[dieman1968]

I recently switched back from mazak lathe work to mazak mill
work on a new vcn510c. I have ran other mazak mills and never had
a problem with fixed tapping, but since I have been assigned to this
new machine the only way I can tap a hole without breaking a tap
is to use the peck2 cycle witch greatly adds to cycletime. Is there
a parameter from the factory set to something I need to change?.
or do I need to put in a T.P.C. with data? or do I need to stand on
one foot and rub my belly while it runs? Any help or suggestions would be
greatly appreciated.

DIEMAN1968

[mazakguru]

Check param D30 if you make it 0 the tap cycle will go to the depth you program. From factory it it usually 3 which makes the cycle go 3 times thread pitch deeper than programed

[dieman1968]

I WILL CHECK THE PARAMETER D30 THANKS FOR THE HELP. BUT MY
PROBLEM IS NOT ONLY WITH BLIND HOLES. THE JOB I AM WORKING
ON IS A FIXTURE PLATE WITH 37 TAPPED HOLES PER PLATE. MATERIAL
IS STANDARD COLD ROLLED BOILER PLATE. THE PROBLEM IS THE TAP FEEDS IN GREAT BUT THE MACHINE REVERSES SO QUICK AT THE BOTTOM IT
JUST SNAPS THE TAP RIGHT OFF. THE ONLY WORK AROUND i HAVE BEEN ABLE TO COME UP WITH IS TO DRILL .01 OVERSIZE TURN OFF THE COOLANT
AND MANUALLY APPLY TAP LUBRICANT. THIS WORKS BUT I THINK IS
RIDICULUS I SHOULD BE ABLE TO TAP THESE HOLES IN 3 MINUTES BUT
THIS WAY ITS TAKING ME 12 TO 15 DEPENDING ON THE OPERATOR ANY
HELP OR TAP MANUFACTURER OR ANYTHING WOULD BE APPRE4CIATED
THANKS DIEMAN1968

[mazakguru]

Two things, first if you use auto calculate feature in mazatrol best thing I've found is to cut surface speed in half. Second I,ve had my best luck tapping with OSG high helix taps. Good Luck

[stucaruk]

The parameter for # of incomplete threads can get you even with a through hole. I've busted taps untill I realized the tap was driving in an extra 3 complete threads even with a through hole drilled. The tap busted when it reversed to come out... or so I thought. It actually broke just as it finished and the shoulder bound up on the stock.
Try setting the parameter for number of incomplete threads to zero.

If it's a new Matrix control, when you are editing the program, hit the right arrow key and then highlight the TPC key to make a temporay parameter edit. Change the parameter to 0 and hit TPC end. You'll see a blue + sign on the unit number.

Check the pitch of the thread as well. If it's a pipe thread, all the Mazak tables are wrong since they assume British standard pipe threads. Tyr a 1/4" pipe tap and you get a 19 pitch thread rather than the expected 18 pitch for example. It's hard on a standard tap.

Failing that, you don't need to stop the machine to apply a bit of lube. Stick some lube on one corner of the table away from the worst of the coolant splash, use a shiel if you need to. Program the tool to plop into the lube before the tapped hole.

You might grab a refractometer and check the coolant concentration. It never hurts to make sure you have the right drill called as well...

good Luck,

Stu

[sridhartsr]

hi,
auto calculation is working good but in my experince am always maintaning the cutting speed 20. pls try this

[pmarseille]

Do you know if the machine has the SYNC Tapping option?
Just go to Diagnos-->Version-->Option to see if you have it. (assuming you have a 640M controller)

Options that you have are highlighted in black

If you don't have it, you need a tapping holder. Using a rigid holder without the option installed will cause the tap to break for sure.

Pat

[jimiscnc]

on Fusion and matrix, the tell tale sign that you have solid tapping is that, at the start of the hole, the spindle speed starts from 0 RPM and accellerates the RPM in unison with the Z feed.

of course, this takes place in a couple hundred milliseconds and may be hard to see with the naked eye.

if you have floating tap only, then there is no spindle accelleration from zero RPM. it just goes in. stop. reverse. goes out.

If you have matrix with solid tapping, then you can use the recent PECK TAPPING capability in the matrix. I think its one or two hard to understand switches in the tool definition line?

a tip:

most people look at the column heading when mazatrolling. this can be decieving, as these columns can mean something other than the abbreviation that is used in the program unit.

You will be better off longterm if you get in the habit of using the dialog box in the lower right. this is the window where you put your program info in. it usually contains a phrase more applicable to what you're doing than the column headings.

I love Mazatrol!

jim

[peterpan3]

I'm not sur how the Mazatrol is but on my Meldas near the end of the line I have to use ,R then e-# of threads. At the end of the tapping cycle I put in a R, this is a coma .
Don't know if that helps..