Dynamic Milling on C-axis

[Hertz]

Hey guys, Lathe with live tooling. I need to cut a hex on the end of a part, but since its in the lathe already, I'd like to use the live tool to do it. Question is I can do it easily with a face contour however I'd like to know if I can use dynamic toolpaths to do it. I don't see the option in C-Axis however I see it in mill, and even though I can select all proper geometry, it gives me an error. Not sure if I'm just doing it wrong or if it just can't be done, or if its just not recommended.

[Hertz]

Nevermind I got it. I was using dynamic area instead of core.

[crazy^millman]

Peel Mills works good and so does Dynamic Contour. Just make sure you put a amount of material for tool.

[Hertz]

Ya I was looking at it and playing around, I got some code with some crazy feeds on the C axis. Perhaps its cause I'm not fully understanding the code? I'm getting speeds of 2000. see code

 

(TOOL - 5 OFFSET - 5)

(1/2" 4 FLUTE CF ENDMILL)

G54

N5 T0505

G98

M43

M91

G0 C58.605

G0 Z3.

X2.8271

G97 S2500 M13

Z.1

G1 Z-1. F80.

X2.5883 C57.043 F999.75

X2.5521 C56.707 F1372.35

X2.5188 C56.236 F1917.59

X2.4894 C55.641 F2000.

X2.4649 C54.934

X2.4458 C54.133

X2.3852 C50.646

X2.3343 C47.019

X2.2933 C43.27

X2.2626 C39.422

X2.2424 C35.501

X2.2329 C31.537

X2.2341 C27.564

X2.246 C23.613

X2.2685 C19.717

X2.3013 C15.904

X2.3443 C12.199

X2.3914 C8.966

X2.4458 C5.867

X2.4671 C4.604

X2.4831 C3.311

X2.4939 C1.995

X2.4993 C.666

C359.334

X2.4939 C358.005

X2.4831 C356.689

X2.4671 C355.396

X2.4458 C354.133

X2.3852 C350.646

X2.3343 C347.019

X2.2933 C343.27

X2.2626 C339.422

X2.2424 C335.501

X2.2329 C331.537

X2.2341 C327.564

X2.246 C323.613

X2.2685 C319.717

X2.3014 C315.904

X2.3443 C312.199

X2.3914 C308.966

X2.4458 C305.867

X2.4671 C304.604

X2.4832 C303.311

X2.4939 C301.995

X2.4993 C300.666

C299.333

X2.4939 C298.005

X2.4832 C296.689

X2.4671 C295.396

X2.4458 C294.133

X2.3852 C290.646

X2.3343 C287.019

X2.2933 C283.27

X2.2626 C279.422

X2.2424 C275.501

X2.2329 C271.537

X2.2341 C267.564

X2.246 C263.613

X2.2685 C259.717

X2.3013 C255.904

X2.3443 C252.199

X2.3914 C248.966

X2.4458 C245.867

X2.4671 C244.604

X2.4831 C243.311

X2.4939 C241.995

X2.4993 C240.667

C239.334

 

Of course there is a lot more code, I just didn't want to paste it all but this is to rough out a hex on the end of the bar using dynamic core.

[crazy^millman]

Is that degree per minutes feed rates? Then yes that would make sense the fastest the post is allowing it to feed on that axis.

 

Or that could like your approach feed rate or does it change drastically when going to back feed on the Micro Life moves from one side of the cut to the other. Is the back move the same feed rate as the cutting? Be careful using a very high feed rate on C axis toolpath. I seen on some machines the other Axis cannot keep up and gouge the part. I like to keep my back moves the same feed rate as my feed rate moves when programming HST toolpaths this way. If it will cut it good at the programmed feed rate then is should be just as good feeding back to place. Can do the Retract between moves on the 3D HST toolpaths in the Motion > Gap size, retract, but we do not have that same ability for 2D toolpaths. I wish once we invoked axis sub that would open up to us so we can rapid the toolpaths is we want and not be stuck with always feed rates. I understand the logic to keep it feeding so the software can better predict feed moves that rapids, but in instances like this the software cannot really keep track of all the different axis combinations and controls out there. I have done the OptiCore on a flat surface so maybe you could make a flat surface of the 2D toolpath and then you would have the Motion > Gap size, retract to use here and ten set it to When exceeding a distance to get rapid moves. Then when it is going to the Micro Retract and you have set a small enough distance in your gap setting you will get retracts verse feed moves.

 

Hopefully that is some good food for thought.

[Hertz]

It is. Thanks. I have not put it to the machine yet and I know of the possible gouging as well. Seen that happen at my last job while the guy was engraving. I will definitely watch for it. Appreciate your input as always.

[gschlen]

Have you considered using polar coordinate interpolation if your machine has the option? You would have less code and a single feedrate.

[Rocketmachinist]

^^ What machine are you using?

[Hertz]

Hyundai L230LMSA

I am using a 30 day trial right now that the reseller gave us (Company is waiting to buy it for now) and I am using an older post from my old shop. The machine has polar interpolation but until we buy the software package, this post will have to do. Unless one of the other standard posts have it?

[gschlen]

The mplmaster on this site has it as well as the 4 axis posts that come with Mastercam. You turn it on by making a misc integer a one. The misc integer is typically labeled as a milling cycle. The generic posts are not hardwired to start at C0, so I use an approach reference point of Y0 and a positive X.

[Hertz]

I asked the dealer about a post. They are going to whip one up for the machine for me for the demo.

I'll let you know how it goes.

[guitar]

Peel Mills works good and so does Dynamic Contour. Just make sure you put a amount of material for tool.

 

I really loves me some peel milling