. It is a 60 X 60 square, with the second square cut down to calibrate the Z axis. I have made my fusion model available at the following location: A360 you can see the model and CAM profile. So I've modelled a fair bit before in Solidworks and Fusion, but have no experience of CAM apart from my WorkBee which is only 4 or so weeks old. Alex Chambers posted some useful notes on feeds and speeds and this is the area I am probably most nervous about. I usually cut wood, and take fairly light passes, this is Aluminum and would rather not break my endmill. These are the settings I have used, can some more experienced eyes have a look and give me the benefit of their experience? To give a complete picture this is a photo of the setup of the workbee. As always, thank you for reading... Regards Colin.
I'll let someone with more experience comment on the speeds and feeds @Colin Hart, but do you know what your aluminium is? Most people on here recommend 6061 aluminium - some alloys do not machine very well. Alex.
That's another alloy I have seen mentioned as machinable - so probably no problems there. Where did you get it from? Alex.
It was an ebay purchase: Aluminium imperial flat bar 6082 upto 6" (152mm) wide + free cutting & p+p | eBay
As a newbie and comming from a completely different angle in so far as CAM/CAD software is concerned I can offer you completely nothing by the way of help , but I am following your thread with interest and most importantly I do hope your daughter is OK Regards C
Ok.. So not sure what went wrong, if it me, feeds and speed of the alloy is to hard, bu judder, deflection and I have to stop the job. some re-thinking is required. maybe back in at the weekend, but also may do a calibration cut on a hardwood.
6061 cuts like butter, but only if you can push it hard enough. When it comes to machining metals, you need some meaningful guide rails to get started with. This seems like a good option: Harvey Tool - Speeds and Feeds Guide | General Machining Guidelines So in this instance, assuming that's a 1/4" endmill... 1) Don't be too conservative on the speeds. Rubbing kills endmills quick. I'd go for maybe 1100 SFM. 1/4" tool has a circumference of 0.7854". 1100 feet is 13,200". 13200/0.7854 = 16,800, rounded. That's RPM. So off the bat, you need to increase your spindle speed. 2) Feedrate. At 16800rpm, 0.002" per tooth is 33.6IPM. That seems very low to me for a 17000rpm spindle, not even 1000mm/min. I'd be ready to increase that, but the machine may not be able to handle much more. Leadscrews and CNC (climb) metal machining don't go very well together. You have it set to 0.0254 (0.001") per tooth, which combined with the low speed is probably causing rubbing and intermittent engagement. Bump it up so it says 0.05mm/tooth and somewhere in the ballpark of 850mm/min. Based on what I just calculated, feed per rev for a 4 flute should be 0.2mm, not 0.02mm. Something's way off there. That said, before I go any further. 1, you should really be using a 2-flute end mill, aluminum is gummy and likes the extra gullet space. It also would reduce the requirements of the machine- you could half the feedrate because you'd be taking off half as much material per rev, which is also half the spindle HP requirements. 2, that cutter is TiAlN coated. Guess what that contains? Yup, clue's in the name, it's aluminum. Aluminum loves aluminum, it's like silicone in that way. You're gonna have to take major precautions to eliminate chip welding, which is where the aluminum basically welds itself to the tips of your cutter and you have to scrape it off with a steel rule, taking your coating with it. But before that, it causes massive amounts of friction heat, destroys your cutting edges, chips your carbide, and makes a big mess of the part. Best to go uncoated or maybe, what is it, titanium boride? Something like that, there's a bunch of aluminum-friendly coatings out there now. Though coatings do change your feeds and speeds as well, and sometimes you need way more power because they want to run at high temperatures and pressures. I'd just go uncoated (or even HSS, typically takes less cutting force than carbide and is less brittle/susceptible to shock). A good airblast or mist coolant would be ideal, keep the cutter buried and cutting full chips, no rubbing. Chip thinning might still get you depending on the geometry, that's something you'll have to look into because it's pretty context-specific. Oh, and focus on chip evacuation so you're not recutting chips, that'll kill your cutter too. Airblast helps there as well. TL;DR: These machines aren't really designed for metals, you'll still have to learn basic machining, and even then you might still not be able to. But hey, give it a shot, right?!
