I searched alot about this and didnt find anything helpful, i know its a drilling code, but the meaning of "I","K","Q","j"?
For Example:
G79 Z.402 I.1 K.05 A.01 Q100 J200 F.001
Printable View
I searched alot about this and didnt find anything helpful, i know its a drilling code, but the meaning of "I","K","Q","j"?
For Example:
G79 Z.402 I.1 K.05 A.01 Q100 J200 F.001
Radial Cutting Cycle G94 (B set G Command G79)
Command function: From start point, the cutting cycle of cylindrical surface or taper surface is
completed by radial feeding(X) and axial (Z or X and Z) cutting.
Command format(A set) : G94 X(U)
_ Z(W) _ F_
_;
(face cutting)
G94 X(U) _
Z(W) _ R__F__: (taper face cutting)
Command format(B set) : G79 X Z. _F;
(face cutting)
G79 X_Z_R_F_ _: (taper face cutting)
Thanks alot but you are talking about something else!! The g97 that i asked about is for drilling, like g83... and what about the meaning of "i,k,a,j"??
I don't think G79 is in milling machines controllers.
https://www.youtube.com/watch?v=Y221oZYU9VY
A G79 depends on what machine control you are using here is a Siemens example, its not normally used for Drilling.Quote:
Originally Posted by Amensn91
https://www.cnccode.com/4147/siemens...these%20blocks.
Its a citizen cincom lathe l20, swiss tybe
There is not a lot on citizen programing,Quote:
Originally Posted by Amensn91
This may help then. https://en.industryarena.com/forum/w...9--187600.html
From what I found online:
Siemens CNC Lathe | G79 – G94 Cycle | Facing
Straight Facing Cycle
With the commands of “G… X(U)… Z(W)… F… ;”, straight facing cycle of 1 to 4 as shown in Fig. 4-11 is executed.
The cycle code can be change due to pre-selected G code system as below ( Selected by machine tool builder by parameter setting).
G code system A = G94
G code system B = G79
G code system C = G24
G83 Normal Peck Drilling Canned Cycle (Group 09)(Haas lathe)
* C - C-Axis absolute motion command (optional)
F - Feed Rate in inches (mm) per minute
* I - Size of first cutting depth
* J - Amount to reduce cutting depth each pass
* K - Minimum depth of cut
* L - Number of repeats
* P - The dwell time at the bottom of the hole
* Q - The cut-in value, always incremental
* R - Position of the R plane
* X - X-axis motion command
* Y - Y-axis motion command
Z - Position of bottom of hole
* indicates optional
May be a combination of above.
G79 is used as a peck drill cycle on all Nomura machines.
Z = absolute depth of hole
I = 1st peck amount in incremental from start position
K = subsequent peck increments
A = clearance to bottom of previous peck (A.01 means to rapid to .01 away from the previous peck depth to start next peck)
Q = dwell at bottom of hole(Q100 = .1 second)
J = dwell at start of hole to cool drill between pecks and to help clear chips (J200 = .2 seconds)
F = feed in ipr
Great cycle that can also be used for cross drilling - just substitute X for Z