Zeroturn fanuc displays "NOT READY"

Any information regarding the Denford ZeroCentre ZeroTurn ZeroBore Fanuc CNC machines

Moderators: Martin, Steve, Mr Magoo

Post Reply
g-speed
Posts: 22
Joined: Thu 02 Nov , 2006 17:49 pm

Zeroturn fanuc displays "NOT READY"

Post by g-speed » Fri 26 Sep , 2008 20:45 pm

I have recently bought a Zeroturn with Fanuc control. On powering it up it wouldn't home and kept giving an axis limit overtravel alarm. On powering it up again I held down the CAN and P buttons as advised and now it gives a "not ready" message at the bottom left of the machine and nothing will move. When the control system was turned on again it showed 0615-08 and PMC:2.17-P. Any ideas?

Martin
CNC Guru
CNC Guru
Posts: 1897
Joined: Fri 24 Feb , 2006 17:09 pm
Location: Brighouse

Post by Martin » Fri 26 Sep , 2008 22:47 pm

Have you tried holding in the "Axis Limit Overide Switch"?

You need to keep it pressed in while you jog the axis away from which ever overtravel switch it is on. the easiest thing is to send it to the Datum position. The switch was normally fitted on the right hand side of the rear electrical box.

User avatar
Lone_Ranger
CNC Expert
CNC Expert
Posts: 220
Joined: Mon 01 Oct , 2007 15:23 pm
Contact:

Post by Lone_Ranger » Sat 27 Sep , 2008 8:33 am

.

If holding down the "Axis Override Button" doesn`t work then the machine had gone too far and over travelled the physical limit switches, to get it back you can switch everything off from the mains and remove the inspection panel/s and then manually wind the X and Z axis away from the limit switches.

Once that is done you need to power up again and you should be able to then use the "Axis Override Button", if you can then using the handwheel move both Axis at least 50mm away from their "Home" position, this is a software limit so that`s why you should move them a long way away, Fanuc systems don`t like to "Home" from close to the home position. I usually move the turret to about halfway along both axis.

When you have moved them away then turn the "Feed Override Switch" down to around 50/60 %, Fanuc doesn`t like to home at full speeds either!!
Then you can press your "Home" "X+" and "Z+" buttons and the machine should first home on the X axis and then do the Z axis.

I have 2 Denford Cyclone Lathes both with Fanuc controls ( 1 is OT "C" and 1 is OT"B") and the above works on both of them whenever I "screw up" and send one over travel!!

Always leave the Lathe at around it`s halfway point in both Axis when not in use and switched off so that you only have to do the "Home" operation when starting up, if you forget and leave it at the "Home" position and try to home it again it will go over travel again so always take note of where the turret is on start up and make sure it`s roughly in the middle of it`s travels before you do the "Home" operation!!

Hope that helps!!

Regards
Rob

:mrgreen: :mrgreen: :mrgreen: :mrgreen: :mrgreen:

g-speed
Posts: 22
Joined: Thu 02 Nov , 2006 17:49 pm

Post by g-speed » Sat 27 Sep , 2008 10:09 am

Thanks for your help. The machine now does something. Next problem!!! When I home the machine the x axis does not read zero! The z axis does read zero and I have cleared all tool offsets and work shift offsets. X did read abot 155mm with a work shift of about 11mm. When I cleared the work shift back to zero it then read 144mm.

User avatar
Lone_Ranger
CNC Expert
CNC Expert
Posts: 220
Joined: Mon 01 Oct , 2007 15:23 pm
Contact:

Post by Lone_Ranger » Sat 27 Sep , 2008 12:52 pm

g-speed wrote:Thanks for your help. The machine now does something. Next problem!!! When I home the machine the x axis does not read zero! The z axis does read zero and I have cleared all tool offsets and work shift offsets. X did read abot 155mm with a work shift of about 11mm. When I cleared the work shift back to zero it then read 144mm.
All depends on how you want to work on your machine as to what you now do with your work shift offsets, there a few ways you can proceed but here is how I have my machines working to suit how I use my CadCAM software and how I like to work. May not be to the liking of all and may not be right to some of the "purists" around but it works for me!!!

I use the face of the chuck as work Zero and have measured the height of the jaws so I know exactly where I am likely to hit something!!
This means in my CadCAM I can set stock and the drawing correctly so it is clear of the chuck.
I put a piece of ground bar in the chuck that I knew the exact diameter of and set my first tool to that in the X axis and set that number plus the rad of the bar as a minus ( It is -38.44mm ) in the X workshift.
Then used a tool setter against the face of the chuck to get the distance from the home position to the chuck face and put that number in as the Z workshift ( It is 201.58mm ).
So now when I first switch on my machine it will show X 0.00 and Z 0.00, after I "Home" my machine it will always show X107.56 and Z201.58 on the position screen and the machine position is shown as "Absolute" X107.56, Z201.58 and "Relative" U107.56, W201.58 and the Machine position as X0.00, Z0.00.
After that all I do is check tools against the same piece of ground bar but any bar you can measure the exact size of will do and use the tool setter off the chuck and put the offsets into the tool offset library.
After that it`s only a matter of calling a tool number and offset number up (eg T0101 or T010101 if using tool nose rad) in the code and presto the right tool will always go to the right place ( That`s the theory anyway and it`s worked so far for me!!! )

Sorry if some of this seems to insult your intelligence but I have no idea what your level of expertise is so I thought I`d just go through what I did with my machines.

After that I modified a couple of Post Processors in my CadCAM software to get the exact code needed for the 2 machines as they do use some different "G" codes for some operations!! (eg One uses G28 for reference and the other uses G50, all good fun!!) Your Denford Manual should have a list of "G" and "M" codes assigned to your particular control.

After having said all that there is a way to have everything actually reading 00.00 on all axis at "Home" position by setting a Parameter in Fanuc to make this happen but unfortunately I have no idea which parameter of the hundreds in there to change or what to set it to anyway!!
You will have to remember that if you do get all axis to show 0.00 at "Home" position then you need to call up your work shift/coordinate position in your program.
I don`t have to set that in my programs.

Boy, that was some "ramble", hope it all made some sort of sense for you!!

Regards
Rob
:mrgreen: :mrgreen: :mrgreen: :mrgreen: :mrgreen:

.

User avatar
Mr Magoo
CNC Guru
CNC Guru
Posts: 301
Joined: Tue 21 Feb , 2006 21:45 pm
Location: Brisbane, Australia

Post by Mr Magoo » Wed 01 Oct , 2008 11:30 am

Just to add... the parameters in the machine were configured when it left the factory so that the x axis displays '0' when the internal tooling 'pots' on the turret are on centreline.

This means that when the X axis is at home, the pots are 144mm (dia) from centreline.

HTH

Post Reply