[togr]

Hello.
I wonder if anyone can help me?
I am programing a yasnac j50m. I am trying to engrave some forging pistons.
The issue is that its limited space in the controller. So i have try to use the program i generated in mastercam( one cut) and used it as a sub program. I programed a main program whit G52 Z-0.05 and call the sub program again and again. If you understand? The problem is that the yasnanc use the G52 for another use.
Any ideas how i can do this insted?
Sorry for bad english. I realy hope anyone can help me?

Tommy. Norway

[fordav11]

try G92. you can set G92 XYZ to any position so instead of an incremental shift using G52 you move incrementally then you set the current position to an absolute X...Y....Z.... position
so....
G91 G00 Z-0.05
G90
G92 X0 Y0 Z0
(do some machining here)
G91 G00 Z-0.05
G90
G92 X0 Y0 Z0
etc

[togr]

Thanks for answer
I will try that. Can i use G92 zo? I want to mentain the x and y datum as it is. I most do the datum shift there the egraving starts. The part i am engraving on is totaly flat so to not get any other marks in the part i got to do the datum shift there?

[holbieone]

G92Z0 sets Z to 0

G92Z1 sets Z to 1

G92X.123Y.456Z.789 will set X to .123 Y to .456 Z to .789

so move to the position you want to call Z0 then use G92Z0 to set it to 0

[togr]

Than you.

I am looking forward to try it over the weekend.
Is there somting i have to do for cansel the G92. Before i put in a new part and press start?. So i dont crash.

[holbieone]

you can't cancel it , G92 resets the Work Coordinate System

to go back to where you were you need to move the same distance but in the opposite direction then do another G92Z0

[togr]

I understand. Thank's for the help.

[fordav11]

G92 physically changes the position and there's no cancel.
You can go back incrementally by the same amount you shifted then issue another G92.
Or to reset the work coordinate system completely go back to the zero return position and set the work coordinate system to your known reference position (in relation to your part origin X0 Y0).
basically if you apply more than one G92 in one program it's very easy to screw up the position so you must go back to your reference position then re-set the coordinates to a known position otherwise you will lose where you are with reference to the part X0 Y0.

so at the end of that tool just put....
G91
G28 U0 V0 W0
G90
G92 X..... Y...... Z......

[togr]

Thank you so much.
It worked great for me.
I am so greatfull there are some experts to ask.
This made my work much easier.

[angelw]

Hi Tommy,

The Yasnac J50M control uses G52 to Return to Base Coordinate System, it has no other use. G53 is a Temporary Coordinate System Shift and can be used instead of G92 with the added advantage that you don't have to go back to a start position to cancel the effect of multiple G92 executions. Both G52 and G53 are options to this control, but given that you make reference to G52 without saying that an alarm occurred, its likely your machine has that option. If the control has G52 then it will have G53, and if it has those two functions, it will also have Work Shift Offsets G54 to G59. If your control has these options, its a better choice to use Work Shift Offsets, or Temporary Coordinate System Shift G53 than to use G92.

Regards,

Bill

[fordav11]

it wouldnt be possible to use workshift offsets because he needs to shift only a small amount then re-run a sub-program. unless he has 1000 workshifts which of course he doesn't. he could shift a single workshift with macro as well, assuming he had macro and knew how to use it which is unlikely. It's probably possible to use G52/G53 but since its use is non-standard G92 is the simplest way to achieve the result in this case.

[angelw]

Using G53 is the simplest method as its implementation is no more difficult than using G92, but without the downside of using G92.

[fordav11]

the problem was solved using G92 some days ago so.....

[angelw]

the problem was solved using G92 some days ago so.....

Big deal if a one solution was given days ago. It clearly isn't the best solution if you think it is, or aren't you aware of the shortcomings of using G92 when compared with using Temporary Work Shift G53. The OP made reference to using G52 without any mention of an alarm, notwithstanding that his stated use of it was incorrect, therefore his control must have this feature. That being the case, it will also have G53 and G54 to G59, and using one Work Shift and G53 to Temporarily shift the "Z" Work Shift will win over using G92 any day of the week.

[fordav11]

:violin:

[angelw]

:violin:

Although lame. your reply is a bit different than usual. Normally its about now that you reply with your little rant about getting OT and that you're not going to reply any more, taking your bat and ball with you.

[fordav11]

while your reply is typical :bs: and predictably over-complicated and late
:wave:

[angelw]

while your reply is typical :bs: and predictably over-complicated and late
:wave:

Its not all that surprising that you find such a simple concept complicated, but the majority don't. Offset Programming was developed to make CNC programming, machine set up and operation simpler and safer. But hey, if you can't come to grips with the more relevant programming methods, and feel more comfortable with the old ways, then just stick with it.

[fordav11]

the OP wants a simple solution, not your long-winded over-complicated book.
And a simple solution is what was provided...... 3 weeks ago.
:wee:

[angelw]

the OP wants a simple solution, not your long-winded over-complicated book.
And a simple solution is what was provided...... 3 weeks ago.
:wee:

Again, who's problem is it if you can't/don't understand simple Work Shifts and Temporary Work Shift G53?