Need help programming, is it possible, conversational, vcn530c

Hey guys,

I'm decent with conversational on lathes. I've programmed by hand my entire career both g code and conversational. We recently acquired a mill, vcn530c, and I'm learning the programming quickly. But the part I'm making has a feature that I'm not sure I can program using conversational. At least I've tried and cant seem to figure it out yet.


I need to make a .75 dia. pocket, .058 deep, with a 1.25 radius in Z, and I want to do it with a ball em.


Ideas?

Tap_or_Die said:

Hey guys,

I'm decent with conversational on lathes. I've programmed by hand my entire career both g code and conversational. We recently acquired a mill, vcn530c, and I'm learning the programming quickly. But the part I'm making has a feature that I'm not sure I can program using conversational. At least I've tried and cant seem to figure it out yet.


I need to make a .75 dia. pocket, .058 deep, with a 1.25 radius in Z, and I want to do it with a ball em.


Ideas?

Click to expand...

.
you can get end mill with rounded corner, its not a full ball. i have gotten for example
1" dia EM with .125 corner radius. can get different corner radius.
.
also its not always ordered as new. some get EM resharpened with corner radius. depends
if the resharpen people can do it. special order new End mills might take a few weeks to
get delivered
.
also some carbide insert mills can get inserts with corner radius

No way to do the spherical radius bottom in conversational. You need a manual unit with lots of typing or an eia 3d surfacing program.

You could switch coordinate planes with g18 g19 and program it as an arc movement in x/y plane. Set your cutter comp to the the ball diameter and it should have no problem doing an arc in the Z. JUST MAKE SURE TO SWITCH BACK TO G17 WHEN YOU ARE DONE WITH THAT MOVEMENT!!!!! I've destroyed a part because of this when the machine tried doing a tapping cycle into the vise... in +Y

Oh crap, you mean .75 dia round pocket with 1.25 radius...

GOT IT!
Do what I said above to make the profile of the bottom. Use G68 to rotate the coordinate system by a degree value and run the same path. Loop this statement until you have gone all the way around. You will want to work incrementally from the center of the the imaginary sphere for the 1.25 radius. You'll have to use g19 y/z coordinate plane to use cutter compensation. And you will need to look in your machines manual for how it requires the parameters to be programmed for the for g68. Before you rotate your coordinate system you will have to go back to the center of imaginary sphere. You'll make a straight movement to the circumference of the half circle path that you will use for your 1.25 radius arc. This will also be used as the 90 degree instate movement for cutter comp. Once it has done the full half circle movement in y/z (will now be on the other side over your pocket) go back to the center and it will be safe to rotate your plane again. Ideally you should only have to go through 180 degrees of rotation since your cutting all the way through. The degree increment you shift each time will determine how smooth the finish is. Once you have the program working I would try like 5 degrees and see how good the finish is. There is going to be alot of air cutting and re cutting, but this is the best thing I can think of off the top of my head without alot of trial/error/proofing.

LEARNING CNC STRATERGIES AND TIPS: G17-G18-G19 Plane selection
^here is a decent resource for g18/g19 planes

G68 & G69 G Codes: CNC Coordinate Rotation [ Easy Tutorial & Guide ]
^here is a decent resource for g68 roation

If your decent with conversation coding looping the code should not be too big of an issue.
This is going to be a fun little project! I'll have to give it a try myself when I have some time to kill. Good luck!

There is probably a better solution for this using boolean/conditional coding to change micros variables for the circle radius and depth each time it loops to get the same result, but by the time you've finished all that coding it probably will take longer than the option I mentioned above.

i have used a mazak with 3D machining capability and you can program a large 1.25 radius and tell it too
use a smaller ball end mill. its programmed conversationally. in like 25 years I am not aware of even once where it was used. they just wanted the ability
.
my limited experience (basically practicing using it) you tell it how smooth or how far apart the mill passes are. it takes considerable time if you want radius really smooth. obviously if you have it do 100 or 1000 mill passes it takes time
.
its a lot faster to have end of end mill sharpened with radius you want

I was just playing with it and wanted to see if it was possible. It would make a much smoother surface. Right now I just plunge with a ball mill and it works fine.