My first part - and a dimple

[ctwo]

I wrote the g-code to create short line segments that define a circle. I used a 1/8" two flute HSS EM at ~2500 RPM and I think it was 6 ipm. 1" aluminum bar stock.

The cutter comes down for a radial depth of 0.063" and plunge depth of 0.020" per CCW cycle around the circumference to total depths of 0.100 and 0.200. I did not cut the outer OD at the bottom.

As near as I can measure, the circles are round and concentric (the center hole is just a plunge cut). Every time Z came down into the "valley" I could hear the cutter vibrate a bit, and you can see the dimple it left. There is also a score in the center groove ID in this one spot (I think this is caused because I plunged to depth and then started, probably picking up chips in the groove).

Any idea what's causing the dimples?

The finish is not very good. I think the EM is just very lightly used.

[GlennW]

You might try slowing the feed rate to about 3 or 4 ipm and use coolant to improve the finish.

[hobgobbln]

Glenn's right. 6 IPM at 0.020 with an 1/8" endmill sounds pretty fast to me. If you look at the bottom of the valleys you can see chatter marks that curve like the tool was bending.

What IPM did you plunge with? I'd put my money on tool deflection for the dimples if you've got the machine tight and tram set. I'm a novice with cnc myself but I avoid straight plunges when I can and when I can't, I plunge at 25-50% of my cutting feed rate.

Griz

[GlennW]

I'm rpm challenged on my mills, so I prefer three flute end mills for aluminum.

A bit more rigid, better finish, less chatter or noise, and increased feed over two flute.

[DavidF]

work feed 4ipm, plunge speed 2ipm for a 1/8" @2500 rpms. How much tool is sticking out? make it just long enough to get the job done. Could also lead in out of part on the outer portion....
is this an actual part or just a test trinket? Care to share the file? I could run it thru sprut cam for you and you could look through the G code and maybe see a few new things?

[ctwo]

The code is linked as a text file just below the image. I ran it several times, raising the knee between runs. The EM is a 3/8" shank double sided and the fluted part is about an inch long.

This is just a test part, but a basis for a lovejoy type slip coupling I want to make. Two ends as pictured with a mating center part of delrin.

Thanks guys. I just took a wild guess at feed.

[ctwo]

I was looking at some online calculators and other rules of thumb. I found that chip load of cutter diameter divided by 120 is a good start. I cannot mill at SFM of 400 because that would require 11k spindle.

So, for 2500 RPM and chip load of 0.125/120, I get a feed rate of 5 ipm. If I bump the RPM to 4k, then I get 8.4 ipm. So now I think I know how to calculate speed and feed:

1. use highest SFM that spindle allows given cutter diameter (SFM*12)/(D*pi)
2. figure out chip load by cutter diameter ~ D/120
3. calculate feed rate by chip load * #flutes * RPM

I thought I would get a better result with such a light DOC, but that is suggested up to 50% cutter diameter for a full slot. So I was pretty close in the feed and light on the depth. Is this right?

I also think climb milling would help a lot.

[DavidF]

Sfm x 3.82 / cutter dia = rpm.
Rpm × chipload x # of flutes = ipm.

For lite duty mills...
Alloy sfm
1018. 65 - 110
4140. 35 - 100
6061. 165
Brass. 100 - 200
This should help you get in the ball park for starters. Its pretty conservative.

[DavidF]

Chip load should be more like .001" not .125

Edit. N/M. .125/120= .00104" i get it now. Lol

[hobgobbln]

It seems like a bad combination of stickout and feeding to fast.

Try thinking of it this way:
You chuck up a piece of 1/8" round stock in the lathe that extends 1" past the jaws and spin it at 2500 rpm. You could try to take a 0.020 deep cut and feed it at 5 IPM, but it will most likely just bend and flip up onto the toolbit.

Somebody correct me if my analogy is wrong.

Griz

[RET]

Hi ctwo,

I've found several things.

First, start out slow in feed rate and ramp up if you find that the machine is OK with what you've got. Unless you are in a production situation, you don't have to have it done "yesterday." Learn your machine and find out what its "happy" with. Looking at your part, it seems that you are trying to push it way too hard. Even although a Bridgeport isn't a "light" machine, it IS light by CNC standards.

Second, I ALWAYS use climb milling if possible. The finish is better, its easier on the tool, and the tool stays sharp longer. With climb milling, the only problem is that your machine MUST be perfectly tight with no give or play anywhere, especially if you are using long cutters (1/4" dia. x 1 1/4" or 1 3/4" cutting length). If there is play or give of any kind, the tool will grab and/or break if you have enough power on the spindle.

Third, try 4 flute end mills. They work better and will give a better finish because if you are cutting on an edge (or even in a slot), one tooth is starting to cut before the preceding tooth has finished, thus the load is almost constant and you get less vibration.

Finally, I have found that end mills are quite happy to rise (on a slope), but they don't like to go down, so you have to descend at a much lower feed rate.

It looks as if the "dimple" could be caused by tool deflection or "give" in the machine because the chip load is too high. If you start off with a low "depth of cut" (although .020" isn't a lot) and use multiple passes to get what you want, it should work better. That's what I do and the end result is MUCH better than what you show. Don't be discouraged, at least the machine works, and that is a big step in the right direction. If you want a good finish in your circular slot, climb mill in one direction on the inside and then go around in the opposite direction on the outside to get a finish pass if you can.

If you plunge to depth and then start, you will leave a mark because the tool vibrates as it plunges, thus creating a slightly bigger hole. Also, once the tool starts cutting, it deflects sideways so the cut generated is very slightly displaced from the start. Its better if you can descend slowly in a spiral if you can't go to depth off the part and then come in.

Also, looking at your part, g2 and g3 will do most of what you want to do without breaking things up into itty bitty pieces.

Hope this helps.

Richard Trounce.

[RET]

Hi ctwo,

As an example, I'm still working on another one of the truck side plates that are shown in "Richard's Latest Project."

With a 1/4" dia. 4 flute end mill 1 1/4" long, climb milling and .025" depth of cut (it will take .050 but I'm concerned about cutter deflection), I'm getting almost a mirror finish on the part. No, you can't see your reflection, but its close. That's at a feed rate of 3.5" per min. Its a actually very impressive what you can get away with in aluminum. Steel wouldn't be nearly as forgiving.

I'm using 6061-T6 aluminum, pure aluminum is sticky and doesn't machine nearly as well. I also don't use coolant, I'm not set up for it and it makes a mess, but I understand it does give a good finish at faster speeds. I've never used coolant in any of my machining, even with the conventional machines I have (Bridgeport, South Bend lathe, etc.).

Richard Trounce.