Nakamura Tome

[hansdeberlin]

I am new to this dual turret dual spindle 5-axis lathe and my only hope is someone on this forum may have been using this lathe.

I want to cut a square but it does not turn out as a perfect square. I end up with something like a square but looks like there is some large radius on the four sides of the square

I am using live tooling .5 end mill pointing towards spindle center line or x-

 

Nakamura Tome WT 250 with Fanuc 18i-T

Upper turret X,Z,C

Lower turret X,Z,C,B axis

 

G20 G40 G80 G99

G54

M91

G28U0

G00Z7.

G40 T0606

G97S600M89

G00Z-.2C0

X2.2

G01X1.1F.01M08

G112 (polar co-ordinate interpolation mode)

G1X.892C-.446F.01

G1X-.892

G1C.446

G1X.892

G1C-.446

G1X1.1M9

G113 (polar co-ordinate interpolation cancel)

G00X5.Z7.

G28U0M41

T0600M90

M30

 

I have looked at the parameter settings but I assume they are correct since square has been cut with it at the previous owner’s place who went belly up.

What is wrong with the above code?

Thanks for looking at this problem

[IntegrexMan]

We run dual turret, twin spindle Integrex Machines here. The example below is without polar interpolation. 25mm square with 12.7mm endmill.

 

 

G0 Z2.

X-50.4 Y18.85

Z-3.75

G98 G1 Z-4. F3.

G41 X-25. F318.2

X25.

G2 X37.7 Y12.5 R6.35

G1 Y-12.5

G2 X25. Y-18.85 R6.35

G1 X-25.

G2 X-37.7 Y-12.5 R6.35

G1 Y12.5

G2 X-25. Y18.85 R6.35

G0 Z2.

 

With Polar Interpolation, X and Y actually become your C axis. The X axis moves up and down as the C axis rotates. Good for when you don't have enough Y travel. Example below:

 

G0 C0.

G0 Z2.

X62.94 Y0.

G12.1 (polar on)

X-25.2 Y18.85

G98 G41 Z-3.75 F318.2

G1 Z-4. F3.

X-12.5 F318.2

X12.5

G2 X18.85 Y12.5 R6.35

G1 Y-12.5

G2 X12.5 Y-18.85 R6.35

G1 X-12.5

G2 X-18.85 Y-12.5 R6.35

G1 Y12.5

G2 X-12.5 Y18.85 R6.35

G0 Z2.

G13.1 (polar off)

 

 

Hope this helps.

 

Craig

[Keith Graydon]

CherokeeChief This is a question for You! Drew, you too!.

 

-Keith

[Tom Dorgan from American Precision]

Well I am a Router programmer and this may not be applicable but our 18i uses G08 P1 to make accurate corner cuts. Don't know if this is true on live tool lathes. If we don't turn on the G08 our corners are rounded instead of square. Turn it off at end of tool with G08 P0.

[McRae]

Call Eliott Applications for some help with this as I think it is a problem with how you are specifying the Polar Interpolation. When I used Polar on a Mori c-ax lathe, I programmed XY and the control did the "Interpolation" to figure out where it had to position itself.

 

Elliott is where you should start.

[Philcott]

Hans,

 

 

quote:

---

I am using live tooling .5 end mill pointing towards spindle center line or x-

---

It sounds to me like you are saying your endmill is set perpendicular to the machine spindle. In other words you are cutting with the end of the endmill NOT the side. Is this correct? If so this is not the correct way to machine your square. You should be using the side of the endmill and orient the live tooling so the cutter is parallel to the part centerline.

 

We discussed this a while back and I will try to locate the thread for you.

 

Andrew,

 

I believe he may have it programmed correctly. Our Mori uses X and C when in the polar interpolation mode too.

 

Phil

[McRae]

Phil - You get the points for reading comprehension. Righty "O" on the undercutting thing.

 

The mori that I programmed used X and C where C was in Cartesion not Angular for Polar Interp. X was doubled (Diamter). My poor memory and it is getting worse.

[steve f]

I think PhilCott nailed this one down.

 

The only way a square could be produced using this method is with a ballnose or using an endmill and 4 axis rotary surfacing in the Multiax toolpaths.

[Philcott]

Andrew,

 

quote:

---

My poor memory and it is getting worse.

---

Another 2 months and you'll get some brain rebuilding Haggis for Robbie Burns. Have faith old man.

 

Phil

[hansdeberlin]

Craig!

As I described at the start of the thread NO Y AXIS on this one!!!

I wish I had known You a year ago when I was struggling with an integrex. No training on integrex or nakamura. Here are the books and DO it says the boss.

 

PhilCott!

Elliott is where you should start( I used to work for Elliott 24 years ago but my boss does not want to contact them he wants me to fiddle with this)

Cutting with the end of the end mill NOT the side. Yes SIR!

Thanks for the advice I will try as you suggested and set the tool parallel to the part center line

 

Steve!

Could you please put up a small example for a 1” square and a 1” hexagon in mastercam to the ftp site using “4 axis rotary surfacing in the Multiax” with a .5 end mill

 

Thanks to all for the Input I will experiment further on monday, John