[1320feet]

My machine will not move in cutter comp today.
I inserted .05 for tool 3 in radius offset. I then watch the machine coordinates between line N825 and N830 and nothing moves.
Machine is at X-11.1416 Y-12.3292 (machine coordinates) on line N825 and N830. If I change tool 3 offset to .002 the machine will not move.
If I change G56 X10.6931 Y-2.9598 on line N820 to X9.6931 Y-2.9598 the machine and machine coordinates will move from X-12.1416 to X-11.1416 weather I have .002 or .05 in tool 3 offset.


Mori seiki SV500 with fanuc 18i

here is the code

( CUT FRONT RAD )
N815 T3 M6
N820 G0 G40 G90 G56 X10.6931 Y-2.9598 S10000 M3
N825 G43 H3 Z2. T4
N830 G42 D3 X10.6931 Y-2.9598
N835 Z.1
N840 G8 P1
N845 M8
N850 G1 Z-.1004 F150.
N855 X.5606 Y-2.0043

[mactec54]

My machine will not move in cutter comp today.
I inserted .05 for tool 3 in radius offset. I then watch the machine coordinates between line N825 and N830 and nothing moves.
Machine is at X-11.1416 Y-12.3292 (machine coordinates) on line N825 and N830. If I change tool 3 offset to .002 the machine will not move.
If I change G56 X10.6931 Y-2.9598 on line N820 to X9.6931 Y-2.9598 the machine and machine coordinates will move from X-12.1416 to X-11.1416 weather I have .002 or .05 in tool 3 offset.


Mori seiki SV500 with fanuc 18i

here is the code

( CUT FRONT RAD )
N815 T3 M6
N820 G0 G40 G90 G56 X10.6931 Y-2.9598 S10000 M3
N825 G43 H3 Z2. T4
N830 G42 D3 X10.6931 Y-2.9598
N835 Z.1
N840 G8 P1
N845 M8
N850 G1 Z-.1004 F150.
N855 X.5606 Y-2.0043

Format is everything when using cutter comp remove the G40 this is canceling the cutter comp. this should be in the safety line at the start of the program here is a PDF which should get you going.

[1320feet]

Format is everything when using cutter comp remove the G40 this is canceling the cutter comp. this should be in the safety line at the start of the program here is a PDF which should get you going.

The G40 was not there when I started. I had entered it after to see if it made any difference.

[Superman]

here is the code

( CUT FRONT RAD )
N815 T3 M6
N820 G0 G40 G90 G56 X10.6931 Y-2.9598 S10000 M3
N825 G43 H3 Z2. T4
N830 G42 D3 X10.6931 Y-2.9598
N835 Z.1
N840 G8 P1
N845 M8
N850 G1 Z-.1004 F150.
N855 X.5606 Y-2.0043

The G40 is NOT the problem, it is forcing the machine to go to the absolute position stated on N820
What is missing is a feedrate on N830, but that line can't make a move as it is the same position as N820

... what does G8 P1 do?... does it force any XY movement ?

N855 is the first line that would make any adjustment to cutter path (using comp), and it really depends on the following code after N855

To put you into the picture about the sequence

Rapid to point over descend point ( ie. circle centre)
Rapid to reference plane above part
Feed into part Z
Feed to your part edge while taking up Comp(G41/G42)
Feed follow the shape contour
Feed off the edge while cancelling comp (G40)(target point must be away from your part)
Rapid retract to reference plane above part
Rapid to next....

There are additional rules ( ie comp starts/finishes using a linear move, but go little steps

Normally.. metal machining uses climb milling (G41 ... cutter to the left of a contour shape)
... but there maybe times when stepping right (G42) is used.

[1320feet]

What is missing is a feedrate on N830, but that line can't make a move as it is the same position as N820

... what does G8 P1 do?... does it force any XY movement ?.

It is still in G0 so no feed rate is needed. I thought N830 should move the .05 I had in radius offset. G8 P1 is turning on high speed look ahead.

[Superman]

It is still in G0 so no feed rate is needed. I thought N830 should move the .05 I had in radius offset. G8 P1 is turning on high speed look ahead.

G0 ???
G41 & G42 force a feed move and is controlled by a feed action
Rapid is (older machines) where each axis runs at max rate to target point.... a bit hard if you descend into a solid part, then use comp to adjust the toolpath while still cutting material.

The 0.05 comp adjust is in what direction ? Going in what direction ? ... there is no data for it to adjust.

You need to have an approach to the comp take-up point of MORE THAN what the comp value being applied...same goes with the cancelling move, AND any internal rads have to be larger than the comp value used.

The lookahead is a nice feature, but I think it's best use is when surfacing features that are controlled by a high density of point-to-point moves. It would allow the control to have better motion over the processing of the point moves.

[the_gentlegiant]

Reiterating some of the stuff mentioned.

The G40 near the beginning is perfectly fine in a safety line. I use one all the time.

The reason you get no change in position is you're turning on comp without a move. I'm surprised you're not getting an alarm. You either need to move a least the length of your D offset, or you can have a very small linear move first, as long as the very next move is an arc move with an arc size that is a hair greater then the entered tool radius.

G8P1 look ahead is great to use anytime. It makes the machine cut more accurately at any feedrate or feature style. Only problem on some of these SV Mori's is it can cause marks on the floor of the part unless it's detuned a little. There are posts on the www about this.

Why are you using G42? Are you conventional milling? Never used G42 in my life on a mill. Have only used it on a lathe.

I would get your tool into a clear area and at depth, then start G8 and G41 PROPERLY.

Read any Fanuc Operations Manual on Cutter Comp. Should solve your problems.

[machinehop5]

...picture worth a thousand words is true. This may help. Also, overlap the ending cut min cutter diameter in your program.

Attachment 489548
https://cnc-programming-tips.blogspo...pensation.html

[kobra_wizzard]

you need to put the D3 onto the same line as your tool offset call.

e.g N825 G43 H3 D3 Z2. T4
N830 G01 G42 X10.6931 Y-2.9598 F?

you can leave the G40 where it is, it should indeed be on your safety line, but because your tool-comp code (G42) is after the G40 it won't intefere

[kobra_wizzard]

conventional milling can improve finish on certain materials and can also reduce vibration when using longer tools to finish cut

[the_gentlegiant]

you need to put the D3 onto the same line as your tool offset call.

Even though it's a handy place to put it, this statement is incorrect. At least on a Fanuc.

Interesting about conventional milling finishes being better. What materials are you suggesting work better this way?

[mactec54]

you need to put the D3 onto the same line as your tool offset call.

e.g N825 G43 H3 D3 Z2. T4
N830 G01 G42 X10.6931 Y-2.9598 F?

you can leave the G40 where it is, it should indeed be on your safety line, but because your tool-comp code (G42) is after the G40 it won't intefere

N820 G0 G40 G90 G56 X10.6931 Y-2.9598 S10000 M3 This line is the same X Y move as the G42 line so it is not going to do anything. D3 can be on the same line as the cutter comp call, G42D3 is fine, what needs to happen is a move on that line.

N825 G43 H3 Z2. T4
N830 G42 D3 X10.6931 Y-2.9598 same X Y move as above it is not going to work.

Example below sniped from the PDF I posted gives the correct move to engage cutter comp, it can of cause be placed anywhere in a Program.

%
O999
G20 G90G40 G49 G80
T1M6
S3056 M3
G0 G90 G54 X-0.01 Y-0.4
G43 H1 Z-0.2 M8
G1 Y2.01 F24.
X3.01
Y-0.01
X-0.4
G0 Y-0.4
G41 X0.375 D1 ( Cutter comp 0n)
G1 Y1.625
X2.625
Y0.375
X-0.4
G0 G40 Y-0.4 (Cutter Comp 0ff)

Another example, Note no feed move required G0 in Modal so no need for a feed move. ( This has been the Faunc Format since 1980 for Cutter Comp)

O1000
N1 G90 G80 G40
N2 T1 M6
N3 G54 G0 X-1.0 Y-1.0 S2500 M3 (Rapid to off the left corner of part.)
N4 G43 H1 Z-.5 M8(Set tool length.)
N5 G41 D31 X0 Y-.5 (Set comp in offset #31, approaching from left.)
N6 G1 Y1.75 F25.0 (Cut part.)
N7 G2 X.25 Y2.0 R.25
N8 G1 X1.75
N9 G2 X2.0 Y1.75 R.25
N10 G1 Y0
N11 X-.5
N12 G0 G40 X-1.0 Y-1.0 (Cancel comp going back to original point.)

[1320feet]

If I change this N820 G0 G40 G90 G56 X10.6931 Y-2.9598 S10000 M3
to this N820 G0 G40 G90 G56 X9.6931 Y-2.9598 S10000 M3 it will move to the same position as the previous line watching the machine position on the screen. It moves to the same machine position no matter what I place in the radius comp.
I like G42 because it makes a bore larger with a positive number. If I use G41 I would have to place negative numbers in the control. For whatever reason G42 make more sense to me. I just read in my Mori programing manual that the cutter comp buffers the next 2 lines to determine what side to go to.I will try the following and see how it works.

N815 T3 M6
N820 G0 G40 G90 G56 X12.6931 Y-2.9598 S10000 M3
N825 G43 H3 Z2. T4
N830 G42 D3 X11.6931 Y-2.9598
N832 X10.6931 Y-2.9598
N835 Z.1
N840 G8 P1
N845 M8
N850 G1 Z-.1004 F150.
N855 X.5606 Y-2.0043

[1320feet]

This worked and the comp was engaged on line N830.

[mactec54]

If I change this N820 G0 G40 G90 G56 X10.6931 Y-2.9598 S10000 M3
to this N820 G0 G40 G90 G56 X9.6931 Y-2.9598 S10000 M3 it will move to the same position as the previous line watching the machine position on the screen. It moves to the same machine position no matter what I place in the radius comp.
I like G42 because it makes a bore larger with a positive number. If I use G41 I would have to place negative numbers in the control. For whatever reason G42 make more sense to me. I just read in my Mori programing manual that the cutter comp buffers the next 2 lines to determine what side to go to.I will try the following and see how it works.

N815 T3 M6
N820 G0 G40 G90 G56 X12.6931 Y-2.9598 S10000 M3
N825 G43 H3 Z2. T4
N830 G42 D3 X11.6931 Y-2.9598
N832 X10.6931 Y-2.9598
N835 Z.1
N840 G8 P1
N845 M8
N850 G1 Z-.1004 F150.
N855 X.5606 Y-2.0043

The only problem I see is that the N830 Line has not moved to engage the G42 Cutter Comp, it has to move at least the diameter of the tool, Buffering is normal this has nothing to do with Cutter Comp.

[mactec54]

This worked and the comp was engaged on line N830.

That would be hit and miss if it did work, not a safe way to do it, no by the manual it never engaged until line 3

With what the manual is saying is that it is starting the offset at position 3 which you would normally start at the G42 Line if that was a move, so unless you programed it to work like this then it would be using line 2 move to engage line 3 to start the Cutter Comp

[1320feet]

One thing I never mentioned is I'm using cutter comp for fine tuning a dimension. I am using Mastercam for the main cutter offset.

[the_gentlegiant]

......... it has to move at least the diameter of the tool, Buffering is normal this has nothing to do with Cutter Comp.

Probably just an oversight, but that would be radius.

And the truth is, even that is not always true. I'll get to that later when I can show an example image.

One thing I never mentioned is I'm using cutter comp for fine tuning a dimension. I am using Mastercam for the main cutter offset.

Ahaa... so you're already running an offset path. Makes a big difference. Then your move to turn on comp hardly needs to be anything at all. Personaly I never use offset finishing passes, but I think that's how they work.

[mactec54]

One thing I never mentioned is I'm using cutter comp for fine tuning a dimension. I am using Mastercam for the main cutter offset.

So, you have not been telling us the whole story, you are using the G42 it to do a finishing cut that a big difference and an ass backwards way to doing a machining process, if it works for you then good luck, it sure would not fly if you were doing any kind of production.

[Superman]

So, you have not been telling us the whole story, you are using the G42 it to do a finishing cut that a big difference and an ass backwards way to doing a machining process, if it works for you then good luck, it sure would not fly if you were doing any kind of production.

He's doing it his way.... not YOUR way
Stop trying to bully or abuse people to your way.
You have riled others, please don't in this thread

It has been stated previously to what is "normal", he stated why he did it that way, so bite your tongue.