388 IPM In A2 (just starting)

[Herding Cats]

Still have a lot of tuning to do. G05P10000 Q2 is supposed to be high speed roughing and it's still cutting a little too accurate and slowing down a little more than I would like to see. I'll probably run these settings in Q1 which is normal. Q3 is finishing. Q4 will be ultra fine finishing and I haven't decided on Q5 yet.

Anyway 1/2" 5 flute 7000rpm 388 ipm in A2 normalized. Enjoy

 

[CNC_Chip_Thin]

Now that's how you make money!

 

[Herding Cats]

Now that's how you make money!

Fun coupons

 

[g-coder05]

Is that the new machine already????

 

[Herding Cats]

Is that the new machine already????

Uh huh

 

[Herding Cats]

Can't wait to play with some aluminum at 1000+ ipm.

Gonna try and make it out tomorrow to go pick up a 48" x 24" x 6" block of 2024 to play with

 

[Macds]

Awesome.
I do the same sort of thing in my shitty old fadal (not as fast).
What software you using?

 

[Herding Cats]

Awesome.
I do the same sort of thing in my shitty old fadal (not as fast).
What software you using?

It wasn't all that long ago my fastest feeding machine was 300 ipm. Actually it was 200 but I tuned it for 300. The last two I got feed up to 1575 ipm

I run SolidCAM. That was a 3d iMachining cycle. Solidcam is not solidworks cam and is a different company but it does run inside solidworks.

 

[CNC_Chip_Thin]

The last two I got feed up to 1575 ipm

What kind of cornering do you trust the machine to do at that speed? 1575 ipm in a straight line I can see. But when you're running a dynamic toolpath like you are. Does it beat the machine up in those tiny cornering moves?

I was programming a Mazak using GibbsCAM Volumill toolpath's and tried 300 ipm roughing some smallish pocket's with corner radius' around .030 once upon a time. All the panels on the machine started shaking and I could just feel the ballscrew's slamming around changing direction that fast. I ended up slowing down to keep from beating on the machine so my boss didn't have to kill me

 

[Mhajicek]

That's what high feed machining codes are for. When activated, the machine will slow down as needed in the corners to maintain the specified degree of accuracy.

 

[Delw]

would you mind showing what the finish looks like after being roughed? and also how ever is the stock thats left on it with in .005?.
never seen what the finish looks like on a part running that fast.
I assume you finish as alot slower speed?

 

[Herding Cats]

What kind of cornering do you trust the machine to do at that speed? 1575 ipm in a straight line I can see. But when you're running a dynamic toolpath like you are. Does it beat the machine up in those tiny cornering moves?

I was programming a Mazak using GibbsCAM Volumill toolpath's and tried 300 ipm roughing some smallish pocket's with corner radius' around .030 once upon a time. All the panels on the machine started shaking and I could just feel the ballscrew's slamming around changing direction

that fast. I ended up slowing down to keep from beating on the machine so my boss didn't have to kill me

That's what high feed machining codes are for. When activated, the machine will slow down as needed in the corners to maintain the specified degree of accuracy.

I can't think of a better way to quickly summarize it than that. While it's a little more complicated than that, that's pretty much what it does. There are several parameters that will help smooth out a machine but the main ones are, the accel/decell time constant, running bell shaped accell/decell curves, allowable speed difference, what angle blocks will clamp feed rate, what radius will clamp feed rate, exc.

Smooth Interp smooths off the points between blocks and allows for even faster and more accurate feeding.

I run pure linear code in this machine when running in HPCC, no arcs. Smooth Interp will not allow any arcs.

I could program a part this size at 1600 ipm but it would not get up to that speed, but you would be surprised how short of a run it needs to accell that much. It doesn't need to be a straight line, just not have any abrupt changes in direction for a couple inches.

There used to be a guy on several forums that went by the name of Psychomill that really knew his shit when it came to this kind of stuff and tuning. I seem to remember someone saying he moved his way up even higher on the food chain and no longer posts anywhere. No surprise there if you read some of his posts and see how knowledgeable he is. Wish he would drop by here but I won't hold my breath.

 

[Herding Cats]

would you mind showing what the finish looks like after being roughed? and also how ever is the stock thats left on it with in .005?.
never seen what the finish looks like on a part running that fast.
I assume you finish as alot slower speed?

Pretty standard for me to leave 0.010"-0.020" stock when roughing. I've never actually measured it manually. When tuning I just keep pushing the parameters till 0.010" stock doesn't clean up when finishing with a ball. Tough to measure true 3D parts like this any other way without a CMM.

For finishing with a ball I programmed 200 ipm but was running G05P10000Q3 which is finishing and really pumps the brakes to maintain accuracy. For most of the top of the part it ran around 120ipm getting up to 200 ipm on occasion.

I'll likely run a few more of these test parts today while tuning and I'll snap a few pics after roughing.

The ability of an old 16i with a 64 bit RISC engine and paired with the right machine (heavy die and mold type, big pretensioned screws, massive servos, exc) is still a force to be reckoned with today. This machine has 24" of X and has 5hp servos

 

[Herding Cats]

Crappy pic as I just zoomed in on the video on my phone and took a screen shot but it kinda shows the finish

 

[Plastikdreams]

Fun coupons

Coopins

 

[Herding Cats]

 

[Delw]

Thanks
thats alot better than I even expected at those speeds, pretty impressive.
sorry when I said .005 I meant was the size with in .005 of the "programmed size"
The floor on that part looks goo as no marks and I can even see your using a rad corner, endmill. I dotn see any wash out so to speak.

 

[Dualkit]

That makes me dizzy watching that. The local metal yard here doesn't sell A-2, they don't sell O-1 either. Lucky for me I make very small parts or shipping costs for those items would be ugly.

 

[Macds]

Thats an older vid with rapids turned down and not really pushing it.
I now run 4140ht, etc the same way but closer to 300+IPM

 

[CNC_Chip_Thin]

Thats an older vid with rapids turned down and not really pushing it.
I now run 4140ht, etc the same way but closer to 300+IPM

Always loved watching an endmill make it rain chips like that, even better that you can run without coolant.

Question tho... Any reason your part isn't centered in the vice?