FANUC Parameters Topic

[CNCAppsJames]

A LOT of people ask why can't my FANUC controlled machine do this, that or the other? The answer isn't always straight forward because FANUC controls are some of the most versatile and powerful controls on the market and depending on the series, can run upwards of 128 Axes. And because of that, the lions share of the responsibility falls on the builder/integrator to configure the machine appropriately.

All that said, you do have a lot behavior available to you to change to better suite your liking.

*LEGAL* Your machine is your machine. Any parameters you change are YOUR responsibility. Consult the FANUC Parameter Book for the series of your control to confirm the accuracy of the information below. The majority of the parameters below are accurate for FANUC 0i-D series and forward and FANUC 30i Series controls. Again, Consult the FANUC Parameter Book for the series of your control to confirm the accuracy of the information below. If you see things like WSEC or TWP, or Dataserver metioned, those are specific to that hardware or function. If you do not have tthose functions present it is best to leave them as they are.

So without further adieu;
#929 = 1 *FTP Data in is always ASCII - This should be the default setting IMNSHO but that's a discussion for another day.

#1300.1 = 1 *Alarm not output for over-travel while in jog handle mode. This should also be the default setting IMNSHO but that's a discussion for yet another day.
#1301.7 = 0 * Stroke pre-check off. There's room for discussion here IMHO
#1401.1 =1 *No dog-leg rapids. All moves are linearly interpolated (axes arrive at the same time). This should be the default setting IMNSHO but that's a discussion for... the days are adding up here
#1401.4 = 1 *Rapid Stops when Feed Override is at 0% Just because I'm ambidextrous doesn't mean I want to worry about rubbing my belly and patting my head. One knob stops everything. I prefer that.
#1434 = Max Feed at Handle. Be cautious here. I don't recommend changing this but it can be done safely in many cases.

#3032 = Max number of digits for T-Code (Up to . Consult your Machine Tool Builder if this will cause problems with tool manager software.

#3101.1 = 1 *When the screen or mode is changed, key-in buffer are not cleared.

#3201.2 = Attempting to load a program who's number/name already exists 0=Alarm, 1=Overwrite if not protected (REP)
#3202 (NE8 and NE9) Protect O8000's and O9000's.

MDI Program Behavior - Like Haas
#3203.6 = 0 *Do Not Delete MDI  Program after execution
#3203.7 = 0 *MDI Program not cleared by reset
#3204.6 = 1 *Do not Automatically erase MDI program.

#3207.5 = 1 *Display #500-#999 MACRO Variable Names
7
#3233.1 = 1 *Folders in the Dataserver can be set as the foreground and background folder.

#3301.7 = 1 *Screen Capture to active I/I Channel Enable  - Hold Shift for 5 sec.

#5004.2 - 1 = Diameter, 0 = Radius for Cutter Compensation.

#5013 = MAX Wear Offset Value
#5014 = MAX INC Wear Offset Input (INP.+ Method)

#5148 (HMC/VMC Boring in Z-Axis - Q Shift Axis)
Z 1 = Shift X+
  -1 = Shift X-
  2 = Shift Y+
  -2 = Shift Y-
ALL other axes = 0

#5200.5 = 1 *High Speed style peck tap
#5202.0 = 1 *Spindle Orient prior to rigid tap (reboot req.)
#5213 = Rigid Tap Backoff Dist.

#5400.5 = 1 *Rotates MACRO Variables to be read in active coordinate system - For Probing while TWP active. (Renishaw InspectionPlus Software MUST support this - generally speaking if your renishaw software had O9744 and the following section, you should have this active;
(FCS*TO*WCS*CALC)
(EDIT ROTARY AXIS CONFIGURATION)
#1=0(MCS FOR THE A AXIS - = 0 IF NO A AXIS)
#2=0(MCS FOR THE B AXIS - = 0 IF NO B AXIS)
#3=0(MCS FOR THE C AXIS - = 0 IF NO C AXIS)
Your tilt axis shoudl have #5024 and your rotary acix shoudl have #5025 in the FCS TO WCS CALC settings)

#6001.3 = 1 Output all MACRO Variables on punch
#6001.6 = 1 #100-#199 not cleared on reset.
#6005.0 = 1 In Sub Program Call use Sequence Number
#6008.3 = 1  On reset, POPEN is closed
#6019.0 = 1 Output all variables as decimal number

#6019.3 = 0 File Format of output file =PRNTnnnn.DAT
#6019.7 = 1 File Format of output file =PRNTnnnn.DAT is memorized

#11200.3 = 1 system variable #5061- #5080 Skip Coordinates can be read - for probing with WSEC active

#11350.1=1 Current section of program only displayed, not look ahead section (Requires Reboot)

#11351.6=1 Parameter Group Names Displayed

#14853.4 = 1 - Able to transfer from memory card to Dataserver. (Reboot Req.) (CONSULT MACHINE TOOL BUILDER BEFORE CHANGE)

#14854.6 = 1 Program Input/Output is enabled during Background Editing

Function - G49 No Move
#5006.6 = 1 (TOS)
#11260.0 = 1 (TCS)
#11400.2 = 1 (TOP)

Function -
M198 to Flash Card
#138.7  = 1 (MNC)
#3404.2 = 1 (SBP)
#6030    = 198 M-Code to execute ext. device subprogram call

This is by no means an exhaustive list. Merely the most common requests over the last 15 or so years.

Bits are as follows;

7 6 5 4 3 2 1 0

Bit 7 all the way left, and bit 0 is all the way right.

If you're not absolutely sure what you're doing, don't. Seek the help of your local machine tool dealer, or if they are no help or non existent, ask here. Someone will know the answer.

HTH

[Jeff]

#3203.6 = 0 *Do Not Delete MDI  Program after execution

This is how it is on our Brother, I kinda like it this way.

[CNCAppsJames]

This is how it is on our Brother, I kinda like it this way.

So in a number of our regions we sell Haas. Operators have gromw accustomed to having the MDI more like a notepad, having all the MDI stuff there for the selecting. On the iHMI interface controls (latest) you can still do that, or you have the ability to save MDI functions for later recall, or you can create MDI stuff for import and future recall. Perhaps I'll add a sample of that code.

[JParis]

MDI Program Behavior - Like Haas

Hahahahahahahaha 

I was with you right up until then...

Then I was laughing uncontrollably   

LIke a Haas 

I nearly snarfed my water

[CNCAppsJames]

Hahahahahahahaha 

I was with you right up until then...

Then I was laughing uncontrollably   

LIke a Haas 

I nearly snarfed my water

That's MY frame of reference for that behavior so... I mean I guess I could have said Siemens 840DI and there'd be like maybe 2 other people in here than could relate. Or I could say what I said, and probably 75% of the people in here would know the reference.

[Tryon]

James,

What is the danger with this parameter change?


#14853.4 = 1 - Able to transfer from memory card to Dataserver. (Reboot Req.) (CONSULT MACHINE TOOL BUILDER BEFORE CHANGE)

Thanks

[CNCAppsJames]

James,

What is the danger with this parameter change?


#14853.4 = 1 - Able to transfer from memory card to Dataserver. (Reboot Req.) (CONSULT MACHINE TOOL BUILDER BEFORE CHANGE)

Thanks

On machines with a Panel I or iHMI interface it messes with the operation of the control.

[Tryon]

Anyone know if it's possible to get a +input button on the macro screen?

[CNCAppsJames]

Anyone know if it's possible to get a +input button on the macro screen?

I've never seen +INPUT there... it would be handy though. I'll see if there. is. I'm not hopeful though.