| | |
I have an Okuma Lathe (OSP700L), and was wondering how it is possible to set up a threading cycle so I can thread a part, stop the machine, measure the threads (without removing it from the spindle), and then make adjustments to the minor diameter in the program in order to adjust the thread depth.
I have tried this with a standard thread cycle but it doesn't always seem to work correctly. It will usually just make a multiple threads across one another, instead of a single thread. Needless to say, this is not what I want to happen.
Is there a specific command so the machine will remember the spindle encoder position, and it will just continue the previous threads the next time you run the program? In other words, what is the correct procedure for doing this?
there are two ways.
1. slide hold; mid-auto manual mode, measurements, insert change, tool offset change, return from mid-auto manual mode, green button.
read operator manual carefully.
2. setting to follow "foreign" thread. Okuma lathes provides possibility to set-up threaded workpiece and to follow this thread. There is even an option, but no needed to buy if You read the manual and understand instructions.
I have only ever used sequence restart when recutting a thread and have not had the problem with recutting threads that you state.
Usually I have programmed the minor diameter according to the thread standard being cut and then adjust to get correct size on the pitch diameter (or Ring gauge) by adjusting the tool X axis offset.
spindle works nearly as C axis while cutting the thread. hence, C axis zerro offset works. There is very simple procedure to set it on Okuma.
and yes, of course - there is the third way:
Sequence restart. the simplyest one, I believe.
If you use the standard G71 cycle you should be fine using the sequence restart - unless you change RPM or take the part out of the spindle. The machine triggers off of a spindle pulse so changing RPM changes the timing from when it sees the pulse to when it starts the thread. Other than that, all Okuma's remember the pulse even across power off. They also can slide hold in the middle of the thread without destroying it. It just pulls out at the programmed pitch and retracts to the start point. When you cycle start again, it will try to complete the previously started thread.
Can you supply an example threading cycle that you are using on your machine?
That way we might pickup any error... keyword=might!
Sequence restart is the way to go
here an example of treading cycle
if you still get problems , check if the pulse generator works correctly (but it usually set an alarm on the controller)Code:(TOOL - 9 OFFSET - 9) (TREAD TOOL 12 TPI INSERT - NONE) ( 7/8-14 ) N830 G0 X20. Z20. NAT9 N840 T0909 N850 G97 S500 M03 M41 N860 G0 X1.075 Z.214 M09 N870 G71 X.7977 Z-.875 B29 D.0299 H.0773 M32 M73 F.0714 N880 G0 X20. Z20. N890 T0900 N900 M01
Sorry for the late reply...this is the sort of program that I've been running:
I think that the problem I was having was coming from the machine operator adjusting spindle speed in addition to minor diameter. This would certainly explain the multiple threads.Code:G90 G50 S 1000 G00 X10.0 Z5.0 T 0606 G97 S500 M3 M8 G00 X1.25 Z0.2 G71 X1.1342 Z-1.250 B60.0 F0.0833 H0.1158 D0.001 U.001 M74 M33 M5 G0 X10.0 Z5.0 M9 M30
Is it still possible to run the program in auto mode, let it finish, go to manual mode and then return to auto mode and re-run the program?
What is the correct procedure for using sequence restart?
Yes, it's perfectly possible. Even across power off as long as the part is not removed from the spindle.
Not only is it possible to change modes it is usually the case when cutting threads. i.e. Cut the thread in AUTO, program stops, go to manual to maybe debur the front of the thread or something else, check the size of the thread, and then return to AUTO mode to recut the thread to size.Originally Posted by H234
I don't know if you are familiar with the Block Count method of restarting or not, but this is a quick way of restarting mid cycle (of a thread cutting cycle or some like that). If you look in the upper RH corner of the screen you should see a ever increasing number that represents the number of "Blocks" executed since cycle start (resets to zero at program start).
For example, if your BC is at 156 at the start of the threading cycle and it takes 10 passes to cut your thread, you will end up with a BC value of 166 at the end of the thread cutting cycle.
If all you want to do is take another 0.02mm off the thread, restart on 165 and the machine will only do the last pass of the cycle.
To restart, using the BC number, press the Restart Key and enter the number at which you want to restart at. i.e. on screen you should see "RS 165" (without the quotes).
If you want to restart the complete threading cycle, select your line number prior to the start of the threading cycle and key in the line number, after pressing the restart key, eg: "RS N1002"
It has been quite some time since I have actually Run a lathe now, but I am certain this is correct.
The BC number is a very fast way of only taking the last pass in a threading cycle.
IT IS VERY IMPORTANT THAT THE SPINDLE SPEED IS UNCHANGED FROM WHEN THE THREAD WAS FIRST CUT!
Like Okumawiz states, it is possible to recut a thread even if the power is cut, just do not remove the part from the chuck!
Hope this helps.
Brian.
Posting Permissions
| | |
LinkBack URL
About LinkBacks
