Fadal RIgid Tapping Problems

Hi Folks,

I have a new-to-me Fadal VMC15 that I'm getting running. It is mostly working, but I'm having trouble with rigid tapping. When it is in the rigid tap cycle (G84.1), the spindle motor oscillates instead of turning smoothly, and the load meter pegs (which isn't surprising given the motor is changing direction quickly and frequently). When I run a non-rigid tapping cycle (G84) it runs as expected.

The machine has a Yaskawa G7 drive that has a sticker on the front with Fadal P/N: INV-0083. I probed the encoder wires at the 9 pin connector just outside of the drive, and the signal looks correct to me. A bit of noise, but it seems reasonable to me (but perhaps that is the problem).

Mechanically, everything seems to be tight.

Any thoughts on what would cause this behaviour?

Here is the code I was running:

Which format are you in?

I think that depending on which format you are in the gcode for tapping changes.

Here is a sample I pulled from a program



Your F number could be the issue, In the code above F300.1 represents a spindle speed of 300 rpm in low range (.1) rather than a feedrate.

The lines below are both preparatory for rigid tapping on fadals, if I remeber correctly they were pulled directly from one of the manuals

G0 G90 S.1 M5 G80 M90
G84.2

F should be the RPM. The thread pitch is Q.

G84.1 Right Hand Rigid Tapping

G84.1 G99 R0+.1 Z-1.2 F2000.2 Q.05 X-.50 Y-.35 (Format 1)

The code you have looks like it would be for non-rigid tapping. But the manual shows this:

G84 Right Hand Tapping
N3 G84 G99 R0+.1 Z-1.2 F550.2 Q.05 X-.50 Y-.35 (Format 1)

Format 2 looks like what you're using, or trying to use:

********
Format 2
The feed rate must be calculated by the programmer. These cycles use the F
word as feed rate and do not use the Q word. The F word in the cycle indicates
the calculated feed rate.
*******

Tapping Cycles

The fixed cycle used for tapping is depends on which tapping attachment is
being used. The cycles and examples given here have been approved by the
tapping attachment manufacture specified.

General Tapping Rules

Ramping:
Program a G8 (No Ramps) for the tap operation. This allows the tool to feed at
a constant rate in and out of the hole.

Clearance:
The rapid plane (R0 Plane) should be at least .4 above the hole to be tapped.
This insures that the tap fully retracts prior to movement to the next position.

Spindle Speed:
When using the G74 and G84 cycles, the spindle should be programmed for
the high gear range. This will provide better spindle reversal for tapping. This is
accomplished by programming a “.2" at the end of the S word or F word. For
example, S1000.2 or F1000.2 sets the spindle speed at 1000 rpm in the high
gear range.

Feed Rate:
The feed rate is determined by the thread lead and spindle RPM. The thread
lead is calculated as 1 divided by the number of threads per inch. When using
G74 and G84, the feed rates may be programmed differently for Format 1 and
Format 2. When using the G85 cycle for tapping, the feed rate must be
calculated by the programmer for Format 1 or Format 2. When using rigid
tapping in Format 2 and the F word requires decimal entries, use at least three
place accuracy.

Format 1
The feed rate is calculated by the control. These cycles are programmed using
the F word for RPM and the Q word for thread lead. G74, G75 and G84
calculate the feed rate as the RPM times the thread lead. These cycles
automatically use 100 percent of this calculation for the feed rate into the hole
and 105 percent for the feed rate out of the hole. The P word may be used to
increase or decrease the feed rate out of the hole. Use a positive P to increase
and a negative P to decrease the feed rate out of the hole.

Feed Rate Calculation
The feed rate programmed should use 100 percent of the optimum feed rate.
The optimum feed rate is the RPM times the thread lead.
EXAMPLE: 1/4-20 Tap at 2000 RPM
Feed rate = (1 / threads per inch) * RPM
= (1 / 20) * 2000
= .05 * 2000
= 100.

The machine says it is in format 2, so I wrote the code according to the manual for format 2. I haven't tried format 1.

Some of the manual pages say to use low range for 750 and below (S750.1), and high range above that, so I tried with S1000.2. I went and tried both higher and lower spindle speeds. I tried S100.1, and S4000.2. Both seemed to run about the same as S1000.2

But my VMC15 only has one mechanical speed, so I don't know if it makes any different. It does appear to have the Delta/Wye contactors, so perhaps that is what it is using a speed range.

Does the machine actually have rigid tapping? There should be a yes/no option for rigid tapping somewhere in the parameters you could check.

If it does have rigid tapping, you could try using the g84.2 command (prepare for rigid tap). If memory serves correct this should orient the spindle for tapping. It will perform up to three full rotations looking for a reference mark on the encoder (or something similar to that). If there is a problem with the spindle encoder it should throw a c axis fault when you run it.

From the fadal manual

In depth info on rigid tapping in this manual

https://www.fadalcnc.com/media/pdf/tech_docs_1/User_Manual/Sect_4_Fixed_Cycles.pdf

***********************************

EDIT:

Also, have you retried using code in the same format as posted earlier? Just took a look at your original post and it looks like you didn't include an R plane. The cycle probably cant start if it doesn't have a start/return plane defined.

Fadals are pretty finicky with tapping codes, you need to be by the book or you will get unexpected axis faults.

Directly from the manual posted above, examples of code for rigid tapping in either format.

Note on your machine, you cant use s.2. I don't know how it will act if you do. You could try using s.1 or try excluding the (s.x) all together and see what it does.

EXAMPLE:
N52 G0 G90 S.2 M5 G80 M90 Do not turn the spindle on!
N53 G84.2
N54 H1 M7 Z.4
N55 G84.1 G99 R0+.4 Z-.3 F2000.2 Q.05 X0 Y0
N56 X1.
N57 G80

EXAMPLE:
N52 G0 G90 S2000.2 M5 G80 M90 Do not turn the spindle on!
N53 G84.2
N54 H1 M7 Z.4
N55 G84.1 G99 R0+.4 Z-.3 S2000.2 F100. X0 Y0 100% feed calculation here
N56 X1.
N57 G80

Click to expand...

I added the R0 codes to all the fixed cycle lines, and there wasn't a change. I haven't tried to switch to format 1. I'll maybe try that tomorrow.

As far as I can see, this is a rigid tap machine. The option sticker inside the pendant says rigid tap, the spindle encoder is connected to the drive, and it is connected to the control card in the control cabinet. The parameters also have the rigid tap option selected.

The drive that is in there doesn't match with the Yaskawa model drive shown in the pdf manuals. Such as this one: https://www.fadalcnc.com/media/pdf/tech_docs_1/Maintenance_Manual/Spindle_Drive_and_Motor.pdf

I wonder if the person that installed that drive perhaps didn't configure it correctly. The guy I bought the mill from said he never uses tapping cycles, and he wasn't the one that installed the drive, so he doesn't know anything about it.

Looking through that spindle manual again, I see that on page 293 there are some parameters listed for the control for rigid tapping. My numbers are different. I guess I need to figure out which software version I have, and whether they are inch or metric screws and then maybe try the numbers from the manual.

Did you include the "+" in the R0 line? I burned up half a day trying to get it working on my machine just to find out that the plus is required. If possible I would try and use the exact code from the manual (tweaking just the (.2) line, since we know you have a single speed gearbox) just to see if it will work. If its a drive/encoder/parameter problem I would expect a fault to pop up.

This is from the manual for the format you are using, just run it dry with no tool and see if it does anything

G0 G90 S2000.2 M5 G80 M90 (Do not turn the spindle on!)
G84.2
H1 M7 Z.4
G84.1 G99 R0+.4 Z-.3 S2000.2 F100. X0 Y0 (100% feed calculation here)
X1.
G80

I got back to working on the Fadal today. I seem to have the rigid tapping working. I tested it with an M6 tap in thin, soft aluminum. That's weak enough that if there is a sync error it will strip the aluminum rather than break the tap. It tapped fine there.

I had the + sign after the R0 when I added that to my code. I tried the code you posted (but with the H1 and M7 removed), and it behaved the same. I also ran the code from the "Rigid Tap Testing Procedure" I found at fadalcnc.com https://www.fadalcnc.com/media/pdf/Old_Service_Files/Rigid%20Tapping/Rigid%20Tapping%20Test%20Procedure.pdf It also behaved the same.

The test procedure had some parameter values, and they were different than what was in my machine. Particularly the Gain was set to 100, and the test procedure shows 130. So I tried that, with no change. Then I looked at the parameter listing on the sticker inside the pendant, and the gain was 68. I tried that, and it significantly cleaned up the behaviour air tapping. The test code doesn't have .1 or .2 on the S-word. I tried it at S750.1 and it seemed better, and then S750.2, and it seems slightly better than S750.1.

At that point I went to a modified version of my program at the top, ran it at S750.2, and put the R0 codes it, and it produced clean threads in the thin aluminum. Next to run it with a bigger tap in steel.