I've been wondering about this too.
anyone know how to set an 18i-mb to restart the spindle after stopping via opt-stop (m1)... i can't find a parameter (or mtb parameter) for it but all my other machines do it...
I've been wondering about this too.
Insert M03/M04 after M01. Even if optional stop is not being used, M03/M04 would do no harm.
this is a fine solution in some circumstances, but not always
for programs coming from our cam system, the post can easily insert an extra M3/M4 after the M1, but besides being extra code in storage and to send via rs232 every time, its not ideal
but more important than that, if the operator wants to add an M1 somewhere in the program to check the part/tool, there is a great possibility of error if that m3/m4 is forgot... and since all other machines in my shop will restart the spindle and coolant after an m1, i'd rather address the issue on the machine itself
PMC keep relays that are relevant but not the solution (this is a mori seiki nh5000, msg-501 control (fanuc 18i-mb):
K5.5: 1:M01 command does not stop the spindle/coolant
K24.3: 1:When given an M01 command, door is unlocked
thanks for the suggestion
Having a Spindle restart without an M3/M4 is a major safety violation.
Enough that OSHA might own your company, or get your insurance canceled.
If anyone can Insert a M01 they can also add the M03.
Don't be stupid, if an accident happens and they find you modified the machine function its going to come out of someones pocket, and it won't be the insurance company.
well i agree, after a reset or emergency stop, but an m1 is not really the same thing... cycle start is being pressed for pete's sake (same as starting a program from the top, user doesnt have to press an extra spindle button)
not to mention most mtb's would agree with me, as can be seen by the factory behavior of all other machine tool builder's our shop has...
so the Mori Seiki is the one that does not restart the spindle after a cycle start after M1
i also have:
Fanuc (MTB and control, robodrills) 2 models 3 machines
hardinge/bridgeport, 1 model 2 machines
kitamura, 1 machine
chevalier, 1 machine
hwacheon, 1 machine
miyano, 1 machine (lathe)
all of these act the opposite, which is to restart the spindle after a "cycle start" is received while at an opt-stop M1 or any M0
what if the tool was M4/CCW and the operator didn't know the difference or check the status... there's also m5 and m19 to think about if the operator has to actaully hand code this stuff...
or imagine you want a non-hand edited program, but has an m1 after every hole for tap chip clearing or part measuring... the door interlock takes care of all the safety concerns
The program header sets all sorts of condition variables that are often only set once. Usually a shortened sub set of these commands are used for each tool change.
Any time an Autocycle is allowed to be interrupted a potential danger has been created. How much of a danger varies somewhat with the age of the control. A FANUC 0mB behaves differently than a FANUC 0i. After a M01 the machine will continue with the commands on the next line of code, does that line contain enough data to be a safe start point, like after one or more axis was homed.
I believe our Mori Seiki SV50B with MSC 518 (FANUC 18) will resume after a stop if the door switch and mode switches are not disturbed. I honestly am not sure since all programs have all the needed code after any optional stop or conditional alarm stop.
Code is cheap - fill it up. Hardware, material, tools and operators are expensive.
i tend to disagree, the less code the better in most circumstances... especially when it comes to operator's proving out and prototyping parts... in a shop where rarely do parts run in a machine for more than a day or two... so a handful of parts/setups may be done in a day on each machine... the more that can be configured on each machine to make operation identical throughout the shop is proving to be more and more beneficial... standardization
putting the safety code into macros and establishing general safe practices is the only way i can get trained but inexperienced operators to use machines safely and still be dynamic enough to and edit programs or repost as necessary from the cam system...
on most of my fanuc controls (all prior to the 31i) there is no limitation to prevent a program from being started at any point in the program... they did finally add this warning to the 31i i've seen, which is a good error prevention measure... but otherwise transmission errors and operator errors are always a possibility... proper training and procedure definition, and simplifying code and procedures, is working for me better than anything else i've tried...
in most cases what it boils down to in our shop is "safe" toolchange macros on all machines, which establish certain safety code necessary for each machine... followed by an m1... so the only places which programs are allowed to be started are at a tool change...
ie (from memory):
N3 M6 T3 (TOOL CHANGE MACRO M6 INCLUDES ALL SAFETY CODE)
M1 (T3 - 0.500 ENDMILL)
M3 S12000 (SPINDLE)
G54 Xi Yi (STARTING POSITION AT WORK OFFSET)
G8 P1 and/or G5.1 Q1 R# (LOOKAHEAD and AI/HSM)
G43 Zi H3 (RAPID/SAFE PLANE with TOOL OFFSET)
/M8 (COOLANT ON)
of course i'm always looking for improvements but its working for me now...
again the real problem is standardization throughout the shop... so the more similarly the machines act, the better, however it is... surprises are the worst for operators...
thanks for your feedback
a better comparison would be to single block... unless you press reset, however the program stops certain things shouldn't be changed or codes canceled...
I'd say your on the right track with the use of safe tool change macros to make the differences between machines more operator transparent.
You can try to make things idiot proof, then someone will come along and do something even beyond what you would consider possible.
thats for sure...
tool change macros were the key...
the standard in our shop is the m6 t# [x0 y0] will:
turn off coolant and AI/HSM
reference z(1or2) (whether or not the tool is actually going to change)
turn off tool length comp (g49)
reference 2 x-axis on certain machines which need an x location for tool change ONLY if the tool is actually going to change (using *** when necessary)
set absolute mode g90
set sequence number N(tool#) for easy reference in the top right corner
set spindle tool number to macro #148 for reference***
unlock spindle orient if necessary
optional x0 and y0 will optionally home those axis after homing z and turning off coolant, bringing the part to the door (ref2 g30 location) for the final toolchange of a program to toolchange to the first tool (for faster next cycle)