Steel and Aluminum How to get a Better Surface Finish

[Cartierusm]

So attached are pics of steel and aluminum with the type of surface finishes I get on my CNC'd BP. For steel I'm using a 9/16" HSS Center cut endmill 4 flute at about 1000 rpm and just skim cuts to level it out and 8 ipm., for the Aluminum I'm using a 2 flute 3/4" end mill 2500 rpm and 12 ipm. I'm running the feedrate slow to get it to be milled completely flat.

So the question is how do I get better finishes on these types of material? Here is an indexable cutter would this work better? If so what angle they have 45 and 90 degree inserts? Also what feed and speeds?
http://www.wttool.com/product-exec/p...utters_Toolmex_

Thanks.

[Jason3]

Yes, you should see much better results with something like that. I'm very happy with my 3.15" 45⁰ face face mill - http://www.maritool.com/Indexable-To...110/index.html - I've had great results with the ACZ330 inserts in 1215 steel, I run it at about 1600 rpm & 40 ipm. Use the same body with polished high rake inserts on aluminium and you should be able to approach a mirror finish.

Edit - just to say, the 45⁰ face mill gives a nicer finish than my 2" 90⁰ rectangular insert face mill, but not by much. The 90⁰ one will do everything except chamfer though, whereas the 45⁰ one will chamfer and face, but is obviously no good for cutting up to a shoulder. If I had to have just one, it would be the 90⁰ one.

Best regards,

Jason

[HuFlungDung]

Carbide inserts can produce better surface finishes, because the tool will maintain its edge for a longer period. Part of getting a good finish is related to a high surface footage cutting rate. HSS just cannot go fast enough in machining steel without burning up before it gets above the critical speed where the surface finish improves.

In aluminum, you can generally use all the rpms that your spindle can muster. Aluminum is easily scuffed, and the sharp corners of a conventional endmill tend to be bad for this. I like Iscar helimills (and facemills). The special inserts for aluminum can produce a remarkably smooth surface with the end of the mill.

If your plan is just to buy a face mill for facing surfaces without shoulders, the tool you referred to is probably going to work better than what you are using now. You might want to check on the insert availability for that tool. Look for "wiper inserts" to get the best facing finish, at a healthy feedrate, providing that your machine is accurately trammed.

[John Welden]

You could use a single lip fly cutter, especially on the aluminum. If you're going for a perfect finish, they're tough to beat. Grind the bit nice and sharp with a lot of rake and put a slight radius on the nose.

Spin it as fast as you can reasonably go without shaking the machine to death. The key is to try and cut the part full width, one pass.

Sometimes a quick shot of WD40 can help get things extra shinny.

Take between .0005 and .002 for your finish pass. Adjust feed until it looks about right.

On a bridgeport I tilt the head about .0003 to .0005 over about a 6 inch radius. Facing the machine, the top of the motor should tilt towards the left. This allow the fly cutter to only cut on the front side and not scratch on the back.

If everything is right, you should have a mirror finish.

[Cartierusm]

Thanks for the help.

A couple more questions, should I use mist with the carbide insert tools? I just got a 90degree 2" face mill from Shars so I should run that 1600 RPM 40 IPM, but DOC?

I also got a 1/2" indexable endmill with a single insert, how fast should I run that RPM, IPM and DOC?

With this endmill and face mill can I make holes with it or pockets if I use ramp (which I always do anyway)? Thanks.

[HuFlungDung]

Face mills would be difficult to pocket with, as you'd need to use a shallow angle, long ramp in order to have the tool clean out the dead zone in the center of the tool.

The single insert 1/2" mill, if it is centercutting, you can actually drill with it. So it can either plunge or ramp to depth for pocketting.

Cutting speed with carbide: 350 feet/min (conservative speed) in steel, pretty well anything your spindle can muster in aluminum. You need to calculate how many rpms the spindle must run in order for the circumference of the tool to travel 350 feet in one minute, when milling steel.

For aluminum, just crank her up You might have to cut back a little if heat buildup is significant enough to cause chip welding to the tool.

Mist is fine for aluminum. Steel is better cut dry (with air blow) when cutting significant depths as thermal shock from water cooling can crack the carbide and make your new inserts seem dull rather quickly. As some will recommend, painting the surface with WD40 or other cutting oil prior to the final finish pass may improve the appearance of the surface, but it will generate a bit of smoke, too.

[Cartierusm]

I calculated on LMS with 350 fpm and 2" diameter endmill and got 668 RPMs, but that doesn't tell me DOC and ipm I should run (at least I don't know how to calculate it). Also, I don't think the endmill is center cutting. Thanks for all the info.

[Oldmanandhistoy]

Originally Posted by Cartierusm I calculated on LMS with 350 fpm and 2" diameter endmill and got 668 RPMs, but that doesn't tell me DOC and ipm I should run (at least I don't know how to calculate it). Also, I don't think the endmill is center cutting. Thanks for all the info.

http://yarchive.net/metal/empirical_feed_rates.html

John

[ImanCarrot]

Thanks for that Oldmanandhistory- brought a smile to my face, I thought I was the only one who did it like that

Particularly liked this bit

Lights, curtain.. One last check around...spindle clear, feed disengaged, SAFETY CHECK..these machines are NOT fitted with an "OUCH" switch. No "oily rags" about (apprentices rubbernecking) No laborer shoveling chips out of the back of the machine. Bootlaces tied, floor clean and dry..two or three clear escape routes..nothing to trip or fall over. Did I mention safety glasses? Safety WHAT??

Sweeet.

[mc-motorsports]

Originally Posted by John Welden Sometimes a quick shot of WD40 can help get things extra shinny.

+1
especially if the back side of the fly cutter/facemill is dragging chips or scratching, spray some WD-40 and try to keep inside of the cutting radius wet so the back side gets constant lubrication. Makes a huge difference, if you can stand there and keep it lubed... I used to do this on a conventional operation using a facemill on aluminum, worked great.