[Tommie]

Dear,

I like to know if and how I can "peek" in the control if the M1 button is pushed on the control.
This to make sure that the tool will not stop inside the material if the M1 line is really applied. And so all inserts will break.
So basically I like to “peek” to the marker that is set by the button on the control display and react on that marker by a motion before really applying the M1.

My drilling program should look like this:​
#1=1
G00Z+#1M3
N1
#1=#1-1
G01Z+#1F50
IF[#4???EQ?]GOTO1000
IF[#1GT-100]GOTO1

N1000
Z+50 F500
M1
M30​
​

[Superman]

M1 is only applied if the Optional Stop is turned ON on the control panel

It seems a silly way to program a drill cycle that is usually standard on all machines
- you seem to want it to "peck drill" at 1mm pecks until Z-100 is achieved, retract at feed to Z50 then Opt stop them program end ( the opt stop would do nothing as the next line (M30) stops everything anyway )
but this it will perform like a G81 for a 100mm plunge, with no apparent chipping ( as there is no back-off at each "peck" )

Look up a G73 cycle using the Q value ( peck at each Q peck until Z is achieved )
or
G83, ( where the tool retracts to R after each Q peck, but done at rapid)

there is a bore cycle that feeds in & feeds out (used for reaming), look up G85

[Tommie]

Hi Superman,

Okay, good point. I need to give more background info.
The machine is a vertical lath with a 1600mm chuck!
The drilling operation will be done in the center of the product, with the tool standing still and the chuck turning.
The tool is a HTS index drill from Kennametal, diameter 150mm!!
HTS-R Bohrsystem - Bohrtiefen bis 10 x Durchmesser und mehr - Konradin Verlag

The point is that I don't want to peck (thats very bad for the drill) but i want to have one continuous drill motion (made by incremental moves) that can be "aborted" at any moment with for example the button M1.
If we push "stop", "reset", ore realy use "m1", the inserts will be be broken and also the insert carriers! This due to the slow stopping of the very big chuck and the pressure on the drill!
By using the "peek" for the marker of the M1, I can allow the operator to interrupt the drilling motion and give the machine a retract out of the material, so the inserts will remain intact (hopefully;-)).

The second thing that I can make is not the M30 after the M1 is a readout of the actual z-position where the drill was so the process can be continued after inspection ore replacements of the inserts.

Hopefully you can see my problem and the fact why I like to have a answer on my question!

[underthetire]

Sounds like you need either manual handle interruption or mid cycle interruption. Both were options. I suppose you could wire something up to a skip input and use that with a macro to retract a certain distance.

[Tommie]

"manual handle interruption" or "mid cycle interruption" should be like tool retract and recover??
For some reason this feature is not supported by the machinetool builder (tongtay and honer) so not active....

But you guys set me to think!! I am a heidenhain fan and only work very little with the fanuc.
How about blockskip. I find on google that I is supported and that should be a good solution for me.
But now a dummy question!!
I have never seen that buttons on the control screen, so where can I find them? Ore is blockskip also some fanuc option that can be turned off??

Thanks in advance

[Heavy_Metal]

Hi Tommie,

Check your manual at page 394--- for the G10.6 function, TOOL WITHDRAWAL AND RETURN, 18i-TB OPERATOR'S MANUAL GFZ-63524.
I don't know how it works.
You can also try [ / ] and [ BLOCK SKIP ] with incremental move's.

Regards,
Heavy_Metal

[fordav11]

Those functions are optional and I doubt you will have them available.
Also, I don't think you can check the status of the switches without some advanced functionality (like a skip signal)
you can use block delete [/] and a Z+ movement that will rapid the tool out of the hole when / is on then stop.
if you use a sub program for the drilling you can set the Z start position in the main program when you restart it.

in theory, something like...

O0001
G0 T0101
G97 S100 M3
G0 X0 M8
Z5.0 (edit this position on restart)
M98 P0002
G0 Z300.0 M9
M5
M1
M30

O0002
N1 G1 W-0.5 F0.1
/G0 Z300.0 M5
/M0
(code to check depth here from attached example)
GOTO N1
M99

another idea is to store the current Z position using #5042 in the sub program and then in the main program use G00 Z[#5042 - 2.0] to go back there (less 2mm) on a restart.

there is an example drilling macro in the programming manual where the current position is stored and re-used and the depth is added up until the end position is reached. I'm not going to re-write that and customize it to your problem but have a look at that to get some ideas.
it could be as simple as using it as-is but in a sub program (so you can control the start Z on a restart) and adding a /G0 Z300.0 M5; /M0; after the feed line.