Hello Guest it is March 08, 2021, 04:17:05 AM

Author Topic: Very basic question about tool diameter compensation  (Read 36116 times)

0 Members and 1 Guest are viewing this topic.

Re: Very basic question about tool diameter compensation
« Reply #10 on: August 08, 2008, 01:27:12 PM »
So I take it tool diameter compensation has to be done before Mach3? Will LazyCam do this perhaps? It's not that I'm terribly afraid of G Code, it's that it would be much more efficient for me to simply change a parameter when I need to try a different tool, instead of opening an editor, remembering what I'm supposed to do, make the changes, and hope I didn't make a mistake.

Offline ger21

*
  • *
  •  6,289 6,289
    • View Profile
    • The CNC Woodworker
Re: Very basic question about tool diameter compensation
« Reply #11 on: August 08, 2008, 01:54:12 PM »
So I take it tool diameter compensation has to be done before Mach3?

The G-code needs the G41/G42/G40 in it, and must be coded correctly to allow for the lead in. But if you use G42 Dx, then all you'll ned to do is change the tool diameter in the tool table to make adjustments for tool size.
Gerry

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

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

Offline jimpinder

*
  •  1,232 1,232
  • Wakefield, West Yorks, UK
    • View Profile
Re: Very basic question about tool diameter compensation
« Reply #12 on: August 09, 2008, 08:25:23 AM »
Yes Gerry -
We understand the pros and cons - but what we need is someone who can properly explain G41 and G42 to us - i.e. comp left and right etc. - for example if you are cutting a window with the tool on the inside, which with standard bit rotation would probably mean you are cutting round in a clockwise direction, what do you use, and for example (since it says left and right) do you need to alter it when you come down the other side)???
Not me driving the engine - I'm better looking.
Re: Very basic question about tool diameter compensation
« Reply #13 on: August 09, 2008, 08:58:53 AM »
Hi, Imagine the cutter is a car with 2 steering wheels, one on the left for turning left and one on the right for turning right.
OK so far.

So you get in your car on the right hand side and drive. You can only turn right hand turns so, eventually if you turn 4 rights you have travelled in a rectangle or square. Which ever compensation you used, right for a hole, left for an island. You did not need to change it.

Now lets say the road is an S shape. The start of the S is a left hand turn so jump over to the left seat of the car and start driving left. You follow the S road until you get to the middle of the S you will see that you will need to turn to the right. To do this you have to stop the car and jump into the right hand seat to turn right.

The point at which you have to jump over to the correct seat in the car is the point at which you need to change the cutter compensation if you want to keep following the correct cutter path.

If you were actually cutting an S in material and you had only left compensation on, the bottom of the S would follow the correct path but the top part would not.



 John

Offline ger21

*
  • *
  •  6,289 6,289
    • View Profile
    • The CNC Woodworker
Re: Very basic question about tool diameter compensation
« Reply #14 on: August 09, 2008, 09:47:12 AM »
Hi, Imagine the cutter is a car with 2 steering wheels, one on the left for turning left and one on the right for turning right.
OK so far.

So you get in your car on the right hand side and drive. You can only turn right hand turns so, eventually if you turn 4 rights you have travelled in a rectangle or square. Which ever compensation you used, right for a hole, left for an island. You did not need to change it.

Now lets say the road is an S shape. The start of the S is a left hand turn so jump over to the left seat of the car and start driving left. You follow the S road until you get to the middle of the S you will see that you will need to turn to the right. To do this you have to stop the car and jump into the right hand seat to turn right.

The point at which you have to jump over to the correct seat in the car is the point at which you need to change the cutter compensation if you want to keep following the correct cutter path.

If you were actually cutting an S in material and you had only left compensation on, the bottom of the S would follow the correct path but the top part would not.



 John

I thought I already explained it in one of my previous posts.

But in regards to following an S shape, you do NOT switch from left to right comp. If you are cutting out a letter S, you use the same comp, all the way around. You use Left or right depending on whether you want to climb cut or conventional cut.

Think of driving down a two lane road, and the center line is the toolpath. G42 is driving on the American side, G41 is driving on the British side. Changing the comp would cause you to cross the line. You never switch comp direction in the middle of a cut. If you drive along an S shaped road, you don't cross the center line when you switch from turning right to turning left, do you?
Gerry

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

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: Very basic question about tool diameter compensation
« Reply #15 on: August 09, 2008, 10:07:24 AM »
Duh, So I'm another one that's got it wrong!

I think I'll stay as confused as everyone else.

Offline ger21

*
  • *
  •  6,289 6,289
    • View Profile
    • The CNC Woodworker
Re: Very basic question about tool diameter compensation
« Reply #16 on: August 09, 2008, 10:28:12 AM »
- for example if you are cutting a window with the tool on the inside, which with standard bit rotation would probably mean you are cutting round in a clockwise direction, what do you use, and for example (since it says left and right) do you need to alter it when you come down the other side)???

Again, I explained it in my previous post, and offered an example for cutting around the outside. Here's one for the inside.

G40
M3
G0 Z0.1250
G0 X0.6391 Y0.7309 Z0.1250
G1 X0.6391 Y0.7309 Z-0.2500 F50
G42P0.25
G1 X0.0000 Y1.5000 Z-0.2500 F150
G1 X0.0000 Y3.0000 Z-0.2500
G1 X3.0000 Y3.0000 Z-0.2500
G1 X3.0000 Y0.0000 Z-0.2500
G1 X0.0000 Y0.0000 Z-0.2500
G1 X0.0000 Y1.9312 Z-0.2500
G40
G1 X0.5000 Y1.9312 Z-0.2500
G0 X0.5000 Y1.9312 Z0.1250
G0 X0 Y0
M5
M30
Gerry

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

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

Offline ger21

*
  • *
  •  6,289 6,289
    • View Profile
    • The CNC Woodworker
Re: Very basic question about tool diameter compensation
« Reply #17 on: August 09, 2008, 11:01:07 AM »
Here's an S.

G40
M3
G0 Z0.1250
G0 X1.5603 Y4.3285 Z0.1250
G1 X1.5603 Y4.3285 Z-0.1000 F50
G42P0.0625
G1 X1.1250 Y4.2500 Z-0.1000 F150
G3 X1.1250 Y2.0000 Z-0.1000 I0.0000 J-1.1250
G2 X1.1250 Y0.2500 Z-0.1000 I0.0000 J-0.8750
G3 X1.1250 Y0.0000 Z-0.1000 I0.0000 J-0.1250
G3 X1.1250 Y2.2500 Z-0.1000 I0.0000 J1.1250
G2 X1.1250 Y4.0000 Z-0.1000 I0.0000 J0.8750
G3 X1.1250 Y4.2500 Z-0.1000 I0.0000 J0.1250
G2 X1.0000 Y4.3750 Z-0.1000 I0.0000 J0.1250
G40
G1 X1.0000 Y4.6250 Z-0.1000
G0 X1.0000 Y4.6250 Z0.1250
G0 X0 Y0
M5
M30
Gerry

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

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

Offline bowber

*
  •  216 216
  • Kirkby Stephen,Cumbria, UK
    • View Profile
Re: Very basic question about tool diameter compensation
« Reply #18 on: August 09, 2008, 02:21:11 PM »
As Gerry has said one is for going down the left of the line (tool path) as you look in the direction of travel (g41) the other is for going down the right of the line as you look in the direction of travel (g42)
You can can also lie to it to alter the offset in relation to the size of the cutter to get a larger or smaller part (or hole)
G41 also climb cuts while G42 is conventional cutting.
So if your machine has a significant amount of backlash then always use G42 and go Anti clockwise to cut on the outside and clockwise to cut on the inside.

I tend to use a CAM program though as it sorts it all out for you and it always says in the code what size cutter was used.

Steve

Offline Sam

*
  • *
  •  987 987
    • View Profile
    • hillbillyhilton.com
Re: Very basic question about tool diameter compensation
« Reply #19 on: August 10, 2008, 05:21:19 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? That is the standard way of doing it, right? If there is indeed a reason for the D word, please tell. I know I was at a loss trying to use comp without the D word. In 99% of my projects, tool comp is applied inside the cam program, not at the control. However, there are times when needed at the control.
Quote
3) Basically the same as #2, but don't call any tool at all. Mach3 will use the diameter of the current tool (based on the diameter in the tool table). Just use G41 or G42.
Don't seem to work for me. Never has. Maybe I'm just doing something wrong. Maybe this has been giving other people trouble as well.

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

If I insert a D value, toll comp IS applied. For instance if I change the first line to....

g90g20g61t1d1f1000
or
g90g20g61d1f1000
(whichever one you prefer, pick your poison)

now....stay with me here...if you edit the code AGAIN, back to the original way it was, (without the D value, and only a T call) tool comp magically works, and I can modify the value in the tool table, and MACH will indeed account for those changes.

So, in short..... If you use code without a D value, a tool call alone will not work. If you ADD a D value, and then remove it, a tool call alone WILL work. Strange indeed.
"CONFIDENCE: it's the feeling you experience before you fully understand the situation."