How do I include a probing routine?

[Bill H]

I'm running a Haas mill with a Renishaw probe.  I've got a batch of parts to run and need to locate a hole at the midpoint of their Y dimension.  The Y dimension varies, however, and is +/- 0.03 from its nominal value.  The Haas can a canned probing cycle (Web Y Axis) that will probe the part and assign the midpoint to any of the work offset registers.  I'd like to incorprate this routine into my program.  How do I do this?

[djstedman]

Several methods..

 

Method 1: Manually enter NC code into the editor after you post your code..

 

Method 2: Use a manual entry to include the cycle so that it posts with the rest of your code.

 

Method 3: Make a modified post that allows you to use custom drill cycles as probing routines (I think this has an example in the posts forum)

 

Method 4: Talk to your reseller about getting the probing addon for Mastercam.

 

I prefer option 2, its easy and flexible and costs nothing in time and effort..

[EX-wccprogrammer]

The easiest way is to specify the command line as a manual entry, posted as code.

[htm01]

the haas can add it to your program, its 1 of the options to add to program or you can create the probing as a program and use as a sub-routine

[Bill H]

Does anyone have the code that I would include in the program?

[EX-wccprogrammer]

You have an existing macro routine that you use?  When you use MDI to use the macro, that is the same information that you put into the manual entry.

[EX-wccprogrammer]

For my Haas with the Renishaw Easyset macro, the instructions are:

(EASYSET HAAS)

G65 P9023 A, XorYorD, Z, S

(A MUST ALWAYS HAVE A DECIMAL POINT AFTER THE NUMBER)

A1. INSIDE DIAMETER, D=APPROX DIAMETER OF ID 
A2. OUTSIDE DIAMETER, D=APPROX DIAMETER OF OD, Z=INCREAMENTAL Z MOVE (ALWAYS Z-)
A3. INSIDE XorY CENTER FIND (X or Y POCKET), XorY =APPROXIMATE SIZE OF POCKET 
A4. OUTSIDE XorY CENTER FIND (X or Y WEB), XorY=APPROXIMATE SIZE OF WEB, Z=INCREAMENTAL Z MOVE (ALWAYS Z-)
(A1. THROUGH A4. ARE FOR CENTER FIND)
(A1. AND A2. WILL SET X AND Y AT THE SAME TIME)
(A3. AND A4. WILL ONLY SET XorY. CANNOT HAVE X AND Y IN THE SAME CALL LINE)
(IN CENTER FIND Z IS ONLY INCLUDED IF DOING OD OR WEB)
(EXAMPLE OF OD MEASURE: G65 P98023 A2. D1. Z-0.5 S54.)

A5. X+ EDGE FIND
A6. X- EDGE FIND
A7. Y+ EDGE FIND
A8. Y- EDGE FIND
(EXAMPLE OF X+ EDGE FIND: G65 P9023 A5. X0. S55.)

A9. Z SURFACE FIND
(EXAMPLE OF Z SURFACE FIND: G65 P9023 A9. Z0. S56.)


S54.=G54                                S101.=G154 P1
S55.=G55                                S102.=G154 P2
S56.=G56                                S103.=G154 P3
S57.=G57                                S104.=G154 P4
S58.=G58                                ....
S59.=G59                                S400.=G54.1 P300

[Craig-B]

what type of probe operation are you trying to do? I sure that we can help you if you can provide more info.

[htm01]

when you go to haas probe quick code on the machine it prompts you for MDI, add to program or create program.

you would have to add your tool change and move the probe to position, that's why I mentioned putting it in a sub-routine

[rsbeadle]

I used to run a Mori that used the easy-set program. All you need is the code "G65 P9023 A3. Y(hole dia.) Z(check depth) S54. (for G54Y)".

 

That will call the probe out and run the routine. You will have to establish the X,Y,Z location of the hole to check before you call the G65 line. Also on the Mori, the Z depth was an incremental distance from the current machine position before the G65 call. So, if the line before the call is "G00 G90 G54 X0. Y0. Z1." and the call line is "G65 P9023 A3. Y.375 Z-1.5 S54." the probe would go to X0,Y0, Z1 then drop to Z-.5 and do a Y axis center find on the 3/8" hole and then retract to Z1. and continue the rest of the program.

 

I personally would use the A1. routine and replace the Y with a D for the hole diameter. If the X location is too far off the probe might not give you an accurate number. Also you can edit the 9023 program to get more or less starting clearance distance if the hole location being off causes you problems.

 

Good Luck. I hope this helps.

[Reece L Gibson]

Might look into productivity plus, pretty seamless....

Worked first time thru when the Renishaw guy was in town.

Pretty easy to set-up too.

[Machineguy]

Bill,

 

Here you go.

 

G00 G40 G80 G91 G28 Z0

G103 P1 (LIMIT BLOCK LOOK-AHEAD TO 1 LINE)

T24 M06 (SPINDLE PROBE)

G65 P9832 (TURN PROBE ON)

G43 H24 (TOOL HEIGHT CALLOUT)

G00 G90 G54 X0 Y0 (CENTER OF BORE TO CHECK OR SET)

G65 P9810 Z1. F200. (PROTECTED Z MOVE TO 1.0" ABOVE THE PART)

G65 P9810 G01 Z-.3 F50. (LOCATION INSIDE THE BORE WHERE YOU WANT TO HIT . CHANGE TO Z.3 FOR Y-WEB !!!! )

G65 P9023 A1. D2. S54. (PROBE BORE MACRO PROGRAM SET G54 D= DIA) 

G65 P9833 (TURN PROBE OFF)

G00 G91 G28 Z0

G103 P0 (ENABLE FULL BLOCK LOOK-AHEAD)

(CONTINUE ON WITH YOUR PROGRAM HERE)

 

The above is for locating the bore on a Haas.

You paste this just below the % and the part # at the beginning of the program.

This is set up for T24 H24 as the probe. Change as required.

 

Run your probe routines first to set the Work offsets for the part, then change the following:

 

Change the G1 line to Z.3 to stay above the part.

 

Change the P9023 line  to : G65 P9023 A4 Y1. Z-0.5 S54 to do a Y-web

 

This is a y-web, (A4), 1.0 outside dim (y1.). It will go down z-.5" on the outside to take the hits. The S54 is the Work Offset you want it to go to. (That should = what the program is using.)

 

This is for the renishaw probe on a Haas.

 

I have a VM-3 with all the bells and whistles. I use this all the time in a lot of production jobs.

 

 

Machine guy

 

Run slow the first time so you see how it works.

[Jorgeva]

Hello, am kind o new to the probe, i have a part that i need to probe, i copy the codes on MDI and i have it:

 

T10M6

GOG90G54X.Y.

G43H10Z.25

G65P9023A4.Y1.815Z-.9S54.

To locate the the center of the part on X and than i have a to locate Y edge but I'm been getting a alarm probe failure, in other occasions I've been successful on touching on X or. Y. And can u please help me on G103 and G65P9810 when to use,  if can help me writing an example program. 

 

 

[JoshC]

I have been diving more and more into probing with mastercams producitivity plus lately on our Haas Vf2 with next gen controller and its working great, its really easy to use. Here is how you use mastercam producitivity+ to probe a y-axis web. https://fastechincorporated-my.sharepoint.com/:v:/g/personal/joshc_fastechinc_net/EYRLO68typpPvXdPL9C3V78BmU7kEFVmHV8ZTbbJKwXzqw?e=t1F6WN

there is so much you can do with Prod+ and probes in general, i have been doing a bunch of reporting (DPRNT) lately and that is fun/cool stuff.

Another option is if you setup the Y-axis probing cycle on the machine through the controllers built in probing cycles you can output that data to a file or flash drive, then in mastercam you can use that cycle that you pulled from the machine controller by manually pasting the G-code into your mastercam file using the manual entry toolpath. Haas's Tip of the day youtube channel has a video on how to do this and a few other very good probing videos so if you have not watched the haas tip of the day videos on probing i would suggest starting there.

[medaq]

On 9/2/2014 at 9:52 AM, Bill H said:

Does anyone have the code that I would include in the program?

Use manual entry tool path in the 2d toolpath section.