Sign in to follow this  
AMCNitro

Indicating bore with Probe on Haas

Recommended Posts

I mat have to cut some molded parts on a mill for a second opp.  Its a round part with a bore.  Bosses want to have each part indicated, I know how to do that.  Problem I'm seeing is that the Indicate Bore routine on the Haas doesn't ask for a depth, you have to take it to the depth and then run the program.  

How would I go about doing that?  Write the coordinates BEFORE the probe program ?

Share this post


Link to post
Share on other sites
13 minutes ago, AMCNitro said:

I mat have to cut some molded parts on a mill for a second opp.  Its a round part with a bore.  Bosses want to have each part indicated, I know how to do that.  Problem I'm seeing is that the Indicate Bore routine on the Haas doesn't ask for a depth, you have to take it to the depth and then run the program.  

How would I go about doing that?  Write the coordinates BEFORE the probe program ?

you set the probe up as a tool and just program it to the center of the bore and to the z depth that you want then call the probe bore sub

Share this post


Link to post
Share on other sites

This is a sub I call to...it'll look something like this...though mine is not for a Haas, the premise will be the same

(******************)
(*PROBING ROUTINES*)
(******************)
N8901(PROBE 1 ROUTINE - FUSION LASER BENCH)
(PROBE 1 POSITIONS AFTER INITIAL OFFSETS SET)
()
(PROBE POSITION 1)
()
Z1.
G65P9809T1X.155Y-.1467F100.
G65P9809T1Z.1F100.
G65P9810Z-.565F100.  (This goes down inside the bore)
G65P9814D.22S#19(X,Y OFFSET)     (This calls the ID cycle)
G65P9810Z.25F100.
G65P9810X.625Y-.1467F100.
G65P9811Z-.125S#19(Z OFFSET)
G65P9810Z.1F100.
G28Z1.
()
(END PROBE 1)
M99

  • Like 4

Share this post


Link to post
Share on other sites

Below is for a Haas, you will want to use the inspection plus macros and not use the Haas GUI  

You can find the inspection plus manual here:

https://service.haascnc.com/sites/default/files/Locked/2/Renishaw_Programming_Manual_H_2000_6222_0A_B.PDF


M06 T24 (PROBE)
G00 G90 G154 P1 X0. Y0. 
G43 H24 Z3. 
G65 P9832 (TURN ON PROBE) 
G65 P9810 Z0.2 F100. (PROTECTED MOVE) 

G65 P9810 Z-0.5 F100. (PROTECTED MOVE)
(S1=G54,S2=G55....G154P10=S154.10) 

G65 P9814 D1.75 S154.01 (BORE CENTER FIND) 


G65 P9810 Z0.2 (PROTECTED MOVE)

G65 P9833 (TURN OFF PROBE) 


G00 G53  Z0. 
(T10) 

(START MACHINING) 

  • Like 3

Share this post


Link to post
Share on other sites
On 11/19/2021 at 7:56 AM, civiceg said:

Below is for a Haas, you will want to use the inspection plus macros and not use the Haas GUI  

You can find the inspection plus manual here:

https://service.haascnc.com/sites/default/files/Locked/2/Renishaw_Programming_Manual_H_2000_6222_0A_B.PDF


M06 T24 (PROBE)
G00 G90 G154 P1 X0. Y0. 
G43 H24 Z3. 
G65 P9832 (TURN ON PROBE) 
G65 P9810 Z0.2 F100. (PROTECTED MOVE) 

G65 P9810 Z-0.5 F100. (PROTECTED MOVE)
(S1=G54,S2=G55....G154P10=S154.10) 

G65 P9814 D1.75 S154.01 (BORE CENTER FIND) 


G65 P9810 Z0.2 (PROTECTED MOVE)

G65 P9833 (TURN OFF PROBE) 


G00 G53  Z0. 
(T10) 

(START MACHINING) 

I did it right from the machine control, I had to add some lines of code, but it was very easy.  Just saw what the machine wanted to do, and from there I figured out what it needed from me.

Thanks for this though.  And thanks to everyone that offered help

  • Like 1

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
Sign in to follow this  

  • 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