PDA

View Full Version : Problem okumal b15



bthomps5
03-07-2009, 09:11 PM
trying to figure out how to tap with this lathe , wonder if there is a parameter that needs setting in order for it to do tapping , i have all the manuals for the osp5000 but it dosent have par settings in it or anything on tapping, any help would be appreciated

Thawk53
03-09-2009, 08:05 AM
G77X0.0Z-____K.25F.03125 (Right hand tap)
G78X0.0Z-____K.25F.03125 (Left hand tap)

K is the amount from start point (before G77 block) to cutting start point.
You don't need to use it if you position directly to cutting start point.

Rick

bthomps5
03-11-2009, 08:15 PM
thanks for the info i will give it a try tommorow:) and will reply back to let you know if it works

bthomps5
03-13-2009, 10:00 PM
it gives an error unusable g code , maby you cant tap with this lathe , one guy told me the parameter needs to be turned on or set for it to be able to tap??????

skidoo
03-13-2009, 11:36 PM
it's probably an option, verify it by a test if you have the axe c



4283-E P-130
SECTION 7 FIXED CYCLES
7. Tapping Compound Fixed Cycle
7-1. Right-hand Tapping Cycle (G77)
[Function] Eeoell7p7024
The compound cycle called out by G77 executes a tapping cycle like the one illustrated below.
EIOELL7P7056r01
[Programming format]
G77 X__ Z__ K__ F__
Axis movements:
G77 : G code to call out tapping compound fixed cycle.
Specify this G code immediately after a sequence number (name).
X : X coordinate of tapping cycle start point (target point)
Z : Z coordinate of tapping cycle end point (target point)
K : Rapid axis feedrate for axis feed from the cycle start point to the cutting start point
F : Feedrate
Q1 : The X-axis is positioned at the specified positioning target point (cycle start point) at a
rapid feedrate. In this positioning cycle, no Z-axis movement occurs and thus the turret
must be positioned at a point where it will not interfere with the workpiece during this
positioning before calling out the G77 cycle.
Q2 : The spindle rotates clockwise at the speed applying before the G77 cycle is called.
Therefore, the required spindle speed must be specified before calling the G77 cycle.
If this compound fixed cycle is called without designating a spindle speed, axis infeed
does not occur since the spindle does not rotate and thus the cycle is halted.
Q3 : The Z-axis is positioned at a position designated by a K word at a rapid feedrate.
Q4 : Tapping is performed from the point reached in Q3 to the depth specified by a Z word at a
specified feedrate (F).
Q5 : The spindle stops once and then starts in the reverse direction at the same speed as
used in infeeding.
Q6 : The Z-axis retracts to a point reached in the Q4 cycle at a cutting feedrate.
Q7 : The Z-axis retracts to a point reached in the Q3 cycle at a rapid feedrate.

Superman
03-14-2009, 01:06 AM
It should be a standard cycle suppied with the machine

Have you set the machine ready to tap ?
ie a Realistic Speed ( S150 ), Feed/Rev (G95) , sometime a gear range may be required ( G41 ) to suit Spindle speed,

S150 G41
G95
G77 X0. Z-.5 K0.4 F0.040
G00

DIFF OVER
03-14-2009, 06:41 PM
is this an M tool lathe? if not main spindle sync tapping is an option. On the OSP, options are NOT turned on by parameter, unlike Fanuc. If you get the unusabe g code - you do not have the option.

budgieW
03-16-2009, 03:06 AM
Sync Lathe Tapping and Sync milling tapping are options. The normal float tapping should work

Thawk53
03-19-2009, 09:29 AM
G77 & G78 tapping cycles should be standard on an OSP-5000L. Are you sure it's an OSP-5000L and not an OSP-500L?

Rick

Algirdas
04-04-2009, 06:59 AM
did You changed feederate per revolution. You need to set constant revolution speed also - it could be reason if constant cutting speed is on.