Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

HAAS Rigid Tapping Code


Code_Breaker
 Share

Recommended Posts

( TOOL 17  -  5/8-11 TAPRH )
(TAPS 5/8-11 HOLES)
N4320M906T17
N4325G00G17G90X-2.0428Y11.8883Z0.W0.
N4330M01
N4335S100M03
N4340G43W2.H17M08
N4345M05
N4350S100M29
N4355G98G84X-2.0428Y11.8883W-2.75R1.F9.0909
N4360X5.3351Y10.8185
N4365X10.6752Y5.6165
N4370X11.9377Y-1.7309
N4375X8.6404Y-8.4171
N4380X2.0428Y-11.8883
N4385X-5.3351Y-10.8185
N4390X-10.6752Y-5.6165
N4395X-11.9377Y1.7309
N4400X-8.6404Y8.4171
N4405G80
N4410G80G49W0.
N4415M01
N4420M30
%

Link to comment
Share on other sites

This is mine.

(TAP)
(T4|6-32 ROLLFORM TAP|H4|D4)
G20
G0G17G40G49G80G90
(T4|6-32 ROLLFORM TAP|H4|D4)
T4M6
G0G90G54X.175Y-.4S450M3
G43H4Z.1
M8
G99G84Z-.45R.1F14.0625
X1.1
X3.875
X2.765Y-1.45
X1.085Y-1.545
X1.185Y-2.84
X2.0526Y-2.8878
X3.25Y-2.875
X3.875Y-2.84
Y-4.6
X2.345Y-4.59
X.175Y-4.6
Y-3.22
G80
M09
M5
G91G28Z0.
G28Y0.
M30
%

The feed is the pitch times the RPM. (In this example).

Link to comment
Share on other sites

This is what I am getting:

(1/2-13 TAPRH)
N6000
T6 M6
G0 G90 G54 X-4.625 Y2.075 S1200 M3
G43 H6 Z6.
M8
Z1.
G95 (feed per revolution)
M29 S1200
G98 G84 Z-1.5 R.3 F.0769
Y.075
Y-1.725
G80
Z6.
M5
G91 G28 Z0. M9
G28 X0. Y0.
M30
%

 

Feed Rate equals Pitch (ie. 13TPI = F.0769; 20TPI=.0500...{1/pitch])

G95 tells the Control that Feed is based on Revolution, regardless of RPM. Allows the Operator to increase/decrease RPM without changing the PITCH. Otherwise, both FEED and RPM must be changed proportionally (inviting Operator's Error).

 

This is the way it works for FANUC Controls. I wanted to know how it works on a HAAS without testing it. I don't want to TEST until I am fairly sure of the Outcome.

Don Dawson

Corona, CA

 

 

Link to comment
Share on other sites
2 hours ago, mkd said:

haas' don't take g95 period. (mills)

g84 must be calculated feed rate for whatever rpm you choose

no m29 either

100% G95 works on Haas mills, but ive found an issue on some software versions where certian rounded pitch past 4 places machine freezes, but same pitch calculated in G94 works fine.

Non issue in my mill but ive run into the issue in other software versions.

Link to comment
Share on other sites
1 hour ago, Codeworx said:

100% G95 works on Haas mills, but ive found an issue on some software versions where certian rounded pitch past 4 places machine freezes, but same pitch calculated in G94 works fine.

Non issue in my mill but ive run into the issue in other software versions.

Please. Tell us more about G95.😁

I forgive you, but I'm still gonna make fun, just this once🧐

IMG_20191121_192539.jpg

Link to comment
Share on other sites

If its an old dinosaur machine from the 90's I don't believe g95 works but on anything newer it does. I have our post set to output g95 so the guys can change rpm at machine without having to calculate the feed rate. Also have post modified to allow for peck tapping.

 

  • Like 1
Link to comment
Share on other sites

from Haas website

 

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...