[qinaide2]

How can i do a off set for Cutter compensation geometry offset register number (D) in fanuc??i want the machine recognize what is the tool diameter.

[SirDenisNayland]

That depends on the particular control, and if its a mill or a lathe you're talking about.

You use G41/G43 to call the offsets and turn on cutter comp.

[qinaide2]

i mean is how can i offset the too diameter in machine??if i just write on the program G41 D01 but didnt offset the tool diameter also useless right?


N10 G90 G00 X0 Y0 Z2 S3000 T1 M03
N20 G91 G00 Z-26
N30 G01 Y0.75 F200
N40 G41 G01 X7.25
N50 G03 X-7.25 Y7.25 Z0.375 I-7.25 J0
N60 G03 X0 Y0 Z1.5 I0 J-8
N70 G03 X-7.25 Y-7.25 Z0.375 I0 J-7.25
N80 G00 G40 X7.25 Y-0.75
N90 G90 Z2

on the program above N40 this step the cutting tool already move to X7.25 if i didnt offset the tool diameter...if i offset the tool diameter it just will move X1.3 only...now i just dont know how to offset the tool diameter in the machine...My machine is MAKINO S33 that using fanuc soffware...So how i can i offset in the fanuc sofware? In tool offset there i just see the height offset didnt see the word tool diameter offset..any expert can tell me how to do??Thanks!!

[angelw]

i mean is how can i offset the too diameter in machine??if i just write on the program G41 D01 but didnt offset the tool diameter also useless right?


N10 G90 G00 X0 Y0 Z2 S3000 T1 M03
N20 G91 G00 Z-26
N30 G01 Y0.75 F200
N40 G41 G01 X7.25
N50 G03 X-7.25 Y7.25 Z0.375 I-7.25 J0
N60 G03 X0 Y0 Z1.5 I0 J-8
N70 G03 X-7.25 Y-7.25 Z0.375 I0 J-7.25
N80 G00 G40 X7.25 Y-0.75
N90 G90 Z2

on the program above N40 this step the cutting tool already move to X7.25 if i didnt offset the tool diameter...if i offset the tool diameter it just will move X1.3 only...now i just dont know how to offset the tool diameter in the machine...My machine is MAKINO S33 that using fanuc soffware...So how i can i offset in the fanuc sofware? In tool offset there i just see the height offset didnt see the word tool diameter offset..any expert can tell me how to do??Thanks!!

The following program will work provided the intention was for the compensation to be to the left of the tool path.

Unless your control is set via parameters to use “Pocket Calculator Format”, make sure you don’t omit periods from integer values other than Zero. If the control is set to the Fanuc default, Z2 will be interpreted as Z0.0002 (Imperial Mode)

The Offset Number used with the D address will depend on the Offset System available on your control. If the Offset Registry has a “D” offset column, then use the same offset number as the Tool Number. If your control uses the same offsets for Tool Length and Cutter radius Compensation, use an Offset Number that relates to the Tool Number in some way. For example add 50 to the tool number and use that as the Cutter Radius Comp offset number. Accordingly, T01 would use H01 for the Tool Length Offset and D51 for the Cutter radius Comp. The radius of the tool being used is registered under the Offset Number corresponding to that used with the “ D” address in your program

Regards,

Bill

N10 G90 G00 X0 Y0 Z2.0 S3000 T1 M03
N20 G91 G00 Z-26.0
N30 G01 Y0.75 F200
N40 G41 G01 X7.25 D01
N50 G03 X-7.25 Y7.25 Z0.375 I-7.25 J0
N60 G03 X0 Y0 Z1.5 I0 J-8.0
N70 G03 X-7.25 Y-7.25 Z0.375 I0 J-7.25
N80 G00 G40 X7.25 Y-0.75
N90 G90 Z2.0

[qinaide2]

How if i use below program to do a thread mill process is it correct??My thread mill diameter is 11.9mm want to make M16 pitch1.5 hole.If after thread mill process use go plug gauge to test still cannot go in. So maybe the thread hole not enough big. if i want to make the hole bigger a bit is it just adjust at N40 and N60 for the figure of R??Anyone can help me?

N10 G90 G54 G43 H1 X0 Y0 Z10 S3000
N20 G00 Z-24
N30 G01 G91 G41 D1 X1.025 Y-1.025 Z0 F200
N40 G03 X1.025 Y1.025 R1.025 Z0.1875
N50 G03 X0 Y0 I-2.05 J0 Z1.5
N60 G03 X-1.025 Y1.025 R1.025 Z0.1875
N70 G01 G40 X-1.025 Y-1.025 Z0
N80 G90 X0 Y0 Z0

[angelw]

How if i use below program to do a thread mill process is it correct??My thread mill diameter is 11.9mm want to make M16 pitch1.5 hole.If after thread mill process use go plug gauge to test still cannot go in. So maybe the thread hole not enough big. if i want to make the hole bigger a bit is it just adjust at N40 and N60 for the figure of R??Anyone can help me?

N10 G90 G54 G43 H1 X0 Y0 Z10 S3000
N20 G00 Z-24
N30 G01 G91 G41 D1 X1.025 Y-1.025 Z0 F200
N40 G03 X1.025 Y1.025 R1.025 Z0.1875
N50 G03 X0 Y0 I-2.05 J0 Z1.5
N60 G03 X-1.025 Y1.025 R1.025 Z0.1875
N70 G01 G40 X-1.025 Y-1.025 Z0
N80 G90 X0 Y0 Z0

You’re using cutter radius compensation. Therefore, the program remains unchanged, and you alter the value of the cutter radius comp registered for D1. To make the cutter cut bigger, you make the value of the cutter radius compensation smaller.

What you’ve done as far as the cutter radius compensation is concerned, is that you have compensated for the radius of the cutter in your program, and you’ve used cutter radius compensation via the control as well. This is often referred to as Partial Cutter Radius Compensation. When using this method, the whole radius of the tool is NOT registered in the Tool Radius Comp Offset registry. In the perfect World, your above program would cut the correct size thread with a Zero value registered for the Cutter Radius Compensation. If you want the thread mill to cut larger, a small Minus value will be registered and the value made more Minus to continue to make the tool cut a larger diameter until the thread gauge fits.

Regards,

Bill

[SirDenisNayland]

In your G3 commands you switch between specifying the radius, and specifying the arc center.

It is best to stick to one format, it makes life easier for anyone reading your program, as well as yourself.

[ChattaMan]

In your G3 commands you switch between specifying the radius, and specifying the arc center.

It is best to stick to one format, it makes life easier for anyone reading your program, as well as yourself.

I always use G3 X Y R
But if I want to do one full revolution, then I use G3 I, as in the example.

@SirDenisNayland....how do you program one full revolution?

[SirDenisNayland]

The short answer is I dont.

The long answer is that it is a 'bad' programming practice which can lead to issues with swapping programs between machines. The way some machines deal with arcs is only in half and quarter circles: this is a "throwback" to days of old where controls were not as powerful and as such I always program in only 90degree arcs for all programs.

Some machines even require you to always specify the arcs using ijk. Even more confusing is that with some machines the ijk specifies the center to the arc from the current machine position, rather than from the position commanded in the same line as the ijk values themselves.

I even have a machine which allows you to specify where the center is in relation to the start and end points using a positive or a negative R value (arc sweep less than or greater than 180degrees), but I never use that because to my knowledge it is only that machine which operates in that manner. This machine will also let me specify a full circle by just putting in the same xy positions and the rad on the G2/3 line.

When you've got several different mills and can and often have to swap existing jobs between them it pays to make your code as tactile as you possibly can.

It's not super critical for everyone, but the methods of circular interp definition are not held to one strict standard, even within the same control manufacturers over the years.

Cheers.

[ChattaMan]

........It's not super critical for everyone, but the methods of circular interp definition are not held to one strict standard, even within the same control manufacturers over the years......

Exactly! So don't pull the guy down for doing it his way. His issue is with cutter comp and not IJ/R.

[angelw]

I even have a machine which allows you to specify where the center is in relation to the start and end points using a positive or a negative R value (arc sweep less than or greater than 180degrees), but I never use that because to my knowledge it is only that machine which operates in that manner.

All Fanuc controls from 6Series Model B on will do as you describe above. This scenario is not as rare as you seem to infer.

This machine will also let me specify a full circle by just putting in the same xy positions and the rad on the G2/3 line.

If you mean that the "rad" referred to in your previous comment can be programmed with an "R" address, then this is not the case with any control, be it Fanuc or any other make. The following attached picture illustrates why. The following program block would seem to satisfy the full circular interpolation of either circle. Accordingly, as there is clear ambiguity regarding which circular path should be executed, the control will execute neither.
G03 X0.0 Y0.0 R-25.0


If you meant that the block can be commanded with the following:
G03 X0.0 Y0.0 I-25.0 or G03 X0.0 Y0.0 I25.0

Then this is valid and has also been around since the Series 6 Model B. The above commands will execute the Left and Right tool paths respectively.

When you've got several different mills and can and often have to swap existing jobs between them it pays to make your code as tactile as you possibly can.

It's not super critical for everyone, but the methods of circular interp definition are not held to one strict standard, even within the same control manufacturers over the years.

Within the realm of the Fanuc control, the only format that would allow for seamless transportation of programs using circular interpolation across all models would be to use I,J and K format and moves within quadrants only.

I personally choose to use only I,J and K format. I do so because I don't find using R format any easier, as is the argument by many. If creating the program manually, you have to calculate the Start and End points of the circular path, with the I, J and K values being byproducts of the calculation. If a CAM system is used, then there is definitely no difference either way in terms of difficulty. I also avoid using the "R" format because there can be inherent errors with regards to the calculated center coordinates when the center angle approaches 180°. Following is a direct Cut and Paste from a Fanuc Manual regarding this matter. I concede, however, that using the "R" format can be handy when used with a lathe to counteract a taper in a part where the profile also contains radii.

Regards,

Bill

Quote from Fanuc Manual
"When an arc having a center angle approaching 180° is specified, the calculated center coordinates may contain an error. In such a case, specify the center of the arc with I, J, and K."

[qinaide2]

You’re using cutter radius compensation. Therefore, the program remains unchanged, and you alter the value of the cutter radius comp registered for D1. To make the cutter cut bigger, you make the value of the cutter radius compensation smaller.

What you’ve done as far as the cutter radius compensation is concerned, is that you have compensated for the radius of the cutter in your program, and you’ve used cutter radius compensation via the control as well. This is often referred to as Partial Cutter Radius Compensation. When using this method, the whole radius of the tool is NOT registered in the Tool Radius Comp Offset registry. In the perfect World, your above program would cut the correct size thread with a Zero value registered for the Cutter Radius Compensation. If you want the thread mill to cut larger, a small Minus value will be registered and the value made more Minus to continue to make the tool cut a larger diameter until the thread gauge fits.

Regards,

Bill

Thanks for your reply MR BILL,
As you say in in the perfect World, my program would cut the correct size thread with a Zero value registered for the Cutter Radius Compensation. After i try this program the size of thread hole is too small so which step of program i need to edit??I didnt registered D1 value so if i want make the thread size bigger just edit step N40 till N60??Can you teach me how to edit the program to get the correct size thread that i want.i'm using MAKINO S33 via fanuc software version CA-0300-AA07 SP1..It is this software can registered the value of D1?If have can you tell me go where to registered the value of D1??i just saw the tool height offset in fanuc software.

[angelw]

Thanks for your reply MR BILL,
As you say in in the perfect World, my program would cut the correct size thread with a Zero value registered for the Cutter Radius Compensation. After i try this program the size of thread hole is too small so which step of program i need to edit??I didnt registered D1 value so if i want make the thread size bigger just edit step N40 till N60??Can you teach me how to edit the program to get the correct size thread that i want.i'm using MAKINO S33 via fanuc software version CA-0300-AA07 SP1..It is this software can registered the value of D1?If have can you tell me go where to registered the value of D1??i just saw the tool height offset in fanuc software.

If you’re not going to register a value in the corresponding offset for the D address used in your program for Cutter Radius Compensation, then there is no point in including in your program, the Cutter Radius Compensation codes G41 and G40 to respectively start and cancel Cutter Radius Compensation.

You will have to edit the blocks from N30 to N70 inclusive, not just N40 to N60, and you will have to edit these blocks every time the tool wears to the extent that the size of the feature is out of tolerance. When Cutter Radius Compensation is available, and particularly as you have it already included in your program, to do what you’re suggesting and edit the program to correct the size, is tantamount to having a dog and barking yourself.

Regards,

Bill

[qinaide2]

If you’re not going to register a value in the corresponding offset for the D address used in your program for Cutter Radius Compensation, then there is no point in including in your program, the Cutter Radius Compensation codes G41 and G40 to respectively start and cancel Cutter Radius Compensation.

You will have to edit the blocks from N30 to N70 inclusive, not just N40 to N60, and you will have to edit these blocks every time the tool wears to the extent that the size of the feature is out of tolerance. When Cutter Radius Compensation is available, and particularly as you have it already included in your program, to do what you’re suggesting and edit the program to correct the size, is tantamount to having a dog and barking yourself.

Regards,

Bill

N10 G90 G00 X0 Y0 Z2 S3747 T1 M3
N20 G91 G00 Z-16
N30 G01 Y0.75 F200
N40 G41 G01 X7.25
N50 G03 X-7.25 Y7.25 Z0.375 I-7.25 J0
N60 G03 X0 Y0 Z1.5 I0 J-8
N70 G03 X-7.25 Y-7.25 Z0.375 I0 J-7.25
N80 G00 G40 X7.25 Y-0.75
N90 G90 G00 Z30

Program above will be using same size of thread mill like previous one. i want to know what is the different between this two program..which program will be better for doing the thread size hole??

[angelw]

N10 G90 G00 X0 Y0 Z2 S3747 T1 M3
N20 G91 G00 Z-16
N30 G01 Y0.75 F200
N40 G41 G01 X7.25
N50 G03 X-7.25 Y7.25 Z0.375 I-7.25 J0
N60 G03 X0 Y0 Z1.5 I0 J-8
N70 G03 X-7.25 Y-7.25 Z0.375 I0 J-7.25
N80 G00 G40 X7.25 Y-0.75
N90 G90 G00 Z30

Program above will be using same size of thread mill like previous one. i want to know what is the different between this two program..which program will be better for doing the thread size hole??

It makes little difference which program you use, both programs will work. In the one above, you have programmed to the true coordinates of the part, and in this case you MUST use cutter radius compensation and register the radius of the cutter under the offset number being used in your program. In your program example you have omitted the cutter radius offset argument. Accordingly, any previously used cutter radius argumnet that is active will be used with possible disaterous results. What you should have is as follows:

N40 G41 G01 X7.25 D01
where the radius of the tool being used is registered in the Offset Registry Number 01.

When the program has been created as above, where the true coordinates of the part are programmed, you will vary the value registered in the associated offset either side of the actual radius of the cutter, depending on whther the hole is too large or too small.

When the program is created as per your previous example, where the radius of the tool has been compensated for within the program code, and where cutter radius compensation is used via the control, the value for the associated offset will be varied either side of Zero, again depending on whether the size of the feature is too large or too small.

Regards,

Bill

[qinaide2]

N10 G54 G90 G00 X… Y… Z2 S3745 T01 M03
N20 G91 G00 Z-14
N30 G01 Y0.75 F2247(Contour) F576(Centre point)
N40 G41 G01 X7.25 D01
N50 G03 X-7.25 Y7.25 Z0.375 I-7.25 J0
N60 G03 X0 Y0 Z1.5 I0 J-8
N70 G03 X-7.25 Y-7.25 Z0.375 I0 J-7.25
N80 G00 G40 X7.25 Y-0.75
N90 G00 Z-2.25
N100 G01 Y0.75 F2247(Contour) F576 (Centre point)
N110 G41 G01 X7.25 D02
N120 G03 X-7.25 Y7.25 Z0.375 I-7.25 J0
N130 G03 X0 Y0 Z1.5 I0 J-8
N140 G03 X-7.25 Y-7.25 Z0.375 I0 J-7.25
N150 G00 G40 X7.25 Y-0.75
N160 G90 Z2




From above program, if i want to use two pass for thread milling process, is it possible that i put two Cutter compensation geometry offset register number (D) in one program?? Means that first pass i need to do roughing process then the D01 i set tool offset diameter is 6.00mm and D02 is for finishing process so i set the tool offset diameter is 5.9mm. anyone can tell me the true answer??Thanks!!

[Alf0412]

Yes, you can use multiple cutter comps within a single tool.