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

CRC help

O

overtimeking

Plastic
Joined
Jun 5, 2014
Location
england
I just started this new place and noticed we don’t put no radius compensation in tool data, it’s always 0.0.
I have always put the radius of the tool in the tool data. The is also no D number on the G41 line?
Is this normal to you guys? Here’s an example program... any help thanks!

T1M76
G10 L1 P2 R0.0
G12 B0
T3
S1000 M3
G55 X23.0 Y23.0
G43 Z200.0 H1 M8
Z3.0 M26 M735
G1 Z-10.0 F500 M97
Y32.0
G41 Y34.0 F100
G3 J-11.0
G1 G40 Y23.0 F500
G00 Z200
 
overtimeking said:
I just started this new place and noticed we don’t put no radius compensation in tool data, it’s always 0.0.
I have always put the radius of the tool in the tool data. The is also no D number on the G41 line?
Is this normal to you guys? Here’s an example program... any help thanks!
Click to expand...
It's not unusual to program center of spindle and leave the rad/dia offset at zero for full size cutters.

The risk in your program is that since though there is no D called out, the control may use the value for the last D it read. As long as that is zero, no problem. But if it comps when you are not expecting it to, you will lose a part.
 
My default is no comp at all..

Makes the programming easier, don't have to worry about lead in and lead outs..

And it eliminates a point of error, leaving an incorrect value in the offset table.

And then 99% of the time that I do use comp, I use centerline.. Again, less chance
of an error. If I leave .003" in the offset table, odds are I won't scrap anything
next time I use comp.

If you've ever used a machine that is memory limited, sometimes ditching the comp can
make the difference of getting the program into the control or not.

And when I do use full "radius" comp... My machines are set up to use "D"iameter, not "R"adius..
 
Cool thanks for your help,

So because I’m using 0.0 cutter comp, programming to centre of spindle, then just out of interest would it make a difference if it was G41 or G42 in my example?
 
overtimeking said:
Cool thanks for your help,

So because I’m using 0.0 cutter comp, programming to centre of spindle, then just out of interest would it make a difference if it was G41 or G42 in my example?
Click to expand...
No, it would not make any difference, because you are comping a zero value. As soon as you put a number in the D register, it does make a difference.

G41 is for a climb cut, G42 is for a conventional cut. If you program a climb cut tool path with a G42 offset, it's going to offset the tool to the "wrong" side of the line- e.g. it will behave as if the plus/minus sign in the D register is reversed.
 
The only issue with not using cutter comp is if the end mill has been periphery reground or is not exactly to size then the part is wrong. You either have to repost with a different cutter diameter or add the comp in.
 
Cheers thanks for your help, think I’m getting it.
Don’t suppose I could ask you guys for example programs of a center line programmed tool vs edge of tool programmed tool cutting a circle.
It would help me understand better! Thanks for any help you guys can give!
 
Here is EDGE of Tool .500 endmill cutting on the outside of a 2.000" circle.

(T2 1/2 BULL EM 0.03 R H2 D2 D0.5000 R0.0300)
N2 G00 G17 G20 G40 G80 G90
N4 G91 G28 Z0.
N6 (COMP TYPE:CONTROL COMP)
N8 T2 (1/2 BULL EM 0.03 R)
N10 M6
N12 (MAX: Z.1)
N14 (MIN: Z-.25)
N16 G00 G17 G90 G54 X-1.5 Y0. S5900 M03
N18 G43 H2 Z.1
N20 G94 G01 Z-.25 F25.
N22 G41 D2 X-1. F35.4
N24 G02 X1. I1. J0.
N26 X-1. I-1. J0.
N28 G01 G40 X-1.5
N30 G00 Z.1
N32 M05
N34 G91 G28 Z0.
N36 G28 Y0.
N38 G90
N40 M30
 
Here is CENTERLINE .500" endmill cutting on the outside of a 2.000" circle

(T2 1/2 BULL EM 0.03 R H2 D2 D0.5000 R0.0300)
N2 G00 G17 G20 G40 G80 G90
N4 G91 G28 Z0.
N6 (COMP TYPE:WEAR COMP)
N8 T2 (1/2 BULL EM 0.03 R)
N10 M6
N12 (MAX: Z.1)
N14 (MIN: Z-.25)
N16 G00 G17 G90 G54 X-1.75 Y0. S5900 M03
N18 G43 H2 Z.1
N20 G94 G01 Z-.25 F25.
N22 G41 D2 X-1.25 F35.4
N24 G02 X1.25 I1.25 J0.
N26 X-1.25 I-1.25 J0.
N28 G01 G40 X-1.75
N30 G00 Z.1
N32 M05
N34 G91 G28 Z0.
N36 G28 Y0.
N38 G90
N40 M30
 
This depends on what controller you are using, and how it is set up. Sometimes calling T1 will activate and read the register for that tool. I have a Haas, and I call the D word at the tool change, so I don't need to repeat it throughout multiple comp'ed toolpaths. My best guess is that you need to have a D word on you G41 line, or you have no control of the size, regardless of whether you are using tool diameter/radius comp or zero comp at the outset.
 
overtimeking said:
I just started this new place and noticed we don’t put no radius compensation in tool data, it’s always 0.0.
I have always put the radius of the tool in the tool data. The is also no D number on the G41 line?
Is this normal to you guys? Here’s an example program... any help thanks!

T1M76
G10 L1 P2 R0.0
G12 B0
T3
S1000 M3
G55 X23.0 Y23.0
G43 Z200.0 H1 M8
Z3.0 M26 M735
G1 Z-10.0 F500 M97
Y32.0
G41 Y34.0 F100
G3 J-11.0
G1 G40 Y23.0 F500
G00 Z200
Click to expand...

.
ask the programmer
 
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