What's new
What's new
By:
Advanced search…

G40,g41,g42 rads on mori seiki

E

ellis115

Plastic
Joined
Oct 17, 2017
Hi all
Im having problems trying to add tool nose comp for first time on a mori cl20 lathe.
Im trying to do internal rads with a small boring bar, tip facing away from me and down towards floor as I look at it.

G0Z1.0
G1G41X20.15F.08
G1Z0.0
G02X18.55Z-.8R.8
G1Z-5.5
G03X16.95Z-6.3R.8
G1X16.7
G02X14.3Z-7.5R1.2
G1Z-13.5
X13.0
G0G40Z3.0
G00G28U0.0W0.0
M09

This is the code I have as I understand it should be with a .4 rad and tool option 2 in offset page.
The program is stopping at the G1Z-13.5 line with error code 041 INTERFERENCE IN NRC and the m/c looks to be starting to radius at the G1G41X20.15 line before it even gets to the first G02.
Any help please?
 
When you move to X13, the radial distance is 0.65. Since it is less than the tool dia, it would cause interference.
Change X13 to X12.7 or less.
The rule is, width of a channel should be enough to accommodate the dia of the tool. If not, it would cause an opposite motion with respect to defined toolpath, at the bottom of the channel, which is identified by the control.
 
I think you need to look at your' math, maybe. You are telling the machine to start at X20.15 and end at X18.55. Assuming that the start position is correct, you should be ending at 19.35 (20.15-.8). The machine would surely recognize that and kick an error code. I might also suggest to keep one operation on a line at a time. It does help to keep it clear, at least for me, and doesn't slow the machine. I operate an SL-2 almost every day and I just add, or subtract, tool nose radius into the R values. I don't generally mess around with compensation, I know the mill guys will balk at that, but lathes are different. One last thing, the G00 in front of your G28 isn't needed, just G28U0W0 will send the tool post home. Best of luck. Darin
 
He is defining a profile with radius 0.8. Therefore, to have a quarter circle, the change in X would be 1.6.
20.15 - 1.60 = 18.55 which he has correctly used.
 
Yes thanks sinha. That has stopped the machine error. I presumed since I was coming off a bore dia into fresh air that it didn't matter. (never presume haha) however something is still amiss. running through in single block the tool is doing the first G02 rad then coming to the position X18.55 Z-5.5
When the G03 line is read the absolute position of the machine changes to X16.95 Z-6.3 without the tool actually moving and no "distance to go" movement. then reads the X16.7 as normal with a .25 distance to go.
any ideas?
 
thanks darin
But doesn't the Rad work radial with double x movement to z movement so X20.15 - 1.6 = X18.55?
or is it not that simple?
the tool path on my editor looks fine.
 
Don't use radius comp on a lathe. It's shit. Program from centerline and you'll never have these problems.
 
ellis115 said:
Yes thanks sinha. That has stopped the machine error. I presumed since I was coming off a bore dia into fresh air that it didn't matter. (never presume haha) however something is still amiss. running through in single block the tool is doing the first G02 rad then coming to the position X18.55 Z-5.5
When the G03 line is read the absolute position of the machine changes to X16.95 Z-6.3 without the tool actually moving and no "distance to go" movement. then reads the X16.7 as normal with a .25 distance to go.
any ideas?
Click to expand...

You have 0.8 entered as tool radius in the offset table?
 
ellis115 said:
tip rad is .4 entered in offset
Click to expand...

Hello ellis115,
That being the case and if you have a Tool Type 2 registered, there is no logical answer. The coordinates in your sample program in the area of interest are correct and shouldn't cause a problem with a 0.4 TNR registered.

Following is a Part Program snippet incorporating a 0.4 TNR for your part profile. A 0.4 TNR successfully completes the profile.

G00 X20.950 Z1.000
G01 Z0.000 F0.10
G02 X18.550 Z-1.200 I0.000 K-1.200
G01 Z-5.900
G03 X17.750 Z-6.300 I-0.400 K0.000
G01 X17.500
G02 X14.300 Z-7.900 I0.000 K-1.600
G01 Z-13.500
G01 X13.000

Regards,

Bill
 
I have a question, and it might be due to my lack of experience with compensation. What kind of tool has a .4 TNR, at least on a machine that size?
 
Beam Junkie said:
I have a question, and it might be due to my lack of experience with compensation. What kind of tool has a .4 TNR, at least on a machine that size?
Click to expand...

All inserts have some nose radius.
For example, in ISO system, CNMG 120408 is an 80-deg diamond insert with 0.8 mm nose radius (last two digits divided by 10).
 
You must log in or register to reply here.








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top