[juniormachinist]

we have a 96 fadal VMC4020 with a cnc 88HS controller and are using mastercam x6 for solidworks
we have recently began using tapping and have had limited success. we discovered that the feed rate in is correct but the feed rate out is 5.5% faster so therefore its breaking the taps.

[Superman]

we discovered that the feed rate in is correct but the feed rate out is 5.5% faster so therefore its breaking the taps.

???? It's right...but it's wrong

- Have you defined the tool correctly, put in the correct thread pitch ? ( pitch is what defines feedrate, not the Z plungerate. depends on your general output settings at the top of the post---- )
- Does your NC file output the feed per rev.... or feed per minute ( G95/G94 ) ?

- Is the RPM and feed/pitch the same in the Mastercam session & the NC file ?
( if not, the post may have a feedrate compensation for use with compression type toolholders, instead of a rigid tap holder )
- attach your post ....change .pst to .txt so that it will upload to the zone

plus
put up some NC code for a M6 x 1.0p tap that is posted straight from Mastercam
- & also the edited NC file that has been proven to work on the machine

[juniormachinist]

our pitch is right. all the numbers in mastercam match whats in the nc code. it outputs g95
i have attached the same file we were using which is a 8x1.25mm as well as a 6x1mm file

[Superman]

Your post & tool settings appear to give correct NC code for rigid tapping
- the problem would seem to be your machine, as it is NOT following the NC code
I would start looking at the machine's parameters for tapping, there may be an incorrect feed adjustment in the parameters to the G84 cycle ( or the M29 component function )
- it may have set-up for use with the compression type holders, normally they adjust to approx. 95% of the pitch (not 105.5% ), so, as you tap, the tool is pulled out further ( if the tap breaks, the holder springs back to it's correct length, or, for when the spindle reverses, it allows for non-synchronisation between the spindle & the Z axis )

I worked on a fanuc, and assumed it had rigid tapping, found that the threads were stripping / stretching.
- Problem was when the spindle slowed down to a stop, and reversed, the feed had actually stopped dead during that slow-down & reversal.
- Fix was to only use a floating type tap holders, you can get the straight shank holders that use an ER11-ER16 collet to hold the smaller taps, it does mount into a sidelock or a larger ER32 toolholder. Also got a ER32 holder to be able to use the larger taps. There is a wide range to choose from. sample

[cadcam]

This is the format you really need for that control.

Sample of my Post for the fadal I have used on that control for close to 10 years.

TA,1
%
O0001 ( TEST REV: )
( TEST )
(MACHINE TOOL : FADAL FORMAT 1 )
(DATE - 15-09-13 )
(TIME - 13:02 )
(*)
(MATERIAL: )
(STOCK SIZE: X = 0. Y = 0. Z = 0. )
(HOME POSTION COORIDNATES ARE THE FOLLOWING)
(X= )
(Y= )
(Z= TOP OF PART)
(*)
( TOOL - 199 DIA. - .25 1/4-20 TAPRH )
(*)
(USING FIXTURE OFFSETS: E1 )
(*)
G0 G17 G40 G49 G80 G90
T199 M6 ( TOOL - 199 1/4-20 TAPRH DIA. OFF. - 199 LEN. - 199 DIA. - .25 )
G0 G90 S300.2 M5 E1 X-1.4147 Y-.0557
G43 H199 Z1. M8
G84.2
G98 G84.1 X-1.4147 Y-.0557 Z-.5 Q.1 R.1 F300.2
X-.2882 Y.6386
X.9562 Y.0426
X.8449 Y-1.1298
G80
M5
G0 G49 Z0.0 M9
G0 X0. Y0. E0
M0
M2
( BECAUSE YOU HAVE A CHOICE - )
( THANK YOU FOR CHOOSING PRECISION PROGRAMMING )
%

[nikolaiownz]

I think we used M29 before tapping on our old fanuc machines..

[juniormachinist]

Does changing the format mean that it chamges

- - - Updated - - -

Does changing the format mean that it changes weather its imperial or metric