[Chispas]

I need help on Okuma LB 25 M
So i would like to someone help me with programing and milling
I need some program examples with drawing so i can understand it better
I m mostsly use G90 code
What i need is program exampes of turning cycle and milling cycles
I know for this cycle :
this is how i start :

G90
G95
G50 S2000
S500 T060606 M42 M04
G00 X650 Z5
G00 X160 Z2 G96 S200 M08
G85 NAP1 D5 U1 W0.1 F0.2
NAP1 G81
G01 X0 Z0
X40
Z-20
X60
Z-50
X100
G80
G00 X650 Z5 M09
M02


BUT THIS CYCLE dont work when i have radius

[Algirdas]

one more comment:
Your Okuma is right handed. You need to use right handed tools, the tip facing down. M3 is normal spindle rotation for OD cutting.
concerning radius.
You need to use G41 or G42 for start of radius compensation. G40 to cancel.

[uperez]

I need help on Okuma LB 25 M
So i would like to someone help me with programing and milling
I need some program examples with drawing so i can understand it better
I m mostsly use G90 code
What i need is program exampes of turning cycle and milling cycles
I know for this cycle :
this is how i start :

G90
G95
G50 S2000
S500 T060606 M42 M04
G00 X650 Z5
G00 X160 Z2 G96 S200 M08
G85 NAP1 D5 U1 W0.1 F0.2
NAP1 G81
G01 X0 Z0
X40
Z-20
X60
Z-50
X100
G80
G00 X650 Z5 M09
M02


BUT THIS CYCLE dont work when i have radius

I'm pretty sure this would work.

G90
G95
G50 S2000
S500 T060606 M42 M04
G18 G00 X650 Z5
G00 X160 Z2 G96 S200 M08
G85 NAP1 D5 U1 W0.1 F0.2
NAP1 G81
G01 X0 Z0
X34.4
G3 X40 Z-2.8 R2.8 (this will make 2mm edge radius if you're using 0.8mm radius insert)
G1 Z-18.8
G2 X42.4 Z-20 R1.2 (this will make 2mm corner radius)
G1 X54.4
G3 X60 Z-22 R2.8 (2mm edge radius here)
G1 Z-48.8
G2 X62.4 Z-50 R1.2 (2mm corner radius here)
G1 X100
G80
G00 X650 Z5 M09
M02

If you're not using G41/G42: edge radius = target radius + radius of tool; corner radius = target radius - radius of tool

[uperez]

one more comment:
Your Okuma is right handed. You need to use right handed tools, the tip facing down. M3 is normal spindle rotation for OD cutting.
concerning radius.
You need to use G41 or G42 for start of radius compensation. G40 to cancel.

Uhmm.. sorry to burst your bubble but I don't see right hand/ left hand tool relevant if you're using the correct spindle rotation. This only affects if you're threading which changes your thread start point and direction (ie. left hand/ right hand thread)

And you don't need G41/G42 to make an arc/radius.

Uly

[Superman]

Uhmm.. sorry to burst your bubble but I don't see right hand/ left hand tool relevant if you're using the correct spindle rotation. This only affects if you're threading which changes your thread start point and direction (ie. left hand/ right hand thread)

And you don't need G41/G42 to make an arc/radius.

Uly

1+,
-- Al, what happens if he uses a L/H tool turned upside down....= M4, and he can use the same toolpath he wrote for the R/H tool
---- normal spindle direction is dependant on how the cutting edge ( or tip ) is presented to the material.

I'd agree with Al, if in a production type environment, you'd try to have the spindle running in 1 direction to suit all tools ( drills, OD & ID tooling etc.), it would cut down cycle time not having to stop and reverse the spindle constantly, even run the spindle non-stop to cut more time out of the cycle

Chispas,
put up some of your NC code for doing radii, what you may be doing is adding the radii to the Z endpoint, as well as to the X, (-- X is a diameter, so the radii needs to be added twice)

[Algirdas]

Okuma is designed to use tools properly. "Upside down" and similar you can use, of course.
1. cooling much easier when chips are directed down instantly
2. cutting accuracy. You can cut ø2mm±5µm easy with Okuma, with proper setup.
3. Cutting without coolant. Okuma could be factory or retrofit prepared for steel deep cutting without use of any coolant. Possible with setup chips down only.

[tea hole]

Okuma is designed to use tools properly. "Upside down" and similar you can use, of course.
1. cooling much easier when chips are directed down instantly
2. cutting accuracy. You can cut ø2mm±5µm easy with Okuma, with proper setup.
3. Cutting without coolant. Okuma could be factory or retrofit prepared for steel deep cutting without use of any coolant. Possible with setup chips down only.

Though I typically agree with you on topics, here I differ.

First and foremost, with regards to direction of rotation of the spindle:
From a very mechanical standpoint, Main spindle rotation should be M04 and sub spindle should be M03. Think about the forces on the turret and ways of the machine. if on the main spindle, With the spindle rotating into the tool in the M03, the cutting forces are going to pull the turret away from the ways of the machine. This can cause accuracies to get worse, chatter and even machine reliability problems in a production environment. If you are cutting something in M03, there is no reason it cant be done in M04. This is not Okuma specific. You will flat out always get better machine life doing this and especially so in other brand machines with roller guides for ways unlike Okuma's box ways.
From the heat standpoint, I see no reason anything that can be done to cut steel right side up cant be done upside down or visa-versa. Heat and pressure cut metal so no matter what it will be there. Creating the heat and managing it's dispersal is Machining in a nut shell. Personally, from just physics, i would think having the insert up would be the best for accuracy and repeatability (not to mention make it easier for the operator to change, shortening insert change time). The heat is in the insert and heat rises so diffusion to the steel tool will take longer, meaning adjustments and possible bad parts are minimized.
Last is chip control, my biggest issue with rotating the chuck in M03 is that as chips and coolant come off the part, they hit the chuck or jaws which immediately splash onto the window. This also holds true for catastrophic failures. If the chuck is rotating the other way, the part that flew off will tend to carry either strait up, down or to the back of the machine. In M03, it's strait at the door every time i've seen... The chips themselves should be handled in the cutting parameters. Direction of rotation shouldn't be your go to for breaking a chip. If it's not breaking, you have something fundamentally wrong, not spindle rotation.

as far as Superman's comment about all tools rotating the same direction in a production environment, I agree and disagree. I would try, but i would sacrifice that in the interest of machine reliability. If i save 9 seconds per part over 5 years but have to buy a new machine because it won't hold size any more, what have I gained? However, if I can sacrifice those seconds to change rotation direction and keep the machine for 7 years holding size, then that sure makes the deal easier to swallow.

With regards to why your G85 cycle won't cut a radius, i'm unsure what you mean?
What is it that causes you to think that?
I almost always us a combination of:
G85/G81/G82/G87
G86/G81/G82/G87
for my cycles. Some include no radii, some are nothing but radii. What might help you understand is to better understand the relationship and function of the above G codes. Of course, without knowing why specifically you say you can't do a Radii in G85, I'll never know.
Below is an example of code I wrote that includes the G codes above, G41/42 and cutting radii.
Maybe that'll help.

NFACE
(ROUGH FACE AND OD)
G50 S3000
G97 S1000 M4
G0 X1000Z1000
TG=1OG=1
Z1
X6
M8
G96 S1600
Z.0625
VLMON[2]=1
G85NLAP2 D.05U0W.035F.015
NLAP2 G82
G1G41Z0F.01
X4.9
G40
G80
G87NLAP2
VLMON[2]=0
G97S1000
G0Z1
IF[VORD[00017] NE 1] NNOOS
X1000Z1000
M01
NTURN
G50 S3000
G97 S1000 M4
G0 X1000Z1000
NNOOS
TG=1OG=1
G0Z1
X6
G96S1600
Z.1
VLMON[3]=2
G85NLAP3 D.187U.1W.04F.024
NLAP3 G81
G1G42X5.632F.012
Z.05
X5.732Z0F.01
X5.7982Z-.012
G3X5.864Z-.059L.05
G1X5.864Z-.375F.014
X5.975Z-.5
X6.05
G40
G80
VLMON[3]=0
G0 X1000Z1000
M01

NFIN1
G50 S3000
G97 S1000 M4
G0 X1000Z1000
TG=1OG=1
G0Z1
X6
G96 S1900
Z.1
VLMON[4]=2
G87NLAP3
VLMON[4]=0
G0 X1000Z1000
M01

Hope that helps!

Good luck.

[fordav11]

that example will only confuse him more. you should probably post a more simple example. he's got an LB25 so more than likely has OSP5000 or OSP7000 and none of the fancy options like Tool Groups, Tool Load Monitoring and I'm sure he has no idea what IF[VORD etc does ;-)

something like this....

G50 S3000
G0 T0101
G96 S400 M4
G0 Z.1 M8
X6
G85 NLAP3 D.187 U.1 W.04 F.024
NLAP3 G81
G1 G42 X5.632 F.012
Z.05
X5.732 Z0 F.01
X5.7982 Z-.012
G3 X5.864 Z-.059 L.05
G1 X5.864 Z-.375 F.014
X5.975 Z-.5
X6.05
G40
G80
G87 NLAP3
G0 X1000 Z1000 M9
M01

[tea hole]

I agree it could be simplified to be used on an LB25.
But. I don't have anything that old.
Therefore, if I can't with certainty delete everything his machine doesn't have then there's no reason to delete anything.
In my opinion.

[fordav11]

my example above based on your example will work on an LB25.