Deep Slot Milling in Aluminium - Optimum Cutter Diameter
New poster but long time lurker.
I have he need to cut a number of long, deep (up to 25mm) slots in 6082.
Current strategy is to peck drill a number of 6.5mm holes to depth and the run the slot with a 2 flute carbide end mill at 80% F and S (12000rpm, 1200 mm/min).
This does work but it generates a lot of swarf and the chips fall into the holes.
The question is, would it be better to use a smaller cutter. 5 or even 4mm? Is slot depth a factor?
The machine is a steel frame gantry with flood cooling, 2.2kw spindle.
Re: Deep Slot Milling in Aluminium - Optimum Cutter Diameter
In my experience, chip welding (recutting) is the risk with deep slots in loominum. Pretty much all of the cutters I've broken over the last 2 years have been due to this. The best solution in my situation seems to be to ensure a constant supply of flood coolant, which both cools the chips down and clears the from the danger zone. I don't know if that would work for you, depends how much coolant you get get in there. Must admit, I do get a bit carried away with the feeds and speeds which probably doesn't help.
Using a smaller cutter and an adaptive path might at least reduce the chip size a bit and leave more room for chips and coolant to evacuate. If you are doing a 25mm deep slot with a 4-5mm cutter, you will be doing it in several (4-5?) stepdowns.
Dunno what others think?
Re: Deep Slot Milling in Aluminium - Optimum Cutter Diameter
Quote:
Originally Posted by
Muzzer
In my experience, chip welding (recutting) is the risk with deep slots in loominum. Pretty much all of the cutters I've broken over the last 2 years have been due to this. The best solution in my situation seems to be to ensure a constant supply of flood coolant, which both cools the chips down and clears the from the danger zone. I don't know if that would work for you, depends how much coolant you get get in there. Must admit, I do get a bit carried away with the feeds and speeds which probably doesn't help.
Using a smaller cutter and an adaptive path might at least reduce the chip size a bit and leave more room for chips and coolant to evacuate. If you are doing a 25mm deep slot with a 4-5mm cutter, you will be doing it in several (4-5?) stepdowns.
Dunno what others think?
To be honest, I haven't had any chip welding while using flood coolant. Even if the cutter is running through a pile of chips it sounds grainy and generally to be avoided but it hasn't actually damaged the bit so far. The flood coolant is not as good at removing the chips in a deep slot though, when compared to an air pressure feed. Unless the coolant is pumped into the slot at high pressure, which makes a massive mess of the enclosure, the chips kind of sink in a pool at the bottom of the pocket / slot.
As for the step downs, I'm pretty new to this and am being very conservative on cutting depth. I won't go more than 1mm cut depth for a slot. As I'm not cutting for cash, I don't mind high cycle times and although my machine is capable of cutting deep pockets in Al, I don't want to risk any more carbide cutters.
Re: Deep Slot Milling in Aluminium - Optimum Cutter Diameter
I've done a fair bit of this in the last year and the solution I've come up with (which may not be the right or only one!) is:
1) Cut to >95% of slot width with a roughing cutter - these generate lumpier chips which seem to clear the slot better - then if you need a clean slot do a thin finishing pass with a "smooth" cutter.
2) Use a cutter that is <66%of the final slot width to aid chip clearance.
3) I use (generous) mist coolant with a fearsome air blast - if your slots are annular or change direction multiple nozzle will help.
4) Play with feed rate to see how hard you can push it - with practice you can judge quite a lot from the noise IMHO.
Re: Deep Slot Milling in Aluminium - Optimum Cutter Diameter
Quote:
Originally Posted by
guy_
I won't go more than 1mm cut depth for a slot. As I'm not cutting for cash, I don't mind high cycle times and although my machine is capable of cutting deep pockets in Al, I don't want to risk any more carbide cutters.
There's part of your problem straight away, Carbide likes to be pushed hard and 1mm Doc isn't enough with a 6mm tool. Could easily double this and more without breaking the tool.
Next is the intermittent cut caused by the holes you drilled, Carbide doesn't like shocks and intermittent cutting, I would stop doing this.
I find Mist cooling with plenty of air is better than flood for slots.
Re: Deep Slot Milling in Aluminium - Optimum Cutter Diameter
What width are the slots?
Chip clearance is key, be that flood or air/mist.
I'd be looking at trochoidal toolpaths and making more use of the length of the cutter.
Drilling is the most efficient method of material removal, but if you're recutting air in the drilled holes, there's no point in drilling holes.
Re: Deep Slot Milling in Aluminium - Optimum Cutter Diameter
To be honest, I'm not sure what you mean when you say that carbide likes to be pushed hard. I know that it can be pushed hard and my DOC could be bigger but I'm just getting to grips with what my machine is comfortable with. The intermittent cutting is really the same as any stepover. I know carbide is brittle but I haven't seen any damage to my bits from doing this.
Re: Deep Slot Milling in Aluminium - Optimum Cutter Diameter
Quote:
Originally Posted by
m_c
What width are the slots?
Chip clearance is key, be that flood or air/mist.
I'd be looking at trochoidal toolpaths and making more use of the length of the cutter.
Drilling is the most efficient method of material removal, but if you're recutting air in the drilled holes, there's no point in drilling holes.
Most of the slots are between 6.5 and 8mm wide. The thinking behind drilling the holes is that I get about half of the material cleared before the main slot cut op. It definitely helps, I saw a vid by NYCNC on youtube. Like I say, cycle time isn't really a big issue for me as I'm not making that many parts. I'm really looking for opinions as to how thin a profile cut can be when its made by an end mill. For example, if you were going to cut a 2d profile out of say 15mm thick Al, what's the best cutter to use? I quite often but a square of stock material and have to cut the shape out of it before I even start. Buying laser cut profiles is expensive and normally on a long lead.
Re: Deep Slot Milling in Aluminium - Optimum Cutter Diameter
Quote:
Originally Posted by
m_c
What width are the slots?
Chip clearance is key, be that flood or air/mist.
I'd be looking at trochoidal toolpaths and making more use of the length of the cutter.
Drilling is the most efficient method of material removal, but if you're recutting air in the drilled holes, there's no point in drilling holes.
Trochoidal is a good shout, same sort of logic as my cutting the slot at 1.5x cutter width to help with chip clearance.
