Fanuc MACROs for Haimer 3D sensor automation

[rx8pilot]

I am new-ish to Fanuc controls after spending the past 13 years owning/using Haas machines with Renishaw probes. My new job has only non-probe-equipped Doosan machines from about 2005-2008 with typical Fanuc controls from that era. The senior machinist is very good, but very old school and totally content with edge finders and indicators for setup. While it eventually works - it is sloooooow. Far slower than what I am accustomed to.

I ordered a Haimer 3D taster which I expect will be a nice step up from edge finders, but still hoping for more. The next step is looking to develop or modify some macros that will help with common locating tasks like bores, center of block, center of slot, Z offset from table, etc.

I found this old thread that was interesting....
https://www.practicalmachinist.com/vb/cnc-machining/using-haimer-3d-something-like-probing-macros-possible-322662/

I am reasonably well versed in MACRO programming, but I don't use them every day. Is it practical to have a solution that allows me to, for example, set an X- edge and a X+ edge and have an automatic calculation of the center? Not sure if I can manually jog the machine while it is executing a MACRO.

Am I dreaming or do I need to simply do all the work with a calculator and manually type in the resulting offset?

 

[angelw]

I am new-ish to Fanuc controls after spending the past 13 years owning/using Haas machines with Renishaw probes. My new job has only non-probe-equipped Doosan machines from about 2005-2008 with typical Fanuc controls from that era. The senior machinist is very good, but very old school and totally content with edge finders and indicators for setup. While it eventually works - it is sloooooow. Far slower than what I am accustomed to.

I ordered a Haimer 3D taster which I expect will be a nice step up from edge finders, but still hoping for more. The next step is looking to develop or modify some macros that will help with common locating tasks like bores, center of block, center of slot, Z offset from table, etc.

I found this old thread that was interesting....
https://www.practicalmachinist.com/vb/cnc-machining/using-haimer-3d-something-like-probing-macros-possible-322662/

I am reasonably well versed in MACRO programming, but I don't use them every day. Is it practical to have a solution that allows me to, for example, set an X- edge and a X+ edge and have an automatic calculation of the center? Not sure if I can manually jog the machine while it is executing a MACRO.

Am I dreaming or do I need to simply do all the work with a calculator and manually type in the resulting offset?

Hello rx8pilot,
Yes, its all possible. The touch is made in a Manual Mode (normally via Hand-wheel) and no Macro Statement is actually operating during the manual move. For example, to get the centre coordinate between parallel sides, in its simplest form, proceed as follow:

1. Select Hand-wheel mode and move the Haimer to touch off one side.

2. Select Auto Mode to execute your Measure Program and press Cycle Start to store the current position; an M00 would follow the Macro Statement. #3006=1 (OPERATOR MESSAGE) can be used instead of M00. #3006 is Compulsory Stop and Display Message function. Not all Fanuc Controls are equipped with this functions. in which case use M00 to halt the program. In PRODE's example from the link in your Post, the inclusion of G53 is not required as there is no motion when Position System Variables are read and the values stored and #3006 will prevent Buffering in any regard.

3. Select Hand-wheel mode and move the Haimer to touch the other side.

4. Select Auto Mode to execute the next part of your Measure Program and press Cycle Start to store the current position of the second side and to calculate the centre point. In this case it will simply be the average of the two values recorded.

Whatever can be done with an Automated Probe System can be done without the Automated moves. The only difference is that the touch off moves will be carried out in Manual Mode.

Regards,

Bill

 

[rx8pilot]

Bill -

Thank you very much for the response. This is all good news!

I have two questions that I have not been able to find answers:
1. What do you mean by 'auto-mode'? Is that the same as 'MEM' mode on Doosan machines?
2. Is there a MACRO call that will allow user input? The goal is to prompt/ask the user what feature types and what offset that they want to use and the MACRO would do the rest.
[In HAAS world, this is M109, but not sure if there is an equivalent on real Fanuc controls]

Looking forward to trying this out when my Haimer arrives. It could also be potentially useful to do the offset +/- with a traditional edge finder.

 

[angelw]

Bill -

Thank you very much for the response. This is all good news!

I have two questions that I have not been able to find answers:
1. What do you mean by 'auto-mode'? Is that the same as 'MEM' mode on Doosan machines?

Hello rx8pilot,
Yes.

2. Is there a MACRO call that will allow user input? The goal is to prompt/ask the user what feature types and what offset that they want to use and the MACRO would do the rest.
[In HAAS world, this is M109, but not sure if there is an equivalent on real Fanuc controls]

Looking forward to trying this out when my Haimer arrives. It could also be potentially useful to do the offset +/- with a traditional edge finder.

You could do something like the following:
#1=0 (INITIALIZE INPUT TRY COUNTER)
N10 #3006=130 (INPUT 1 to 10 IN #130) (Numbers 1 to 10 relates to function required)
IF[[#130 EQ #0]OR[#130 LT 1]OR[#130 GT 10]]GOTO900 (ERROR TRAP FOR INVALID INPUT)
#2=[9000 + #130]
G65 P#2 (CALL MACRO FOR REQUIRED FUNCTION)
--------
--------
--------
N900
#3006=1 (INVALID INPUT)
#1=#1+1
IF[#1EQ3]GOTO901 (MAX INPUT TRY EXCEEDED]
GOTO10
N901
#3000=1 (MAX INPUT TRY EXCEEDED]
M99

 

[rx8pilot]

That is an interesting solution -
So the user needs to navigate to the variable page and adjust the #130 and press cycle start?

Not quite as slick as M109 taking direct user input - but not too bad. At least that will allow the user to pick what they want from a list and the macro will deal with the details automatically.

I never knew the control would allow manual jogging while in #3006 STOP condition - that is nice.

Thanks again for sharing. I am hopeful that I can streamline the process of setting offsets as much as practical. The Renishaw system REALLY spoiled me with speed, accuracy, and the variety of measurements that I could take automatically.

 

[CNC Hacker]

I thought I had written a macro along the lines of what you were asking, and checking my notes I actually linked to a thread where AngelW posted a handy macro for finding the center of a bore with an indicator or edge finder.

See post #10
Macros for setting fixture work offsets