Tapping Issues on our V2XT

[5S Dude]

Using this tapping program, we are getting a spindle overload alarm on our V2XT when tapping more than 8 positions. Is the spindle RPM of 750 too fast? Should I program a M0 and change to low gear to perform tapping?

Thank you so much.

N2 T2 M6 ;(1/4-28 TAPPED HOLES)
S750 M3
G00 X2.1793 Y-.25
Z.1
G84 X2.1793 Y-.25 Z.18 F26.78
G80
G0 Z.1
M22

[axis overtravel]

Originally Posted by 5S Dude Using this tapping program, we are getting a spindle overload alarm on our V2XT when tapping more than 8 positions. Is the spindle RPM of 750 too fast? Should I program a M0 and change to low gear to perform tapping? Thank you so much. N2 T2 M6 ;(1/4-28 TAPPED HOLES) S750 M3 G00 X2.1793 Y-.25 Z.1 G84 X2.1793 Y-.25 Z.18 F26.78 G80 G0 Z.1 M22

i would not have thought 750 rpm too fast for a 1/4 inch tap.
what z depth are you tapping?
check the parameters in your G84 block, i have not done any machining center tapping for a few years but there looks to be something missing, like the clearance height, is it the R word?, and should the Z word be negative -???
if the machine has a low speed range, try changing to it and selecting a spindle speed from there.

good luck

atb

axis

[remsandpets]

Here's my 2c,

First try this with the Z offset with a +2.0 to ensure it will work with your machine.

N2T2M6
S750M3
G00 X2.1793 Y-.25 M08
G43 H2 Z.1
M29
G84Z-.(WHATEVER YOUR Z DETH NEEDS TO BE ENTERED HERE) R.1 F26.7857
G80
G00 Z4. M09
G40 M05
G91 G30 Z0.

This program is from SmartCam and is formatted for Fanuc controls. It is fairly generic and is set for rigid tapping. The M29 locks your spindle rpm to your feed rate. I always carry the feed rate out to 4 place to ensure a smooth tap and less liklyhood of tap breakage due to not having the proper feed. Take your RPM and devide by the pitch of your thread and that gives the feed rate.

Good luck and keep posted if this does not work for you.

Russ Jackson in SW PA


N2 T2 M6 ;(1/4-28 TAPPED HOLES)
S750 M3
G00 X2.1793 Y-.25
Z.1
G84 X2.1793 Y-.25 Z.18 F26.78
G80
G0 Z.1
M22

[Servo Wizard]

5S Dude,

Remove the X & Y addresses from the G80 OpCode line. If your control skips the initial X & Y location then include the initial X & Y addresses on the line following the G80 OpCode line just as you would with any subsequent X & Y addresses.

Servo

[machintek]

The problem is not in the program. The problem is in the design of the machine. The current needed to reverse rotation of the motor puts a strain on the overload. Less spindle reversals per minute is the only solution. Sorry.

George

[5S Dude]

axis overtravel; thank you for the quick response. I currently interpolate a .211Ø x .22 deep blind hole with a 3/16 2-flute center cutting end mill. I chamfer each hole 45° x .015 before sending the ¼-28 three flute high spiral flute flat bottom tap .180 deep. It works like a charm on the parts that have 8 tapped holes in it but when the same process is applied to the part requiring 16 tapped holes my poor Bridgeport gives me the “spindle overload message.” I of course do not want to place undue stress on my baby so I may resort to an articulated-arm stand-alone tapping unit and simply tap the holes manually.

Remsandpets; thank you as well, I do not believe the DX32 control is equipped to process rigid tapping so I’m currently using a spring loaded tension tap holder from Procurier. The tapping process has yet to snap a tap as it simply gives the “spindle overload alarm” and requires a machine shut down and resetting the switches inside the control cabinet.

Servo Wizard; thank you for your valued input as well.

Machintek; thank you for your answer to my dilemma! I do realize the V2XT is more a tool room mill than a full-blown production machining center so no need to be sorry.

This part time hobby has blossomed completely out of control and I am beginning to see the machine limitations now.

In your opinion, is perhaps a larger motor upgrade possible as I need the full length advantage of the V2XT table over say a Haas, Fadel or Hurco type machine. Or should I simply move the tapping process to a Tapmatic equipped articulated arm setups and tap manually?

Thank you all so much for your devotion to this great site!! You all have been very supportive and I hope I can one day return the favor!

[Servo Wizard]

5S Dude,

machintek mentioned over current on spindle reversal. That can be delt with by adding a bit of dwell at final depth and Z retract. That will significantly reduce the current required to reverse the spindle.

Servo

[5S Dude]

Originally Posted by Servo Wizard 5S Dude, machintek mentioned over current on spindle reversal. That can be delt with by adding a bit of dwell at final depth and Z retract. That will significantly reduce the current required to reverse the spindle. Servo

Brilliant possibilities Servo! And it shouldn’t take long to prove this theory out! Thanks a million…

I've noticed on a few Lathe tapping programs some of the programmers prefer to start the tapping cycle .2 off the face of the part and I was wondering if this may have any impact on vertical tapping cycles as well. I will post results as they happen. Thanks again.

[gridley51]

"
I've noticed on a few Lathe tapping programs some of the programmers prefer to start the tapping cycle .2 off the face of the part and I was wondering if this may have any impact on vertical tapping cycles as well."

The reason for starting 0.2 of the face is to allow the axis and spindle time to synchronise.

[TARIQ08]

Hi there,
I am having problems tapping on a cnc mill with fanuc omd control. I am tapping 1/2 bsw thread and hole is just reamed when the tap comes out. my program is as follows: can anyone help
N2 T15
N4 M6
N6 G0 G90 G54 X-1.125 Y1.125
N8 S500 M3
N10 G43 Z0.1 H15 M8
N12 X-1.125 Y1.125
N14 G84 G99 X-1.125 Y1.125 Z-1.25 R0.1 P0 F4.0
N16 X1.125 Y1.125
N18 X1.125 Y-1.125
N20 X-1.125 Y-1.125
N22 G80 Z2.0
N24 M9
N26 G28 G91 Z0
N28 G91 G28 Y0
N30 M30

[5S Dude]

Originally Posted by TARIQ08 Hi there, I am having problems tapping on a cnc mill with fanuc omd control. I am tapping 1/2 bsw thread and hole is just reamed when the tap comes out. my program is as follows: can anyone help N2 T15 N4 M6 N6 G0 G90 G54 X-1.125 Y1.125 N8 S500 M3 N10 G43 Z0.1 H15 M8 N12 X-1.125 Y1.125 N14 G84 G99 X-1.125 Y1.125 Z-1.25 R0.1 P0 F4.0 N16 X1.125 Y1.125 N18 X1.125 Y-1.125 N20 X-1.125 Y-1.125 N22 G80 Z2.0 N24 M9 N26 G28 G91 Z0 N28 G91 G28 Y0 N30 M30

Hi TARIQ08, Try this....

To tap a 1/2 British Standard Whitworth Thread

Data;
1/2ø
12-Threads Per Inch
0.0833-Pitch in Inches
0.3932-Core Diameter

Use a Letter Z (10.5 mm) Drill. Change spindle RPM to S200 and feedrate to F16.6667

Let us know how it comes out!

[KTD1]

I’ve used a V2XT machine for 15 years. Didn’t know you could even start the spindle much less reverse it in the program. Are you using a tapping head that reverses rotation?

The DX32 controller is quite capable of rigid tapping on machines that have servo driven spindles. Use the M28, & M29 codes to toggle it in and out of rigid tap mode.

As a suggestion, have you considered thread milling instead of tapping?