[YTMBOSS]

I have a Johnford SV 45 with a Fanuc 18-M control. Just recently downloaded the parameters and now I can't get it to run a program. It gives me an 011 no feed rate alarm at my first G00 rapid move. We havn't ran this machine, we just set it in shop as we bought it used. Also with the swing arm tool changer on it, should there be a table that tells you what tool is in what pocket? I can't find a table for it. And I can't find a tool table to give it cutter offset size for using cutter comp.

[sinha_nsit]

One question at a time please!

G00 does not require a feedrate. You must have used some other code needing feedrate. Specify it and the problem would go.

[YTMBOSS]

I know G00 doesn't require a feed rate, but the machine will not do the move. It gives me a 011 alarm (No feedrate). I'm stumped.

[sinha_nsit]

The block next to G00 might be requiring feedrate.
Post your program, without editing.

[YTMBOSS]

Here is the first few lines of my program. It alarms out on the G00 Z2.0 line. Is there a parameter that you have to set to tell the machine how fast to rapid?


%

G90
G54
M06 T1 (1/4 EMILL)
M03 S2600
G43 H1 D1
G00 Z2.0
X0. Y0.
Z.1
X1.Y1.
G01Z-0.125F1.5
Y0.76F6.0 G41
G03Y1.24I0.J0.24
Y0.76I0.J-0.24
G01Y1. G40
Z-0.25F1.5

[YTMBOSS]

Also how do you change the D values for cutter comp in this control? I really appreciate any help.

[FrankCNC]

D & H cannot use the same offset number one will overwrite the other in the offset table, so if using tool 20 use offset 20 for H and offset 120 for D, most post processors are set up that way to make D+10 or 100 of the tool offset number.
Cutter offsets use the same table as tool length offsets just different offset numbers as stated above.
Try placing the D offset code in the line with the G41 (which I believe is normal programming practice) and not in the same line with the H length offset code.

I've found some of the Fanuc T controllers need an F code somewhere near the start of the program before a G1, but haven't come across that with any Fanuc M controllers yet.

Regards,
Frank.

[sinha_nsit]

Execute G91 G00 Z1.0; in MDI mode and look for any error message. The tool should move up by 1.0 inch (in inch mode) at rapid rate.

[rward1961]

If I was writing the program it would look like this and yes you cannot have the H & D on the same line

G0 G17 G40 G80 G90 G98
G90 G54
T1 M6
GOO X1. Y1. S2600 M3
G43 H1 Z2.
Z.1
G01 Z-0.125 F1.5
G41 Y0.76 F6. D21
G03 Y1.2 I0. J0.24
Y0.76 I0. J-0.24
G01 Y1. G40
Z-0.25 F1.5

The only thing you do and I dont is I dont cancle the cutter comp just to move in the Z
I leave it on so I dont have to call It up again. Good Luck.

[YTMBOSS]

Thanks for all the help. I played around with program yesterday and got the startup codes right. I had to move the G0 towards the top, I guess so it knew it was all ready in rapid mode before I gave it G0 X Y line to rapid home. I'm used to running Haas, Fadal, and different conversational controls. This is my first dealings with an actual Fanuc control. I also didn't know about the different offsets. My machine has 0-99. I'm used to having a tool table with length and radius offset side by side using H1 and D1 for T1. I did a search yesterday afternoon and figured out how to use the Fanuc offsets. I have 1-24 as length and 31-54 as cutter offset.

Also I have always programmed with an H and D on my G43 line. I just do that so I know where it is and I can quickly tell if I'm using cutter comp or not. I know the Haas control will accept this. I did change that for this Fanuc control to two different lines. Your right it won't accept them on the same line.

I really appreciate the help. I was about to pull my hair out with this machine.

[stevo1]

D & H cannot use the same offset number one will overwrite the other in the offset table, so if using tool 20 use offset 20 for H and offset 120 for D, most post processors are set up that way to make D+10 or 100 of the tool offset number.
Cutter offsets use the same table as tool length offsets just different offset numbers as stated above.
Try placing the D offset code in the line with the G41 (which I believe is normal programming practice) and not in the same line with the H length offset code.

I've found some of the Fanuc T controllers need an F code somewhere near the start of the program before a G1, but haven't come across that with any Fanuc M controllers yet.

Regards,
Frank.

This will depend on what offset memory that you have. You can use the same value for D and for H. One does not override the other. If you have the offset memory for length and for geometry then you do not need to specify a different number for one or the other.

Look in your offset page and if you have a column for length and another for geometry you can put the length value in (Z) and the geometry (radius of tool) in the other all under the same tool number. You can then proceed to use G43H1, G41D1.

Stevo

[FrankCNC]

Stevo1 is right, I forgot about Memory B and Memory C as our machines only have Memory A with one page for all offsets and I got use to programming with different offsets for H and D.

If you haven't already got it you should get the book 'Fanuc CNC Custom Macro' by 'Peter Smid'

[stevo1]

If you haven't already got it you should get the book 'Fanuc CNC Custom Macro' by 'Peter Smid'

This is also a very good book for beginners.
http://www.mhprofessional.com/produc...sbn=0071713328

Stevo

[sinha_nsit]

This book is written with reference to the newer 0i series controls. So, it does not describe compensation memory type A and B. Only type C is described.