Fanuc Tapping Issues

[Robo_Tech]

I'm working with a 2009 Mag Fadal 4020 FX with Fanuc control and programming it with CamWorks.

It is Format 1, but I had my post processor changed to format 2 just to double check if that would work.

This is my first time trying rigid tapping on it, and with all the errors I've been getting I'm starting to wonder if it even has rigid tapping. Every person I've talked to assures me a CNC as new as ours has to have it. My first question before getting into all the errors I've had is just, what is the parameter for rigid tapping so I can just check to see if I have it? I have been told it's not a common variation of Fadal as it has a 15,000 rpm spindle, so who knows maybe it actually doesn't have it.

This is my program, I drilled a bunch of holes to size in a row on the x-axis. This is the second half just tapping.


(OPERATION NAME: Tap Test)
(1/4-20 UNF TAP)
N1 T16 M06
N2 G20
N3 G00
N4 G17
N5 G49
N6 G90
N7 G5.1 Q1 R5
N8 G00 G54 X-3.5 Y0 M90
N9 G43 H16 Z1. M08
N10 G84.1 G98 R.3 Z-.65 S306 F15.
N11 X-3.
N12 X-2.5
N13 X-2.
N14 X-1.5
N15 X-1.
N16 X-.5
N17 X0
N18 X.5
N19 X1.
N20 X1.5
N21 X2.
N22 X2.5
N23 X3.
N24 X3.5
N25 G80 Z1. M09
N26 M05
N27 G00 G91 G28 Z0
N28 G00 G91 G28 Y0
N29 G00 G90 G59 X0. Y0. Z0.
N30 M02
%

Going single block mode it randomly fails on lines N1-N6 different every time and gives me the error saying Illegal Address Input. Line N3 it might get past first three tries then fail the fourth. It almost always fails on one of those first lines with that error. If it does make it past those first few lines, it fails on line N10 saying illegal use of a decimal place.

I also have mastercam at my disposal, I haven't tried programming it with that yet to see if there is any difference.

Any help much appreciated, thanks.

 

[706jim]

Couldn't you put all of those codes into a single block? Maybe that would help.

G20G90G00G17G49 whatever

 

[6061Mike]

I am not familiar with the Fadal, but every other machine I have ran uses a G84, not G84.1, also have you tried using a G93 and the ptich for feed? I know the Matsurra I run now has to have a G93 and the feed in pitch for the rigid tapping to work.
T10 M6 (10-32 tap)
G0 G90 G54 X-.7735 Y1.5211 S480 M3
G43 H10 Z5. M8 T11
G93
G98 G84 Z-.36 R.2 F.0313
X-2.3622 Y0.
X-.7735 Y-1.5211
G80
G94
M9
M5
G91 G28 Z0.
M01

 

[HYPERTUNE]

Why you running g5.1 for a tapping cycle? Try changing it to Q0.

 

[angelw]

You haven't specified the model of the Fanuc Control; that would be helpful. As you state the control is Fanuc, there is no Format 1 or 2, as is the case with a Fadal Control. Fadal and HASS do this to emulate a Fanuc control if required.

1. Its not good form to be specifying G20 on anything but the first block. The G codes in blocks N1 through N6 are from different "G" Code Groups; accordingly, as 706jim pointed out, these codes can be combined in a single block. Make this the first block of the program.

2. Rigid Tapping can't be programmed in Simple High-Precision Contour Control

3. Take a look at Parameter 5200. If set to 0, an "M" code specified prior to the G84 block is used to invoke Rigid Tapping. If set to 1, Rigid Tapping is invoked by G84 alone. The disadvantage of this is that Non-Rigid Tapping can't be used if for some reason you wanted to.

4. If Parameter 5200 is set to 0, look to see what value is set in Parameter 5210. The setting range of 5210 is 0 to 255, and specifies the "M" code used to invoke Rigid Tapping. If set to "0", the "M" code will be M29 by default.

5. G84.1 will be causing the error in the N10 block.

6. Your Feed Rate in Tapping is wrong. With 306 RPM the Feed Rate should have been F15.3. The wrong Feed Rate is a real killer when Rigid Tapping; its lucky that you didn't actually get the tapping cycle to work.

The following program code should work if parameter 5200 and 5210 are both set to "0"

(OPERATION NAME: Tap Test)
(1/4-20 UNF TAP)
N1 G00 G17 G20 G17 G40 G49 G90 G94 (This would be the very first block of your program - not used before each tool)
G91 G28 Z0.0
G28 Y0.0
T16 M06
G5.1 Q0
G90 G00 G54 X-3.5 Y0 M90 (M90? may be specific to your machine)
G43 Z1.0 H16 M08
G95 (Use Feed Per Rev - If you have to change the Spindle Speed, you don't have to worry about recalculating the Feed in Rigid Tapping)
M29 S306
G98 G84 Z-0.65 R.3 F0.05
X-3.
X-2.5
X-2.
X-1.5
X-1.
X-.5
X0
X.5
X1.
X1.5
X2.
X2.5
X3.
X3.5
G80 M09 (Z1. is not required in this block. The tool would have finished at the Initial Level Z1.0 set by G43 Z1.0 H16 M08)
G94 M05 (Reinstate Feed Per Minute)
G91 G28 Z0.0 (G00 is not required with G28)
G28 Y0.0 (G91 is Modal - its not required in this block)

N29 G00 G90 G59 X0. Y0. Z0. (Rather than this block, and the two previous blocks, you could use the following)

G90 G53 Z0.0
G53 X_ _ Y_ _ (Where X_ _ Y_ _ equals the position of the X0. Y0. G59 Work Shift)
M30 (Use M30 not M02)
%

Regards,

Bill

 

[Robo_Tech]

Thanks for the replies so far, I've got the CNC tied up today but I plan to try out some of the suggestions on monday.

The reason for separating all the G-codes at the start was it kept stopping there over and over saying illegal address and I just wanted to pin-point if a specific code was doing it.

The G5.1 I forgot was in there, post processor does it automatically. I design and CNC molds for plastic parts and without the G5.1 we were having issues.

The feed rate was wrong because I took the decimal out when it threw the illegal decimal code alarm. I thought that might have been it. Camworks auto scales feed rate and spindle speed if you change one independent of the other and I had an issue in the past where I forgot to uncheck that option. I didn't notice it wanted to do a feed rate of 70.189654 or some really long decimal and the cnc didn't like it. I figured it would break the tap if it actually worked, but I still would have been happy for that little bit of success.

I don't have the user manual here on me, but above the screen says "GE Fanuc Series 18i-MB" I assume that is the model of fanuc control?

Looking at the parameters:





Hoping pics show up, but it looks as though I do have rigid tapping and it's M29.

I have a program wrote up that looks a lot better now and have a good feeling it will work. Looking at some of the things that have been pointed out though it seems I need to do some changes to my post processor.

 

[angelw]

Thanks for the replies so far, I've got the CNC tied up today but I plan to try out some of the suggestions on monday.

The reason for separating all the G-codes at the start was it kept stopping there over and over saying illegal address and I just wanted to pin-point if a specific code was doing it.

The G5.1 I forgot was in there, post processor does it automatically. I design and CNC molds for plastic parts and without the G5.1 we were having issues.

The feed rate was wrong because I took the decimal out when it threw the illegal decimal code alarm. I thought that might have been it. Camworks auto scales feed rate and spindle speed if you change one independent of the other and I had an issue in the past where I forgot to uncheck that option. I didn't notice it wanted to do a feed rate of 70.189654 or some really long decimal and the cnc didn't like it. I figured it would break the tap if it actually worked, but I still would have been happy for that little bit of success.

I don't have the user manual here on me, but above the screen says "GE Fanuc Series 18i-MB" I assume that is the model of fanuc control?

Looking at the parameters:

View attachment 102746View attachment 102747View attachment 102748



Hoping pics show up, but it looks as though I do have rigid tapping and it's M29.

I have a program wrote up that looks a lot better now and have a good feeling it will work. Looking at some of the things that have been pointed out though it seems I need to do some changes to my post processor.

If you write a test program along the lines of my example it will work. Parameter 5210 shows that you need to use M29 to invoke Rigid Tapping. This Parameter is normally left as "0" if the default M29 is used, but having it set to 29 is OK.

One problem is that you're using a Fadal Post Processor with Camworks; G84.1 is Rigid Tapping for a Fadal Control. Make sure you use a Fanuc Post and it will solve a lot of other potential problems you will encounter if using a Fadal Post Processor with a Fanuc control.

Regards,

Bill

 

[Robo_Tech]

I get down to the tapping cycle part, and the spindle spins for a brief second. I get two alarms.

742 - Rigid Tap Alarm: LSI Overflow <---no clue what that means
9081 SPN 1 :S-Spindle Error (AL-081)

The second one is an error that shows up on the drive as well.

 

[Robo_Tech]

On a tip from a co-worker I tried to adjust the servo loop gain but the parameters are write protected. Is there a way around that?

 

[Vancbiker]

Don't eff with the parameters yet. Post the code you were trying to run.

 

[NAST555]

I get a lot of flack for the way that I program but I leave aaaaalllll of that crap out in the starting blocks of my programs because I have a dedicated sub that does it all for me. I even use my CAM post to output it this way.

Now my fanuc Rigid tapping would look like this

O0001
P8003 M98 (MY SUB)
T1 M6
G00 G54 X-3.5 Y0.0 S306 M3
G43 H1 Z10.0 M8
M29 S306 (On my Oi I need this but on my OM I don't)
G84 G98 Z-0.65 R0.3 F15.3 (I never use feed per rev on my Fanucs only on my Mitsubishi but each to their own)
X-3.
X-2.5
X-2.
X-1.5
X-1.
X-.5
X0
X.5
X1.
X1.5
X2.
X2.5
X3.
X3.5
G80
P8002 M98 (TOOL CHANGE SUB)

08003 looks like this but may vary between machines

O8003
(DO NOT DELETE )
(ZERO Z AND Y AXIS)
M5
M9
G91 G40 G17 G64 G80 G98 G28 Z0.0
G49 H0
G28 Y0.0
G90 M1
M99

And 8002 like this which also varies a bit between machines

O8002
(DO NOT DELETE )
(ZERO Z AXIS)
M9
G91 G80 G40 G64 G17 G98 G28 Z0.0 M5
G49 H0
G90 M1
M99

 

[HYPERTUNE]

Maybe try it without the S306 M3.
I think I had an alarm on my Mori with Oi when I tried that, and now only use M29 S____

 

[angelw]

Maybe try it without the S306 M3.
I think I had an alarm on my Mori with Oi when I tried that, and now only use M29 S____

You're right with dropping the M03. Although many say they have no problem starting the spindle in this manner, a greater number do have issues if the spindle is running when Rigid Tapping Mode is invoked. The correct method of starting the spindle is with the code that invokes Rigid Tapping.

Regards,

Bill

 

[NAST555]

Maybe try it without the S306 M3.
I think I had an alarm on my Mori with Oi when I tried that, and now only use M29 S____

Oh ok good to know if I ever run into that problem. I never have and it has always worked for me this way but at least if it does ever happen I know where to look.