DaveR

Haas lathe thread issue G76

17 posts in this topic

Just got a haas lathe it stops dead at the G76 line and will go no further, spindle keeps turning.

 

I'm using the stock X6 haas SL lathe post

 

I dont have any idea what is wrong.

 

The book says it needs a q value with no decimal I have that, it's posting a "0" that is supposed to be the thread start angle.

 

The P value should be an option (single edge cutting) for multi start threads no idea why I get "P010029"?

This is what I get when I post it (standard 1/4-20 thread supposed to be 5 passes)

 

 

G00 T0707

M8

G97 S1500 M3

G00 G54 X.45 Z.4107

G76 P010029 Q0 R0.

G76 X.1905 Z-.29 P297 Q117 R0. F.05

M9

G28 U0. W0. M5

T0700

M01

 

example in the book is G76 X Z K.042 (thread height) D0.0115 ( first pass depth) F.0714

 

any idea what I should change in the post to get this running?

Share this post


Link to post
Share on other sites

N1 G20

(#######################################)

N4600

N2 T4646

N3 G97 S200 M03

N4 G0 G54 X.45 Z.2082

N5 G76 X.1905 Z-1. Q29000 K.0297 D.01 F.05 A59

N6 G28 U0. W0. M05

N7 M30

 

.25-20 thread with my defaults. This will work on an SL or TL haas lathe

Share this post


Link to post
Share on other sites

If I delete the first 76 line it throws an error "no I, j, k" something...

 

 

That format that adage caga posted will run.

 

Anyone know how to change the post so it will output the g76 lines that way?

Share this post


Link to post
Share on other sites

Dave,

 

I should have a few minutes today.

 

If you want to send me a z2g and a sample of what you need, I should be able to get you fixed up.

Share this post


Link to post
Share on other sites

Think your using new style G76 threading.

Need to change switch to old 6T style for Haas.

Should output just one line then.

George.

Share this post


Link to post
Share on other sites

J, thanks a lot.

 

I will send you the z2g this evening I'm at work right now.

 

Appreciate the help.

Share this post


Link to post
Share on other sites

you may need to adjust a few areas. this is a modified mplmaster post i use for HAAS's new DS machine as well as TL, SL & ST lathes. since HAAS's canned cycles do not use the anticipated pulloff option in mastercam for threading, i have a prompt built into my post using the M23/M24. if you look on your control, you will see a default setting for the distance. just didnt want you to get confused when you see the M23 below :

 

# --------------------------------------------------------------------------

# Format statements - n=nonmodal, l=leading, t=trailing, i=inc, d=delta

# --------------------------------------------------------------------------

#Default english/metric position format statements

fs2 1 0.7 0.6 #Decimal, absolute, 7 place, default for initialize (:)

fs2 2 0.4 0.3 #Decimal, absolute, 4/3 place

fs2 3 0.4 0.3d #Decimal, delta, 4/3 place

#Common format statements

fs2 4 1 0 1 0 #Integer, not leading

 

 

 

# Thread output

# --------------------------------------------------------------------------

##fmt P 16 thddepth$ #Thread height absolute

fmt K 2 thddepth$ #Thread height absolute

##fmt Q 16 thdfirst$ #First depth cut in thread

fmt D 2 thdfirst$ #First depth cut in thread

fmt Q 16 thdlast$ #Last depth cut in thread

fmt R 2 thdfinish{:content:}nbsp; #G76 thread finish allowance

fmt R 3 thdrdlt #Thread R delta G92 and G76

fmt U 3 thd_dirx #Incremental X move for G76 mult starts

fmt W 3 thd_dirz #Incremental Z move for G76 mult starts

fmt P 5 nspring$ #Number of spring cuts

fmt 5 thdpull #G76 thread pull off

fmt 5 thdang #G76 threading angle

 

 

pg76nstart #G76 threading, for multiple starts

if old_new_sw = zero, pg76old

else, pg76new

nstart_cnt = nstart_cnt + one

if nstarts$ <> one & nstart_cnt <> nstarts$,

pbld, n$, *sgcode, thd_dirx, thd_dirz, e$

 

pg76old #G76 threading old style

[

pbld, n$, "M23", e$

cham = 0

pbld, n$, *sthdgcode, pfxout, pfzout, *thddepth$,

*thdfirst$, pffr, e$

]

else,

pbld, n$, *sthdgcode, pfxout, pfzout, *thddepth$,

*thdfirst$, pffr, e$

 

pg76new #G76 threading new style

if cham = 1, pbld, n$, "M23", e$

pbld, n$, *sthdgcode, pfxout, pfzout, *thddepth$, *thdfirst$, pffr, e$

Share this post


Link to post
Share on other sites

I need to say this a bit slower maybe.

Machine axis switches Threading type old or new.

new type will post-

 

G76 P----- Q---- R----

G76 X-- Z-- P-- Q-- R-- F--

 

Old type will post-

G76 X-- Z-- I-- K-- D-- A-- F--

Geo

Share this post


Link to post
Share on other sites

you dont need to say it slower george. your point is a good one and is right, but for a HAAS lathe, please see the difference i was making in the below post callouts. for a HAAS, you will need to make the edits seen below even with changing the setting to use "old style":

 

stock post - too much info that is not needed for the haas cycle:

 

pg76old #G76 threading old style

pbld, n$, *sthdgcode, pfxout, pfzout, *thdrdlt, *thddepth$, *thdfirst$, *thdang, pffr, e$

 

for a haas

 

pbld, n$, *sthdgcode, pfxout, pfzout, *thddepth$, *thdfirst$, pffr, e$

Share this post


Link to post
Share on other sites

Sorry Trevor !

Did not intend it to come across like that I really should have said offering a better discription.

Understand fully what you are sayinging ,I was just offering a quick fix to get Dav eup and running.

George.

Share this post


Link to post
Share on other sites

its all good george. i think we have both given dave some good info to get him going.

Share this post


Link to post
Share on other sites

How do you switch from new to old?

 

is it this line...

 

1=yes - Set based on Axis Combination in MD

old_new_sw : 1 #Switch old (6T), new (0T+) cycle formats, 0=old, 1=new

 

I did find the codes listed by Trevor.

 

I'm using the stock haas SL post in X6

 

Oh man this is always an adventure.

 

I appreciate all of your help.

 

I really screwed something up as after some modifications it was not even posting out G76, then I reloaded the backed up post and tried again and it seems to be doing what it should I will have to try and run the code through the machine later this evening and see. I must have fat fingered something. Not the first time. :D

Share this post


Link to post
Share on other sites

shoot me an email if you need to. even though the stock posts says it is for a haas, trust me, you still will need some edits. this is one of the main reasons i always use an inhouse post. anyway, send me an email. i will send you what i have and know that produces good code.

Share this post


Link to post
Share on other sites

Hi Dave

Yes you got it there,just change the 1 to a 0

and it will post old style code as you require.

The other thing is the thread chamfer and angle are set on the control

with setting 95/96 on the machine.use M23/24 to turn it on or off.

it is modal so you only need to insert a M23 into the code line once and it will stay on.

The Q will only post out if you are using multi start threads.

I am sure that Trevor can sort it out for you.(He's my best mate now that I have managed to insult him!)

But it wont hurt to try and understand how to do it as you can bet,sometime down the line you

will need to do it all again !

George

Share this post


Link to post
Share on other sites

dave...the setup i sent you is for X5. you will need to update it to X6, if you are still running X6.

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!


Register a new account

Sign in

Already have an account? Sign in here.


Sign In Now

  • 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