Aluminium cutting

**Washout** · 22-04-2014

At the risk of a bit of shameless self-promotion here's my channel link on Youtube - https://www.youtube.com/user/CCWashout/videos
.
The 5th Video is probably the best one with the two 5mm deep pockets being cut - the noisiest thing in the room was the compressor, but I have made some horrendous noises previously when F&S have been wrong, misting not running properly etc. Oh the description for that vid is slightly wrong as the previous vid was an 8mm Carbide Single Flute and the 5th vid uses a 6mm End Mill @16439rpm, 2mm DoC, 539mm/min.
.
I'll back Jazz up and recommend ramping for single flute cutters - I've broken the tips off of a number of them by plunging and I tend to find if you have to plunge try and set that in your CAM software at ~30% of your normal feed rate.
.
One of the things I found frustrating is the CAM software I am using, as Vectric's Cut3D and 2D does not always consistently apply ramping and in the case of Cut3D doesn't give you a ramping option at all. I am mostly using Deskproto now which does apply ramping, but only if there's enough room on the first move, but at least I can force it to plunge if there isn't at 30% feed.
.
I'm still learning myself and will post more vids as I progress and if you want to see something really cool look at Jazz's video of his machine using iMachining trochoidal toolpaths - that stuff is amazing (one day I'll be able to afford that :-) ).

**corkcnc** · 24-04-2014

Just wondering why you didn't climb mill the 5mm pockets in the vid. Don't take this as a criticism as I bow down to your ability to self build such a nice looking machine. You would find yourself with a longer tool life though if you did all of the 5mm in one pass and cut the pocket using 30% step over. You could increase the feedrate then due to the chip thining so you would have a nice increase in material removal rate. I understand that you are not looking to lash off 1000 pieces so time probably isn't a bit deal but it would be better to let the whole tool wear a fraction than the bottom 2mm wear while the top section does no work.
Regarding speeds and feeds calculators I have a nice .xls file which I got from my tooling supplier. When I read the figures that came out first, I said no way, surely the tool can't handle it but they do. It gives you a range of speeds for carbide and hss tools, which is useful, as if you want to apply it to different brands of tools you can put in the lowest settings and still be in the ball park for things like stainless. Then you can speed up if the conditions allow. If anyone wants a copy just pm me and I'll send it on. One important point though is that I have a rigid NC bridgeport and home made machines wouldn't be expected to have the same rigidity so carbide tooling may not be suitable at high feed rates if vibration is an issue.
Regarding tool paths I'n keen to see how m_c gets on with generating trocoidal paths with cambam. If the software can do that for under £100 it sounds like a great deal. I use trocoidal all the time and cringe when I have to put a tool into a corner when the rads limit my options.
Rgds,
Noel.

Originally Posted by Washout

At the risk of a bit of shameless self-promotion here's my channel link on Youtube - https://www.youtube.com/user/CCWashout/videos
.
The 5th Video is probably the best one with the two 5mm deep pockets being cut - the noisiest thing in the room was the compressor, but I have made some horrendous noises previously when F&S have been wrong, misting not running properly etc. Oh the description for that vid is slightly wrong as the previous vid was an 8mm Carbide Single Flute and the 5th vid uses a 6mm End Mill @16439rpm, 2mm DoC, 539mm/min.

**JAZZCNC** · 24-04-2014

Originally Posted by corkcnc

Regarding tool paths I'n keen to see how m_c gets on with generating trocoidal paths with cambam. If the software can do that for under £100 it sounds like a great deal. I use trocoidal all the time and cringe when I have to put a tool into a corner when the rads limit my options.
Rgds,
Noel.

Yes when you've used Trocoidal toolpaths you really don't want to go back to normal milling. Like Washout says I use i-machining (mostly for roughing) and it's unreal the material it shifts and time it saves even with my low powered spindle and DIY built machine. To watch it dance and chomp 6061 T6 @ 20mm depth between 2500 & 3000mm/min and do it with ease is amazing.

**Washout** · 24-04-2014

Originally Posted by corkcnc

Just wondering why you didn't climb mill the 5mm pockets in the vid. Don't take this as a criticism as I bow down to your ability to self build such a nice looking machine. You would find yourself with a longer tool life though if you did all of the 5mm in one pass and cut the pocket using 30% step over. You could increase the feedrate then due to the chip thining so you would have a nice increase in material removal rate. I understand that you are not looking to lash off 1000 pieces so time probably isn't a bit deal but it would be better to let the whole tool wear a fraction than the bottom 2mm wear while the top section does no work.
Regarding speeds and feeds calculators I have a nice .xls file which I got from my tooling supplier. When I read the figures that came out first, I said no way, surely the tool can't handle it but they do. It gives you a range of speeds for carbide and hss tools, which is useful, as if you want to apply it to different brands of tools you can put in the lowest settings and still be in the ball park for things like stainless. Then you can speed up if the conditions allow. If anyone wants a copy just pm me and I'll send it on. One important point though is that I have a rigid NC bridgeport and home made machines wouldn't be expected to have the same rigidity so carbide tooling may not be suitable at high feed rates if vibration is an issue.
Regarding tool paths I'n keen to see how m_c gets on with generating trocoidal paths with cambam. If the software can do that for under £100 it sounds like a great deal. I use trocoidal all the time and cringe when I have to put a tool into a corner when the rads limit my options.
Rgds,
Noel.

Hi Noel,

At that point I needed the parts off of the machine without mishap, as they had to go on the race car as one of the first bits of assembly, as they sit between the monocoque and the front sub-frame (replacing bonded ali and silly putty....I mean rubber OEM parts ;-) ). I also had limited amounts of 40mm 6082, so I needed safety and the machine was not long up and running at that stage. Conventional was quieter and I figured less stressful than climb, but I do use both these days and I hear you on the wear at the tip, but I have managed to tune my F&S's, using GWizard's help, to the point where (touching wood) I'm getting much better tool usage than I used to.

**Bush Flyer** · 22-04-2014

Hi Washout,
I liked your videos, Thumbs Up. The 5th video is perfect, That's how I want to be cutting aluminium. I don't think I will use your method for testing how sharp the end mill is, It's a bit messy. Can you tell me the plunge rate you have on the 5th video, and I take it as your using the full rate as you ramp down? and you only use the 30% if you were plunging a hole with an end mill instead of a drill bit.

**Washout** · 24-04-2014

Originally Posted by Bush Flyer

Hi Washout,
I liked your videos, Thumbs Up. The 5th video is perfect, That's how I want to be cutting aluminium. I don't think I will use your method for testing how sharp the end mill is, It's a bit messy. Can you tell me the plunge rate you have on the 5th video, and I take it as your using the full rate as you ramp down? and you only use the 30% if you were plunging a hole with an end mill instead of a drill bit.

Correct chap - using full plunge when ramping and only 30% when actually plunging straight down, which I try not to do unless the CAM software forces me to do it.

**GEOFFREY** · 25-04-2014

Probably slightly off topic, but related to material removal. About 3 years ago I visited a factory that had a number of CNC mills, one of which was making some ally boxes for race car electronic enclosures and they were specified as machined from solid billet. The way that the material was removed for "pocketing" was that the machine was programmed to plunge drill a series of holes about 50mm deep with something like a 20/25mm drill, each hole slightly overlapping the next such that it left a series of islands standing and serrations round the edge. The finish milling then simply meant removing the islands and cleaning up the edges. Of course this was a commercial machine, through tool cooling etc., but the factory owner told me that it was by far the quickest and cheapest way to remove material. I realize that this method is probably well known, but I thought it was interesting. G.

**Bush Flyer** · 25-04-2014

I have just ordered a heap of aluminium and Five 1/8 single flute bits for cutting aluminium. When They arrive I will start at one setting and keep a note of exactly what the feed and speed is and go from there. The plan is I will take a slice right through the aluminium from one side to the other ie. mill a slot 1/8th wide.
The aluminium is 6082 T651 the end mill is 1/8th (3.175mm) carbide it is 38mm long 20mm will over hang the collet the cutting edge is 12mm long, the feed it will be 325mm per minute, plunge is 254mm per minute, the spindle rpm 12000, and the depth of cut will be 1mm.
Any advice about changing some of the settings will be welcome.

**cropwell** · 01-05-2014

Worth a look
Sorotec - Werkzeuge click the flag to translate it to English,
.
but with shipping costs you have to buy about £50 quids worth to make it worthwhile.

**Bush Flyer** · 03-05-2014

Well that didn't work out well, cutting 6082 aluminium. The settings were. 12000rpm. Feed rate of 325mm per minute. Plunge rate of 254mm per minute, with a depth of cut 1mm. I used a 3.175mm single flute carbide bit, but as soon as the bit cut in to the side of the aluminium the bit broke, so I tried a cut depth 0.5 mm. The bit did cut through the aluminium of 60mm wide but by the time it was at the end there was a poor shaving curl and when I got down to 5.5mm deep it broke that end mill as well. I did use cutting oil and it was a wash with it, also there was no smoke coming from the bit so it was not getting hot. So what do I do now should I reduce the depth of cut a little more or speed up feed rate. Or is it that I am using to small a size end mill?