Pm727m and face milling

[devils4ever]

Speeds are dependent on the material. Each material class will have a recommended cutting speed that is used to calculate RPM and the same calculation can be used to find a starting speed, whether you're turning or using a milling cutter like your fly cutter. There are tables for cutting speeds, given in SFM (surface feet per minute) all over the net and in reference texts. LMS has a popular one.

Find the material you are working with and look up the cutting speed for the tool you're using. For 1018 being cut with a carbide tool, CS is about 800 sfm. Now plug that CS into the formula: RPM = CS X 3.82 / Diameter, where CS is your cutting speed from the table, 3.82 is a constant and Diameter is the diameter of the cutter on the mill or the work piece on the lathe. In your case, the minimum diameter of your Superfly is 1.5" or so. Plugging in the values, RPM = 800 X 3.82 / 1.5 = 2,037 rpm. This same cut in aluminum would max out the speed of your mill.

Thanks, mikey. The LMS table is a little confusing since it shows 800-885 FPM for lathe work for 1018 and 65-110 FPM for milling 1018. Unless I'm reading the tables wrong. Why would it be different?

Looking in my 25th edition Machinery's Handbook at "Table 11. Recommended Cutting Feeds and Speeds for Milling Plain Carbon and Alloy Steels", for 1018 steel, I see 800-1050 FPM (Opt.) for coated carbide end milling. That matches your value. Feed is 0.007"/tooth (Opt.).

So, for calculating the feed rate: fm = ft X number teeth X RPM = 0.007"/tooth X 1 tooth X 2,037 RPM = 14.3 IPM. That seems a little high.

 

[mikey]

Yeah, you're right. I looked at the numbers for turning, not milling, so sorry for the confusion but you get the idea of how the table and formula is used, right?

I should tell you that at this stage of the game, you should do the calculations and set the feeds and speeds but you have to keep in mind that the cutting speeds in the chart are for a depth of cut of 0.040" deep. If you cut less than that then your speed and feed can increase a little; if you cut deeper then you should slow down. There are no hard and fast numbers here. Start with the calculations but learn to respond to the cut.

The other thing you will find with inserted carbide fly cutters is that the insert needs adequate feed to cut well. Quite often, the response to a swirled finish is to slow down the feed but what usually happens is that you produce fine overlapping lines in the finish instead. This is because the insert is not being fed fast enough. Look at the width of the insert tip and you'll see that it is quite broad. In order to produce a clean finish, the Superfly needs enough feed rate to keep that tip cutting with minimal overlap. Try varying your speed and you'll see what I mean.

Remember also that all inserts require adequate depths of cut in order to reduce deflection from radial forces. On my mill, the Superfly insert cuts well at about 0.010" deep at a minimum. If I go shallower then finishes can be affected so I have to plan for this and make sure I have enough stock to allow adequate depths of cut.

My point is that calculations are only one part of the puzzle. They are not written in stone and with practice you will learn to respond to what the tool produces. Start with numbers but understand how the tool works so you can respond to what you see it produce and change things if the results are not what you want.

 

[Brad125]

Well i went againt reccomendations and bought a Accusize 1.250 "indexable endmill". Only rhing i had laying around was a 3" piece of aluminum. I used the inserts that came with it designed for steel and it worked pretty good. Ill have to get the proper inserts for the cutter soon. There is a few swirl marks on it for what ever reason, but it pretty smooth. What do you guys think?

 

[mikey]

Brad, if your tool gets it flat and accurate and you're happy with it then that is what matters. I suspect the tool can work better, though. I suggest a bit more depth of cut, speed and also see if you can increase feed a little bit. Use some WD-40 to lube it and see what happens.

 

[Brad125]

Mikey, i did use wd40, worked well. I only took a .005 cut because that piece of aluminum is for a project of mine. Id rather been closer to .030 depth of cut. But, i agree i think a deeper cut and the proper inserts would make a difference.

 

[mikey]

Determine what the nose radius is on the inserts, then take a depth of cut at least a few thou deeper as a depth of cut and it will cut much cleaner and more accurately. It should also throw a shower of chips in a steady flow as you feed; get the feed right and the finish will clean right up. It always takes some time to get used to a new tool but congrats - you're on your way!

 

[higgite]

Well i went againt reccomendations and bought a Accusize 1.250 "indexable endmill".......

Brad,
I bought the same Accusize 1.25” indexable end mill back in early May and am very happy with it. It leaves what I would call a good finish on mild steel and a very good finish on 6061. I'm still playing around with feeds and speeds. As you know, it comes with inserts for steel, so I bought some Oscarbide bright finish inserts from Amazon (10 for $45) for use on aluminum and they work well. Mikey is right, deeper cuts will give you a better finish. And, he’s right again (I get tired of saying that. Mike, screw up once in awhile, will ya?) in that it cuts nicely to a 90 degree shoulder which my Superfly won’t do. Enjoy!

Tom

 

[Brad125]

Mikey the rose radius is .019ish , so i knew a .030 would be a good depth of cut, but this project i only had a few thousands to take off. I will get a piece of steel and try again eventually.