Hello Guest it is March 08, 2021, 04:17:47 AM

Author Topic: Very basic question about tool diameter compensation  (Read 36117 times)

0 Members and 1 Guest are viewing this topic.

Offline Graham Waterworth

*
  • *
  •  2,276 2,276
  • Yorkshire Dales, England
    • View Profile
Re: Very basic question about tool diameter compensation
« Reply #20 on: August 10, 2008, 06:11:45 PM »
I have been asked to try and clarify the cutter compensation debate (CC) that keeps raging on and on and on.........

The basics

Compensation is not a quick fix.

Cutter compensation is used to adjust the size of a cut area, this can be on the outside or the inside of a component or section of a component.

Compensation has to be planned into the job, it is not easy to adapt afterwards.

When programming the job the tool is programmed on the centre line of the cut.

When programming the part any inside radius can not be smaller than the radius of the cutter to be used.

The machine should never rapid with an active G41 or G42, Mach3 may allow this move just as you can drive your car off a cliff, its not advisable.

You should not change local (G52) or global (G54-G59 Etc.) work offsets while a G41 or G42 is active.

Cutter compensation should not be used for pocketing and area clearance.

How it works


To use CC we have to command a G41 or a G42, the one we use depends on which side of the line we are on and what direction we want to travel.  The next consideration is how we move onto the cutter path, we can not rapid straight onto the line and start cutting, we have to create a lead in line.  We also have to have lead out lines.  This is why you have to pre-plan CC.

A lead line can be a straight line or an arc or a combination of both.  Straight line moves are the easiest, arcs give the best blend.

The picture below shows 4 examples of how we can use CC, the top 2 show cutting on the outside of the green line.  The bottom two are slots so are cutting on the inside of the green line.

The parts are 10mm wide and 50mm long giving 40 mm centres on the rads.  The example code was written for the use of a 2mm dia end mill.  Before anybody tells me this is not the best cutter for the job, I don't care.

More later........

Graham.

%
G54 G00 G90 G43
T1 M6
S1500 M3

(FIG 1 - CCW INSIDE)
G00 X41.5 Y-2.5
G00 Z1.
G01 Z-2. F900.
G41 X42.5 Y2.5 F1800.
G03 X40. Y5. R2.5
G01 X0.
G03 X-5. Y0. R5.
X0. Y-5. R5.
G01 X40.
G03 X45. Y0. R5.
X40. Y5. R5.
X37.5 Y2.5 R2.5
G01 G40 X38.5 Y-2.5
G00 Z25.

(FIG 2 - CW INSIDE)
G00 X61.713 Y-2.5
Z1.
G01 Z-2. F900.
G42 X60.713 Y2.5 F1800.
G02 X63.213 Y5. R2.5
G01 X100.
G02 X105. Y0. R5.
X100. Y-5. R5.
G01 X60.
G02 X55. Y0. R5.
X60. Y5. R5.
G01 X63.213
G02 X65.713 Y2.5 R2.5
G01 G40 X64.713 Y-2.5
G00 Z25.

(FIG 3 - CCW OUTSIDE)
G00 X41.5 Y42.5
Z1.
G01 Z-2. F900.
G42 X42.5 Y37.5 F1800.
G02 X40. Y35. R2.5
G01 X0.
G03 X-5. Y30. R5.
X0. Y25. R5.
G01 X40.
G03 X45. Y30. R5.
X40. Y35. R5.
G02 X37.5 Y37.5 R2.5
G01 G40 X38.5 Y42.5
G00 Z25.

(FIG 4 - CW OUTSIDE)
G00 X61.074 Y42.5
Z1.
G01 Z-2. F900.
G41 X60.074 Y37.5 F1800.
G03 X62.574 Y35. R2.5
G01 X100.
G02 X105. Y30. R5.
X100. Y25. R5.
G01 X60.
G02 X55. Y30. R5.
X60. Y35. R5.
G01 X62.574
G03 X65.074 Y37.5 R2.5
G01 G40 X64.074 Y42.5
G00 Z25.
G91 G28 Y0 Z0
M30
%
« Last Edit: August 10, 2008, 06:14:05 PM by Graham Waterworth »
Without engineers the world stops

Offline Graham Waterworth

*
  • *
  •  2,276 2,276
  • Yorkshire Dales, England
    • View Profile
Re: Very basic question about tool diameter compensation
« Reply #21 on: August 10, 2008, 06:22:02 PM »
I am at a loss at to why a tool number is even called with a D word. Why not just use the currently called tool number?

Sam,

The 'D' in tool compensation has many uses, as a quick example:-

If you had to rough and finish the outside of a stainless steel part you could use a main program to call a sub program of the finished shape and by using 2 different D's you could use the same sub with 2 different sized tools.

Graham.
Without engineers the world stops

Offline Sam

*
  • *
  •  987 987
    • View Profile
    • hillbillyhilton.com
Re: Very basic question about tool diameter compensation
« Reply #22 on: August 10, 2008, 07:40:47 PM »
Quote
you could use the same sub with 2 different sized tools.
I see. Thank you. I can think of more than once that would have come in handy.
"CONFIDENCE: it's the feeling you experience before you fully understand the situation."

Offline ger21

*
  • *
  •  6,289 6,289
    • View Profile
    • The CNC Woodworker
Re: Very basic question about tool diameter compensation
« Reply #23 on: August 10, 2008, 08:37:53 PM »

If I load Mach from scratch, and load this program, tool comp is NOT applied.

g90g20g61t1f1000
g01x-0.5y-0.5
g01g42x0.0y0.0
x2.0y0.0
x2.0y2.0
x0.0y2.0
x0.0y0.0
x2.0y0.0
g01g40x2.5y-0.5
m30


When you first start Mach3, the current tool is tool 0, which is probably why it doesn't work.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline Sam

*
  • *
  •  987 987
    • View Profile
    • hillbillyhilton.com
Re: Very basic question about tool diameter compensation
« Reply #24 on: August 10, 2008, 09:17:54 PM »
Your absolutely correct, Gerry. I didn't complete the tool call using M6, so it remained at tool 0. Goes to show how much manual coding I do. Good catch.
"CONFIDENCE: it's the feeling you experience before you fully understand the situation."
Re: Very basic question about tool diameter compensation
« Reply #25 on: August 12, 2008, 06:50:45 PM »
hi sid
i havent read all the posts on this topic so someone may have already explained this better but i have a reasonable understanding of cutter
compensation ie left or right.
basically it relates to cutter direction in relation to the programmed path. for G41 (left) the tool will CLIMB mill and for G42 (right) the tool will conventional mill
to put this clearer - if you want to cut the outside of a circle in a clockwise motion use G41
                                - if you want to cut the outside of a circle in an anticlockwise motion use G42
another way to look at it is if you look at the cutter as it cuts away from you , the cutter compensation will put the on either the left or the right of the programmed path. LEFT (G41) for left ect ect
as far as actually calling it up in mach3 i dont know yet. im a newby myself
hope i helped
Re: Very basic question about tool diameter compensation
« Reply #26 on: August 16, 2008, 05:51:34 PM »
While I appreciate all the G Code info (It encouraged me to dig in a little deeper), I have been a little confused as to why nobody told me how to do it in Lazycam. I think I might have just answered my own question. While this is probably obvious to everyone, it took me a little while to figure out the unregistered, non-pro version of lazycam apparently doesn't do tool compensation. I tried adding the appropriate G-codes, but I must not have gotten the syntax right. Can anyone tell me if it's worth it to buy the registered version? I'm a little nervous, it being in beta still, with no instructions.

Offline RICH

*
  • *
  •  7,419 7,419
    • View Profile
Re: Very basic question about tool diameter compensation
« Reply #27 on: August 16, 2008, 08:53:38 PM »
RCHADWICK,
"Can anyone tell me if it's worth it to buy the registered version?"

I can only speak for myself. I use it mainly for the lathe and still learning for the mill. My answer would be yes for a few reasons.
1. Where alse are you going to get a program like that for what your going to pay?
    It's Beta? Hell, I beta'd for five years with one particular program and frankly I think 10 years from now you will
    still be "beta-ing" with any program because nothing stands still.
2. Where else are you going to get the kind of support provided by realy nice knowledgable people? 
    May I add that some do it for a living so will add professional to the people discription.
3. Where else would someone spend the time to explain what you just picked up from this thread?
4. Where alse can you get someone to stay by your side, have you in their thoughts, until you arrived at an end of a
    problem in trying to do or learn something?
5. Some programs require more that what you pay for it just as a yearly support fee and addtionaly you should end up
    getting upgrade for free.
6. Sooner or later you will want to do or try something complex and you will appreciate that program.
Again, just something to think about.
RICH

Offline bowber

*
  •  216 216
  • Kirkby Stephen,Cumbria, UK
    • View Profile
Re: Very basic question about tool diameter compensation
« Reply #28 on: August 17, 2008, 01:52:23 PM »
Not used lazycam but if it works like most other cam programs then it doesn't use cutter compensation.

You tell the cam program the process needed (inside, outside, left, right) and the tool size and the program works out the rest and outputs code for the centre line of the cutter so you have to use that size cutter to cut the job.
Sheetcam can add or remove an amount set in the process dialog so you can leave a small amount for a finishing cut etc, non of this uses G41/42 but seems to off set the original lines.

Years ago when I was using CNC for work we used to have to hand code so we always wrote the code for the centre line of the job and then applied tool compensation.
Now I don't use it, I just send the job through my cam program with a different cutter if I have to change it.

Steve

Offline ger21

*
  • *
  •  6,289 6,289
    • View Profile
    • The CNC Woodworker
Re: Very basic question about tool diameter compensation
« Reply #29 on: August 17, 2008, 02:04:39 PM »
While I appreciate all the G Code info (It encouraged me to dig in a little deeper), I have been a little confused as to why nobody told me how to do it in Lazycam.

Don't use it.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html