Advice required please to refine milling out a part

[Saz]

I have started using my Sieg Kx1 CNC Milling machine after a break of a couple of years. I have forgotten everything!

I started on the retaining piece in the photograph, which is about 75mm long, the aluminium sheet is 5mm thick. The cutter is a 3mm, 2 flute HSS slot drill running at a spindle speed of 6,000rpm. From here on the forum and other sources I've set the following parameters. Feed rate is 80mm/min, depth of cut 1.25mm. I'm using WD40 as a cutting fluid.

Though the piece cut relatively well, the mill did vibrate more than it should and the finish on the milled sides is atrocious. You should be able to see that reasonably large chips of aluminium were produced.

My thoughts are to reduce the depth of cut and the feed rate a little, as it did seem to load the machine a little excessively. I would be grateful for any advice on this.

Regarding the poor finish, is this just down to slot milling? If so would I be better off doing an initial cutfurther out from the piece and then an inner finishing cut at 25% of the cutter diameter? Again I would be grateful for advice from someone who has a lot more experience than myself.

Also is a 3mm cutter the best size to cut out a shape like this in 5mm thick aluminium?

Appreciate any help, thanks.

Similar Threads:

• Metal lathe one off part required
• Need Help!- VF3 part circuit schematic required please
• Need Help!- Spare part required
• Help Required With Part Programme
• Advice required for my next milling machine.

[dazp1976]

I have started using my Sieg Kx1 CNC Milling machine after a break of a couple of years. I have forgotten everything!

I started on the retaining piece in the photograph, which is about 75mm long, the aluminium sheet is 5mm thick. The cutter is a 3mm, 2 flute HSS slot drill running at a spindle speed of 6,000rpm. From here on the forum and other sources I've set the following parameters. Feed rate is 80mm/min, depth of cut 1.25mm. I'm using WD40 as a cutting fluid.

Though the piece cut relatively well, the mill did vibrate more than it should and the finish on the milled sides is atrocious. You should be able to see that reasonably large chips of aluminium were produced.

My thoughts are to reduce the depth of cut and the feed rate a little, as it did seem to load the machine a little excessively. I would be grateful for any advice on this.

Regarding the poor finish, is this just down to slot milling? If so would I be better off doing an initial cutfurther out from the piece and then an inner finishing cut at 25% of the cutter diameter? Again I would be grateful for advice from someone who has a lot more experience than myself.

Also is a 3mm cutter the best size to cut out a shape like this in 5mm thick aluminium?

Appreciate any help, thanks.

Not much different than a Sieg SX2 by the looks of it except for higher rpm.
DOC is the cause of vibration as far as I'm concerned.
With a 3mm 3 flute on my converted Sieg I run:

RPM 1600.
DOC 0.6mm with ramping.
Feedrate 200mm/min.
WOC for finishing 0.2mm at 125mm/min.
You can try this first to see but in theory this should translate to about 650mm/min feedrate speed at 6000rpm using a shallower depth!!
I do have flood cooling though.

I prefer shallower depth cutting on small machines Seems the feedrate can be really pushed rather than piss about slowing down to get a good depth and busting bits.
The time difference is nothing either. Can break carbide tools this way but the cheap Chinese stuff and decent cobalt work well.
I bet the time taken won't be much different betwwen the 2 methods.

You might need to run a finishing pass at 2.5mm and then at 5mm depth to cause as little tool flex as possible.


On my new benchtop PM25 I've just tested a 6mm 3flute HSS/AL cheap end mill at 2500rpm, 1.05mm DOC, 710mm/min and it can still go more. (with flood)

[Saz]

Not much different than a Sieg SX2 by the looks of it except for higher rpm.
DOC is the cause of vibration as far as I'm concerned.
With a 3mm 3 flute on my converted Sieg I run:

RPM 1600.
DOC 0.6mm with ramping.
Feedrate 200mm/min.
WOC for finishing 0.2mm at 125mm/min.
You can try this first to see but in theory this should translate to about 650mm/min feedrate speed at 6000rpm using a shallower depth!!
I do have flood cooling though.

I prefer shallower depth cutting on small machines Seems the feedrate can be really pushed rather than piss about slowing down to get a good depth and busting bits.
The time difference is nothing either. Can break carbide tools this way but the cheap Chinese stuff and decent cobalt work well.
I bet the time taken won't be much different betwwen the 2 methods.

You might need to run a finishing pass at 2.5mm and then at 5mm depth to cause as little tool flex as possible.


On my new benchtop PM25 I've just tested a 6mm 3flute HSS/AL cheap end mill at 2500rpm, 1.05mm DOC, 710mm/min and it can still go more. (with flood)

Thanks for your reply. I'll try your cutting parameters and let you know how I get on. My depth of cut was a bit optimistic, it did produce nice big chips though!

For cutting that sort of profile out is a 3mm cutter the best size to use? The finish was terrible.

Appreciate your help. Regards, Sarah

[CitizenOfDreams]

My depth of cut was a bit optimistic, it did produce nice big chips though!

How could you possibly produce "big chips" at 6000 RPM and 80 mm/min? That would give you the chip thickness of only 0.007mm, which is way too thin I believe.

I would suggest trying much higher feed rate (around 500 mm/min) and much lower depth of cut (maybe start at 0.2 mm to be on the safe side).

[Saz]

How could you possibly produce "big chips" at 6000 RPM and 80 mm/min? That would give you the chip thickness of only 0.007mm, which is way too thin I believe.

I would suggest trying much higher feed rate (around 500 mm/min) and much lower depth of cut (maybe start at 0.2 mm to be on the safe side).

Big chips was a relative term, they are more substantial than I expected. I will try your lower depth of cut and feed rate. Thanks for your advice, I appreciate it.

[cyclestart]

A few thoughts:
Not all aluminium cuts nicely. 6061 is a good general purpose choice but the material in the picture looks like something else ?
Slots are the worst with the re-cutting of chips that happens. If it's possible to aim a good flow of compressed air into the cut it will help a bunch.
Another way to reduce the re-cutting chips is to mill away most of the surrounding material instead of having a slot-type situation.
Those tabs are creating extra chip traps, if possible use a different strategy.

My impression of the KX1 (based on nothing but a few videos) is it's a pretty capable little mill.
If the tool is longer than necessary any flex may be more of an issue of the tool rather than the machine.

[cyclestart]

Since buying a larger mill a few years back the X2 mini-mill has been mostly retired. I fired it up for a little test.
2500 RPM (that's all it can do)
30 inches/min feed
0.3125" 2-flute HSS end mill (far from new)
D.O.C 0.100"/pass, 2 passes =0.200" total depth
W.O.C 0.025"
Finish pass W.O.C 0.010", D.O.C 0.200"
Material 6061-T6

The machine did this easily but I didn't experiment any further. It's limits are somewhere beyond these parameters.
My point is these machines work best when using the side of the tool, and worst cutting full width of tool. Much worse if chips are being re-cut.
If only the protruding boss in this picture was wanted I wouldn't use tabs. Flipping the part over in the vise and milling away the excess material is easier.
Hmm... 1" thick material was a poor choice if that was the goal Anyway this my approach to small parts whenever possible, and it's not always possible.