[dkirby]

Well Brian that's the thing that has me confused, there was just barely enough shank hanging out to reach the bottom of the pipe.
It is a 4 flutter and i purposely kept the feed down. I am using er collets and everything was tight.
I will recheck my math. but I thought that my rpm was in the ballpark. This is pretty mild steel and it was a solid carbide endmill.

[dkirby]

I just checked and here is what I came up with rpm = cutting speed x4 / dia.

cutting speed for low carbon steel 300-400 I used 350x4=1400/.5 = 2800 rpm the feed rate calls for about 8 so i was low there but still doesn't explain why the endmill broke??

[Brian L]

Well, I calculate it like this, 200sfpm with carbide on mild steel, which is probably a little slow, but not out of the ball park. So, your circumference is 1.57 (pi x dia.) and at 200sfpm x 12 = 2400, divide that by 1.57 is 1528 rpm. a 1/2" end mill should be good for .002" per tooth, so a 4 flute should be .008" per revolution. Times that by 1500 and you are at 12ipm. Too slow can tend to make really fine chips that can cause the end mill and the chunk you are taking off to grab and break.

There are a lot of sources for relatively cheap end mills out there.... I buy a lot of YG 3 flute Alumagator end mills from a place called Suncoast Precision on Ebay. You better get used to buying a few to have around, especially if you are going to work steel.... busted end mills is just a way of life until you get some mileage under your belt.

[Brian L]

Unless you have some super duper coating on the end mill, 350 sfpm is high for any kind of steel shy of maybe 12L14. Granted, they have made advancements with the coatings since I ran production (back in the 90's), but carbide is still pretty much carbide and we used to run 200 sfpm on mild steel, slower on 4130 and 17-4, and a whole lot slower on all the 300 series stainless steel.

You are also not at optimal conditions trying to take this whole cope out in one full depth, full diameter pass.

[moldcore]

Dave what is you depth of cut? How rigid is the setup? The combination of chatter from a poor setup, your cutting feeds and speeds, plus your depth of cut is most likely the cause of the broken end mills.

[dkirby]

Brian L , Where do I go for a source to determine proper feeds and speeds for a VMC. All I have done is manual milling, never really paid much attention to speeds and feeds, kind of just went by how things looked and the sound of the cutter and color of the chips.
Today I went back to HSS endmill and everything was OK!!

Moldcore, I am coping some tubing 1.320" dia. with 3/16 wall thickness. I have 2 vises setup on the table, positioned as close as possible to where the 3 copes take place. I understand that chatter and such will come in to play... But... there is the middle of the tube that is open, I am doing a G03 and there is no pile up of chips and I kept the feedrate low to see how it was going to cut.
You may school me on a better way please. I just thought that with the rpm that I was running ( which was on the high end.. 2800) and in conjunction with a low feedrate (with no chips of any size) I can not see why it would snap off a 1/2" carbide endmill.

I am very green at this( CNC), but I have used carbide endmills on my manual mill with out many problems.
Do you think that in this case, maybe carbide is not the way to go?
I look forward to anybody's recommendations and thoughts!!!

Dave

[dkirby]

Another development has occurred. I went to add cutter comp. to 2 of the copes, and I get 507 error. I think that I understand why, but I don't know how to correct it. Do I have to rewrite the program?
Dave

[Brian L]

Speeds and feed.... you can get the G-Wizard from CNC Cookbook, or just look up some speeds and feeds on any brand of end mill's website. Once you have done it for a while, you'll have a feel for what the machine and tools can handle.

Cutter comp? How and why? Was your cope too tight? Without knowing what you did in the code, I have no basis for further info... did you try to use G41/42 and add a D callout in the program?

[dkirby]

Actually, this is basically the same program that you have helped me with before. 1.320 pipe 1.5" dia. cope using .500" cutter and what I was trying to do, was learn what cutter comp. actually did. I ran my same program but in 2 copes I added a G42 .

Here is the part of the program where a G42 was added. I read that cutter comp. had to be added and removed on a line move.

n75 go1 y-.750 f8 g42
n80 go3 x-14.1562 i-.5 f2
n85 go1 y-1 g40
n90 g00 z4.5

Was I suppose to add a D callout?. I just thought that it was getting the readings on the tool offsets, or do I have to tell it what the settings are?

Dave

[Brian L]

OK, you do need to add a D value, D1 if it's tool number 1, D2, if it's t2 and so on. You are programing to the centerline of the cutter, so cutter compensation will work like a tool wear offset. It's been a while, but I think you'd put say -.005 in the D1 offset and that would move the cutter path out .005" bigger. You do generally need a straight-line move to activate it, if you are doing wear type offsets, where they are generally small, then small moves before the arc are ok.

If you were programing the actual edge path of the part, then your D value would be the diameter of the end mill, so .500, and you need the straight-line moves to be at least 1/2 the diameter and better if you keep them 1 full diameter away, so the tool has room to compensate for it's diameter. With the advent of CAM software, folks rarely program to cutter edge any more, almost always to centerline and use compensation as a tool wear type of thing, if they even use that. Most times they just go into the CAM software and change the size value of the end mill.

You could also have just changed your code, swing a .505 R and change the start and stop positions accordingly

[dkirby]

Hi Brian, Here is my understanding of cutter comp. from reading the manual. I thought that if I wanted to change the dim. of the part all you had to do,was go to the tool offsets and put in a smaller dia. and then activate cutter comp.
So I put a piece of pipe in the vices and ran the regular program. I then put in 2 G42's for the side copes, and ran the program again to see what kind of moves I was going to get. It ran a couple of lines, but when it got to the G03 line I got a Error 507 which said " Line to arc lacks intersection"
Maybe you could explain the proper procedure to me.

Dave

[Brian L]

As I explained in my last post, you have to have a D value when you call up G41 or G42. Here is an example from my programing manual. You also have to go to your F7 (Parameters), then F4 (D Off), then you can edit whichever D number associated with the tool you are using.

You said you added G42, if you are climb cutting like I programmed below, you should be G41, cutter to the left, so that might be your issue.

[dkirby]

Thanks Brian.
Dave