[RussellSt]

I downloaded some programs off my 1992 Citizen L20 3M6 and some of the commands used are not in my manual.
Can any on explain G79z1.25I.2k.05A.03F.0035
I saw one comment in the manual G79,G83,G84,G85 are optional commands for Deep Hole Drilling,Tapping Boring etc....I think this is a peck drill callout but what would A.03 Can anyone tell me about these commands? Google search yields nothing!

Also they callout a tool command like this:
T1200H.35
what is H.35????

Also used in the program is M61. What is M61?

Also used :
G1G41x.537z.0005F.003
x.573,c.012
G1G9x.573z.93F.0062
x.713,c.012T1F.001
x.713z1.2F.0035
x.765,C.012
W.03

what are all the C.012???


Thanks
Russ

[RussellSt]

looks like m61 and m62 have something to do with the LNS magazine barloader..anyone know what they mean??
G50s2675Q500 ....... what is Q500?
G79z1.25I.2k.05A.03F.0035 ...Is this peck drill 1.25 total depth, .050 per peck, feed .0035......what is a.03???
Thanks Russ

[MCImes]

A lot of what you are asking is in the WIN-CNC help. If you message or email me I can send you a copy of the G&M code help text from Win CNC.


A -In your peck drilling A is most likely the first peck distance. Try changing to to something huge and watch the first peck to confirm this

M61/2/3 are special M codes that send a command to an external PLC. In our shop they control electric spindles on our machines. They could do anything on yours depending on what extra devices you have hooked up. It could also be high pressure coolant, a bar feed command, a drill detector, an external air blast ect. Comand it and see what happens.

G50:
S### = max rpm
Q### = Minimum RPM when in G96


The C's are chamfers. From WinCNC:
A- The Mitsubishi control can use commands with angles instead of X Z

G1 X.025
X.5 A30. (control calculates the Z position)
Z1.

G1 Z.7
Z1. A10. (control calculates the X position)
X.625

,R- Put a radius on the part but the control does all of the
calculations.

G1 X.5 ,R.015
Z1.

G1 X.5 A30. ,R.05
Z1.

G2 X.5 Z1. R.1, R.05
G1

,C- same as ,R but chamfers instead.




H - You can add funny commands to tool calls on Mitsubishi controls. Here is a short excerpt from the L20 g code help. It doesnt have H but I assume its something similar:
T0202 X.2 Z.3 -This first rapids above the bar stock then goes to a
position of X.2 and Z.3 and turns on offset #2 while
indexing to T200.

T0202 X.2 Z.3 Q1 -Q1 tells the machine to go straight to position
X.2 and Z.3 while indexing. X doesn't go up first.
This possibly saves time but is DANGEROUS.
BE CAREFUL!

T0202 X.2 Z.3 Q2 -Q2 tells the machine to go up to position point
then straight to X.2 and Z.3 while indexing.

T0202 X.2 Z.3 F20.-F feeds the tool not rapid.

T0200 H.5 -H.5 Rapids the current tool to stock size +.5 then
indexes to the new tool. Used for mills with a
value in tool set diam that hang down past turning
tools and would hit.

T2323 * -Don't put offset or Z pos on the T2?00 line use T2300
T3131 **-Don't put offset on the T3?00 line use T3100
T2300 W3. -If in G811 mode and W is NOT on the line Z2 goes
T3300 W3. to home position first then indexes and comes back
in to work. If W1 is on the line Z2 goes to W
amount from home position. W is not from the face
of the part!

*Tool call note T2?00. The L5-16/20 is different than the L3-16/20 when using
T2?00 and T3?00. Always use..

T2200 (don't use T2222Z-.05, this moves Z2!)
G0Z-.05T22

**Tool call note T3?00. The L5-16/20 is different than the L3-16/20 when using
T2?00 and T3?00. Always use..

T3100 (don't use T3131Z-.05)
G0Z-.05T31
""
G0Z-.05T0 (If T0 is left out offsets will add together!!)