[jackmac1958]

Hello every one..
i am setting up a precision contact on a Star SR-10J.the problem that i am having is with my o.d thread.(M 0.9X.225) it seems like it is hit or miss every time i set this job up using the G92 thread canned cycle..i am getting a taper in the thread preventing the go- gauge to go on.there is no taper on the thread dia. prior to threading.i was reading in the star manual and it said i maybe having a problem with acceleration and deceleration..due to the fast motor servos and all.the manual suggests to use a (G32code) for threading.if i write out the code for a G92.would some one please reconfigure it to use a G32 for me..i will write out my first turn sequence and thread..once again its for a Star SR-10J..thank you.
T200(FACE AND TURN THRD. BLANK)
G97S7500M3
G0X.103Z.OT2
G1 X-.04F.001
G4 U.1
G1 X.021F.001
G9X.0324Z.0057 F.0003
Z.1212 F.001
G4 U.1
G1 X.035 Z.122F.0003
Z.156F.001
G4U.1
G0X.5 T0

T400(THREAD M0.9X.225)
G97S2100M3
G0X.093Z-.02T4
X.036
G92X.034Z.122F.0088
X.033
X.032
X.031
X.03
X.029
X.028
X.027
X.026
X.025
X.024
X.023
X.023
G0X.5TO
THANKS AGAIN AND I WILL BE WAITING FOR A REPLY.
JACMAC1958

[fordav11]

your speed could be too fast for the servo to handle the acceleration/deceleration. But using G32 will not solve that. Use a slower speed and position the tool so it has enough time to accelerate to the correct feed before it starts to cut. The end deceleration you will just have to put up with as-is since you are stopping on the material.
The formula to calculate the start point acceleration amount in Z is feed * RPM/500
At 2000RPM with a 0.9 pitch thread you need to start 3.6mm in front of the thread start point (0.9 * 2000/500)
The formula to calculate the end point deceleration amount in Z is feed * RPM/1500
At 2000RPM the machine needs 1.2mm to decelerate (0.9 * 2000/1500)

G32 is no better than any other threading method. Just use G92 and put a taper cut on the last pass to take out any taper
G92 X0.023 Z0.122 R-0.001 F0.0088
R is taper amount on radius. To cut bigger at the back make R positive. To cut smaller at the back make R minus

[jackmac1958]

hey.. thanks for your reply.. thats what i ended up doing.putting a taper pass in last pass.seems to do the trick.ended using R-.003.
thanks again.

[ProProcess]

Is it possible for you to us G76 (compound infeed)?
This would give you more control and less tool pressure.

[fordav11]

there's no tool pressure in this case. did you notice the diameter of the thread (0.034)
in any case there are plenty of spring cuts at the end. G76 is no better than what he has.
G76 is primarily for use when cutting deeper threads where it would be too time consuming to write out several hundred roughing cuts. yes it can cut in at 60 degrees or whatever but you can do that in G92 as well if you calculate the Z position. But like I said not required for this thread since it is so small.

[sinha_nsit]

...
The formula to calculate the start point acceleration amount in Z is feed * RPM/500
At 2000RPM with a 0.9 pitch thread you need to start 3.6mm in front of the thread start point (0.9 * 2000/500)
The formula to calculate the end point deceleration amount in Z is feed * RPM/1500
At 2000RPM the machine needs 1.2mm to decelerate (0.9 * 2000/1500)
...

Thanks for information.
I believe it is nearly correct for all controls.

[MetalZilla]

example here: G92 Example

[harshal]

Fanuc g32 threading cycle program II Single point threading II
August 01, 2018 - FANUC G32 THREADING CYCLE [T]



- angle -
Click Here to Continue to angle
O1571
N10 M06 T02 02 ;
N20 G50 S1500 ;
N30 M03 G97 S200 ;
N40 M08 ;
N50 G00 X30 Z3 ;
N60 G32 X29.08 Z-50 F1.5 ;
N70 X28.78 ;
N80 X28.48 ;
N90 X28.18 ;
N100 G28 U0 W0 ;
N110 M05 M09 M30 ;
More examples..........!!!!
DESCRIPTION OF MAIN PROGRAM :-
Calculation :- Depth of thread = 0.6134 X Pitch
= 0.9201
Crest = major dia - 0.9201
= 29.08
Root = Major dia - 2 x Depth of thread
= 30 - 2 x 0.9201
= 28.16 (root)
Each cut is 150 microns =0.15mm , it means total reduce 0.30 mm and cutting upto root 48.16 mm
First cut is 29.07 mm (Crest)
Second cut is 29.07-0.3 = 28.78
Third cut is 28.78-0.3 = 28.48
Final cut is 28.48 -0.3 = 28.18 (~ 28.16)(root)
*************************all dimension in mm ***********************************
01571 - Name of main program
N10- Tool change command , select tool no 2
N20- Maximum spindle speed command , speed is 1500 rpm
N30- Spindle ON clockwise , constant spindle speed , speed is 200 rpm
N40- Coolant ON
N50- Rapid action command , where X30 and Z3 .
N60- Threading cycle command , where X29.08( crest )(First cut) and Z-50 , feed rate is 1.5 ( it is always is equal to pitch )
N70- Second cut is 28.78 in X axis
N80- Third cut is 28.48 in X axis
N90 - Final cut is 28.18 in X axis (root)
N100 - Reference position command , where X0 and Z0 ;
N110 - Spindle OFF , coolant OFF , main prog. end

MY LINK IS
www.hdknowledge.com