So at work, we have this Fanuc robodrill alpha t10c that boss impulse bought at auction.
I am familiar with making programs and running our other CNC machines ( trumpf punches and flow waterjet) but I've never used a CNC mill before but I managed to get it working...
I cleaned out all the mess out of it, took out the parts we won't be using.
The machine comes with a Fanuc 16 M controller and a Renishaw MP12 probe system.
I have figured out how to input programs into the machine, figured out the drip-feed to the controller the only thing that I can't figure out is probing.
I'd like to do simple things with the probe like edge finding and Z height
There are programs in the machine related to the probe but I cannot seem to figure them out
A mp12 is fairly old. but the ONLY thing you are losing out to on a newer one is the length. They work the same.
step one. go to renishaw.com and get a user manual for inspection plus. An older one if possible because it has changed some on recent years.
step two read that
step 2.5 see if you have programs # 8890 9724 9833 these are key. See what is in the comments for copyright years- this should be step1 but whatever
step three buy a pack of 9volts and replace the probe battery
step 3.5 run macro 9832 to turn the probe on. holding it in your hand but letting the receiver see it, deflect the stylus and watch the skip input. like X4.7 or something. there will be a walkthrough of testing G31 in the book
4- try to calibrate the probe. you will need a master tool and a ring gage. I like to mount the ring gage on a new install, on a bar hanging out of a vise or in some fashion that if something goes wrong i wont munch the probe.
older software requires you to run several calibration routines like length- ball dia & offset and finally vector if you have vector routines. Newer insp plus has a one step cal.
I am checking through Renishaw website for the manuals (hard website to navigate through!)
attached is a photo of all the programs i have that seem to be related to the probe. All of them are protected programs and i cant seem to find a way to send them to the pc to check them.
It seems that I'm missing program 8890 and macro 9832
I mistyped its 8898, maybe you dont have it in an older install. But, you are not showing any 8000 series programs in that pic
9832 is probe on though, I dont know how you dont have that.maybe thats what 9023 is.Or is that the toolchange macro?
someone made programs 9100 and 9101 those are not original so they conceivably could have made their own start routine?
you will have to change PWE and then parameter 3202.4 (NE9) to be able to view them or punch them out. Be careful you dont delete or change anything.
3202.0 for 8000 series
What probe do you have? there is no MP12 I was thinking mp9
here are some documents
Have you seen the Mi12? What you are needing to determine is how they were switching on the probe. Since the normal macro is missing. That probe only supports optical on. Being a Robodrill I doubt they could have used auto on successfully. so you need to determine what Mcodes they used for probe start. If you look at 9833 and search for "M" you will find the off code, not M98 keep looking. The on code will be the counterpart to it most likely (ie: M114 - M115) you can test this in mdi. if you then search in all the other programs in the machine for that Mcode and can not find it. Then you dont have it.
here is a probing routine like you would put inside your part programs
A note on Robodrills. Dont give it a G49 with your + tool length active. If I remember right it moves in -Z direction at rapid. If it wont toolchange without G49 put it after G0G91G28Z0.
(SET Z SURF NO STEP SHIFT AND BOSS ORIGIN 1 PART)
T20 M06
G00 G54 G90 A90.
G43 H20 (PROBE LENGTH OFFSET CALL)
G65 P9832 (PROBE ON)
G65 P9810 X-4. Y0. F100. (PROTECTED POSITIONING)
G65 P9810 Z0.5 F100. (PROTECTED POSITIONING)
G65 P9810 Z0.2 F10. (PROTECTED POSITIONING)
G65 P9811 Z0. S1 (TOUCH Z SURF AND SET G54 Z)
G65 P9810 Z.5 F100.
G65 P9810 X0. Y0. F100.
G65 P9814 D10.0 Z-.4 S1. (PROBE BOSS SET G54 OMIT Z FOR BORE)
G65 P9810 Z2. F100. (PROTECTED POSITIONING)
G65 P9833 (PROBE OFF)
G00 G28 G91 Z0.
G90
M01
Does this machine have a pallet changer?
You have macro 9901 labeled as pallet start change. That is the number Renishaw uses for the new GoProbe routine which is really handy.
your boy TerryBerry posted a video that should be informative for you. He explains a little more in depth about Inspection Plus Macros in a part program.
when he talks about IO, for you it looks way different but functions the same.
I haven't had time to touch the machine in the last couple of months and only got back to it now!
I still haven't found the probe on program
I have downloaded all the programs off the machine now if you want to check through them i can upload them somewhere
Fanuc 16 M Probing
Reply with Quote
