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

Cutter comp in mill/turn machine - like a normal mill?

R

rx8pilot

Aluminum
Joined
Oct 20, 2009
Location
Los Angeles
Newbie on mill/turn machines and trying to understand how cutter comp works with live milling tools.

Specific machine: Doosan PUMA 2000SY [2007] - Fanuc 18i-TB
Axis - Z,X,Y,B,C1,C2

I have been able to self-develop a post for HSMworks/Fusion360 and did some fairly basic mill/turn parts today. Now, that I have the basic toolpaths and M-codes dialed in - the next step is to figure out how to deal with cutter compensation. Do I simply put in the comp in the R column in the offsets wear page? Not sure how/if that works with the coordinate translations needed for milling the face and profile of the parts.
A G18 is called for the profile milling in my post - so perhaps that will allow a G41 to take the value in the RADIUS comp column and it becomes the D value I would typically use in mill?

Any experts willing to chime in?

FYI: I have been programming/setting up/operating/owning 5 axis mills for 13 years. Lathes, however, are very new to me.
 
It depends on the Features you are trying to Machine. If you are doing Mill work Parallel to the Z Axis it in no way different.

I'm not sure what question you are asking, since you have 13 years programming 5 Axe Milling Machines. But you don't use G41-42 for 5 Axis Milling/surfacing, so I'm not sure how to answer your question.

I suspect your question is more about setting and activating Offsets than actual CC.? Maybe I misunderstood though.

R
 
litlerob1 said:
It depends on the Features you are trying to Machine. If you are doing Mill work Parallel to the Z Axis it in no way different.

I'm not sure what question you are asking, since you have 13 years programming 5 Axe Milling Machines. But you don't use G41-42 for 5 Axis Milling/surfacing, so I'm not sure how to answer your question.

I suspect your question is more about setting and activating Offsets than actual CC.? Maybe I misunderstood though.

R
Click to expand...

Thanks for taking a moment to respond. I only mentioned my milling experience as a point of skills reference. I would do a lot of 3, 4, and 3+2 axis setups and of course cutter comp was used to control 2D tool paths for bores, slots, etc, etc.

As I am learning lathes and mill/turn - there is no DIAMETER column in the offsets, but rather and R and T for tool nose radius compensation. In a live tool machine, is the R column used to drive the cutter comp like the D value does in a mill? I am guessing that I have to call the appropriate plane with G7, G18, G19.

The stock Doosan post I started with as a reference does not call a D value when calling a G41 command.

Still digging through available docs and looking forward to the docs generously offered by DouglasRizzo.
 
The method of invoking radius compensation on lathe and milling machines are slightly different.
On a milling machine, we use, for example,
G41 D01;
G01 X_ Y_ F_;
These two can be combined in a single block if G01 is already active: G41 D01 X_ Y_ F_;
D01 would read the radius value entered in the first row under the D column (geometry and wear values are added).

On a lathe, once a tool is called with offset number, say, T0101, the control gets all the information about the tool, including the nose radius and tip direction. So, only G41/G42 are used for invoking radius compensation.

There is a lot more to radius compensation. You first try to use it on a milling machine, which is simple. Lathe would be next.
 
sinha said:
The method of invoking radius compensation on lathe and milling machines are slightly different.
On a milling machine, we use, for example,
G41 D01;
G01 X_ Y_ F_;
These two can be combined in a single block if G01 is already active: G41 D01 X_ Y_ F_;
D01 would read the radius value entered in the first row under the D column (geometry and wear values are added).

On a lathe, once a tool is called with offset number, say, T0101, the control gets all the information about the tool, including the nose radius and tip direction. So, only G41/G42 are used for invoking radius compensation.

There is a lot more to radius compensation. You first try to use it on a milling machine, which is simple. Lathe would be next.
Click to expand...

So, I am confident in my mill based G41/G42 comp. On the lathe, I have been slowly gathering confidence with tool nose radius compensation.

The question of the thread is more focused on how the milling compensation is handled on live milling tools in a lathe - mill/turn machine.

If I write:
G41 D01

There is no D column in offsets/wear - only R and T for tool nose radius compensation. In that case, does the G41 D01 pull the value from the R column? Also, a mill/turn machine can mill with live tooling on two seperate planes - guessing that requires G17 and G18 calls for any compensation to work.
 
I just had the pleasure of teaching myself all about comp on a mill turn machine. (Also Fanuc 18i) this is what I've learned so far

First you are correct in assuming that you need to select the proper plane G17,G18,G19. Generally for milling you'll use G17, and G19. And G18 for turning.

A "D" word is not needed. As said before the offset has been selected previously by either T0101 or in the case of my B axis side G43 H1. (Lathe controls are neat this way)
The value from the "R" column of both the geom and wear pages are used just as "D" on a mill.

So it's pretty easy. You can just call the proper plane and add the comp to a linear feed move like you would on a mill. No D# needed. Cancel similarly on a move away from your profile with G40.

Hope that all made sense
 
rifle guy said:
I just had the pleasure of teaching myself all about comp on a mill turn machine. (Also Fanuc 18i) this is what I've learned so far

First you are correct in assuming that you need to select the proper plane G17,G18,G19. Generally for milling you'll use G17, and G19. And G18 for turning.

A "D" word is not needed. As said before the offset has been selected previously by either T0101 or in the case of my B axis side G43 H1. (Lathe controls are neat this way)
The value from the "R" column of both the geom and wear pages are used just as "D" on a mill.

So it's pretty easy. You can just call the proper plane and add the comp to a linear feed move like you would on a mill. No D# needed. Cancel similarly on a move away from your profile with G40.

Hope that all made sense
Click to expand...

Thank you - it makes sense.
I am also reading through the PDF docs generously provided by @DouglasRizzo

Seems easy enough now that I know the subtle differences between a mill control and lathe control. I am set to make a real part on Tuesday with this machine and this open question was the last major concern. Pretty excited to dive deep into mill/turn and finish a complex part in a single operation.
 
Ok - here is what I have gathered so far.

Cutter compensation with live tools oriented on the X-axis: [tools sticking straight out of the turret]
Call the plane with G19 to select the Y-Z plane and the centerline of the tool is on the X-axis.
Use G41/G42 as you would normally do on a mill, but without the 'D' value.
The control will use the R-value related to the tool offset you call during the tool change.
Don't forget to reset the plane back to G18 for turning.



Cutter compensation with live tools oriented on the Z-axis: [tools at a right angle exiting the turret]
Call the plane with G17 to select the X-Y plane and the centerline of the tool is on the Z axis.
Use G41/G42 as you would normally do on a mill, but without the 'D' value.
The control will use the R-value related to the tool offset you call during the tool change.
Don't forget to reset the plane back to G18 for turning.


Still trying to figure out what the T-value does in this context.
What is 0 and what is 9?
 
0 and 9 are same. These nose numbers are used when the center of the nose is made the reference point of the tool (which nobody does).
Radius compensation on lathe, with live or rigid tools, are fundamentally same.
 
rifle guy said:
I just had the pleasure of teaching myself all about comp on a mill turn machine. (Also Fanuc 18i) this is what I've learned so far

First you are correct in assuming that you need to select the proper plane G17,G18,G19. Generally for milling you'll use G17, and G19. And G18 for turning.

A "D" word is not needed. As said before the offset has been selected previously by either T0101 or in the case of my B axis side G43 H1. (Lathe controls are neat this way)
The value from the "R" column of both the geom and wear pages are used just as "D" on a mill.

So it's pretty easy. You can just call the proper plane and add the comp to a linear feed move like you would on a mill. No D# needed. Cancel similarly on a move away from your profile with G40.

Hope that all made sense
Click to expand...

PM me if you need help. I no longer work for Doosan - I own my own shop now - but I will gladly help if you need.
 
You must log in or register to reply here.

Similar threads

Nerdlinger
Understanding Lathe/Mill Cutter Comp Startup Moves
3 4 5
Replies
88
Views
4K
angelw
A
E
Fanuc 31iB turning center cutter comp
Replies
7
Views
472
EmGo
EmGo
H
Fanuc 30i - Cutter Comp in G19 Not Working
Replies
2
Views
434
PROBE
P
dandrummerman21
Fanuc 16ia cutter comp parameter - cutter comp in a "straight line toolpath"
Replies
11
Views
631
SeymourDumore
S
J
Best practice to machine a cylindrical elongated hole on a turning center
Replies
6
Views
231
???
???








 

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