G83 Face Peck drilling cycle

  1. Home
  2. Knowledge Base
  3. Programming
  4. G Codes
  5. Drilling Cycles
  6. G83 Face Peck drilling cycle
  1. Home
  2. Knowledge Base
  3. Programming
  4. G Codes
  5. G83 Face Peck drilling cycle
  1. Home
  2. Knowledge Base
  3. Programming
  4. G83 Face Peck drilling cycle
  1. Home
  2. Knowledge Base
  3. TCM S Machine
  4. G83 Face Peck drilling cycle

G83-Face Peck drilling cycle.
There are (2) parameters related to G83.
Param #5101 bit2 (RTR) “High speed” if “0” then the pecks do NOT come out
of the hole, they only back up the amount of Param #5114 “G83 Retract”,
to break the chip and then start feeding again.

Param #5114 “G83 Retract -200” is the amount to rapid back into the
hole from the last peck for clearance.

I suggest…
Param #5101 bit2 = “1” -Rapid out of hole every peck.
Param #5114 “G83 Retract” = “-200” =-.02 from last peck. No decimal.

G83 X(U)__C(H)__Z(W)__R__Q__P__F__K__M__
R= Distance from intial Point to R Point in radius
P= Dwell time at bottom of Hole
Q= Depth of cut for each cutting feed
F= Feedrate in IPM(G98) or IPR(G99)
K= Number of Repitions (When needed)

Note: G0,G1,G2 or G3 Cancel G83 Our factory recommends G80 to cancel

Example-
M233 M233
T2222M50
G28H0M103S4000
G0X.15Z-.1
G83Z1.R.05Q0300P500F.003
H120.Q0300
H120.Q0300
G80
G0Z1.M105T0
G128
M230 M230

Z1. =Z position of the bottom of the hole

F.001 =Feed in IPR or IPM

R-.03 =Rapid from current Z position the R amount incrementally.
If starting at Z-.05 and R=.03 then the Z axis rapidly
positions to “Z-.02” and after every peck Z retracts to
the same position “Z-.02”. If you use “R-.03” it is the same
as “R.03”

Q2000 =Peck amount -same as .2 but not allowed a decimal point

P0 =Dwell amount at the bottom of the hole. You can just leave
P off the command line if you want
K = Number of Repeats

Was this article helpful?

Related Articles