Aluminum Smooth Finish?

[keknapp]

I have a general question regarding milling aluminum. I'm currently using a 2-flute HSS 3/8" ball endmill to mill out a half-circle. I'm not having any problems doing this. My speed and feed rates appear to be just fine. After tweaking the speed, feed and plunge some chatter that I was getting appears to have gone away.

 

When I'm done milling the piece, I notice that the "finish" of the milled out aluminum is not as smooth as I expected. I was expecting the finished surface to be much smoother. Should I be using a 4-flute HSS 3/8" ball endmill for the smooth finish that I'm interested in?

 

I'm still a newbie in this world, so be gentle.

 

Thanks in advance.

[Sandybar]

3 flute better for aluminim

[Guest]

3 flute is better for aluminum

 

A hi-helix 2 flute is probably my next choice and a 4 flute would be my last choice.

 

 

HTH

[BernieT]

Are you 'Climb' cutting?

[crazy^millman]

what are your speeds and feeds and what is the machine you are running it on. If you got a machine that can only handle 40 ipm for 3d work and trying to do it at 200 then surface finish will suck. Is the tool running out little as .0004 can give you bad surface finished as well. Alot to check to give the best answer.

 

HTH

[DavidB]

Uncoated 3 flute unimill ballnose.If possible try not to use the centre of cutter either tip the job or rotate tool axis.There is no cutting speed at the centre of a Ball nose cutter.

[Jerosu]

If you are using the ball to machine a full radius slot (plunge the tool half the diameter deep and mill a line) you're finish will probably be bad, or just not quite as good as the other side, on one side of the radius (the conventional cut side). If you can just move over a couple of tenths and retrace the path - climb cutting the side that wasn't as good the first time around.

 

And like they said above, use a tool with as much chip clearance as you can.

[DC Gorn]

Just to add to the good information here. If you are finishing a pocket with a ball endmill your step over amount could be causing the problem. Think of that like a turning insert. Smaller step over = better finish. Also If the finish area you are worried about is a flat bottom of a pocket that means your finishing with the center point of the ball. I don't know the application but you could improve the finish by tilting the part and finishing with the true ball part of the end mill.(may require 4th axis).

[chris m]

Aluminum likes to go fast; carbide endmills at high surface speeds will typically yield a more lustrous finish. Different alloys also look different after machining, 6061 and 7075 look different that 2024 or the casting alloys which are often duller

 

C

[ToolMan184]

We use Garr 3 Flute TiCN coated for alum. and have no mercy on speeds and feeds. It likes it hard and fast........hehe We leave .010-.020 for a finish pass with a smaller step over as mentioned earlier.

[Tom Szelag]

Sharp tool? Sufficiently cooled?

[billystein]

Hi guys

I wonder why no one has asked about the length of the tool in question.

[jeff]

quote:

---

I wonder why no one has asked about the length of the tool in question.

---

Ummm nope I'm not touching that one.

[chris m]

quote:

---

not touching that one

---

[5 AX]

Be sure to tighten up the tolerance in the operation. It might not be tool related.

[HevyMetl]

Filter will also kill you for smooth surface finishes. When I was using it to cut electrodes I would constantly wonder why I had what appearead to be gouges on smooth domed surfaces. I tried recreating the surfaces in MC thinking it was a translation issue. I had to use filter due to machine issues. When we recieved the new machine it was suggested to remove all filters and take the tolerance down to 0.00004. All of a sudden the part was beautiful. I thought hey new machine sloved all problems. For a test I refiltered the tool path back to my original settings, .0002 and .0005 and the gouges were back. My reseller attributed it to mastercam interepeting arcs of slightly different radii as it was moving down the dome shape, ie imperfect surfaces.

 

Just for a test I slowed the feedrate way down and reran the program on the fadal unfiltered with a .0001 tolerance and the part a appeared much better, not perfect, but better.

[keknapp]

Thanks for all the suggestions. I'll try each and see how it turns out.

 

Keith

[stevieboy]

KeKnap

If your surface finish looks segmented, you may want to change your Positioning mode to Contouring (G61) in your program.

If that works, that means (G60) is causing segments in your surface finish.

Check post.

 

stevieboy