Learning G10: please help

[sinha_nsit]

I am trying to learn the use of G10. Please confirm if my interpretation of the following codes is correct:

G90 G10 L10 P10 R-500; (Enters -500 mm into offset number 10, as the geometry compensation value for H-code)

G91 G10 L10 P10 R5; (Enters 5 mm incrementally into offset number 10, as the geometry compensation value for H-code, making the tool length smaller by 5 mm. So, the same tool would dig 5 mm more into the workpiece, for the same program)

G91 G10 L11 P10 R0.5; (Enters 0.5 mm incrementally into offset number 10, as the wear compensation value for H-code. So, the wear value would increase by 0.5 mm, and hence, the same tool would dig 0.5 mm more into the workpiece, for the same program)

[stevo1]

Sinha,
That is correct. The only thing I cannot confirm is if you have the proper “L” for the registry. I don’t have any of my data with me. Speaking of that does anyone have a master list or a spreadsheet with the “L” meaning of each registry? I always have to look it up in the book and IIRC they are not all the same per control.

Stevo

[sinha_nsit]

Thanks for the reply. You are always helpful.
As per 0i manuals,
L2 is for work offsets,
L20 is for additional work offsets (on milling machines only),
L10 is for H-geometry,
L11 is for H-wear,
L12 is for D-geometry,
L13 is for D-wear,
No L is used for lathe compensation values,
L50 is for parameter entry, and
L3 is for tool life data entry.
L1 can be used in place of L11.

Other control versions may use different L values. For example, I have heard that 180i uses L52 for parameter entry.

However, for offset and compensation data, there is not enough reason to use G10 (because one has to remember its syntax). I would prefer to use system variables. Of course, for parameter entry and tool life data entry, through a program, G10 is the only method.

[stevo1]

Your always welcom Sinha.

Thanks for the feedback on the "L" designation.

Stevo

[ChattaMan]

Sinha, all your code looks good.
Maybe not the point of your post, probably just me being picky.

The meaning of this one
.....
G91 G10 L11 P10 R0.5; (Enters 0.5 mm incrementally into offset number 10, as the wear compensation value for H-code. So, the wear value would increase by 0.5 mm, and hence, the same tool would dig 0.5 mm more into the workpiece, for the same program)
.......

This would increase the wear comp by 0.5mm and so make your tool longer (or bigger dia if used for D value). So it would dig 0.5mm less, into the workpiece.

e.g. need to leave more material on, then comp+
need to take more material off, then comp-

[sinha_nsit]

Thanks for your comments.
Actually, I was more interested in verifying if my interpretation was correct.
Since, I do not have 0i M control, I can only rely on you people.

Are other interpretations OK?
How about this (I am repeating):

G91 G10 L10 P10 R5; (Enters 5 mm incrementally into offset number 10, as the geometry compensation value for H-code, making the tool length smaller by 5 mm. So, the same tool would dig 5 mm more into the workpiece, for the same program)

Wiil the tool dig more or less?

[dcoupar]

H10 = -255.000
G43 Z0 H10 moves tool down 255mm.

execute G91 G10 L10 P10 R5

H10 is now - 250.00
G43 Z0 H10 moves tool down 250mm.

This is assuming your control interprets R5 as 5mm, not .005mm

[sinha_nsit]

Thanks.
So, in my previous post, more should be replaced by less, if we are using G43.
Correct?

[christinandavid]

Hi,

Sorry for butting in, have recently discovered G10 myself and I use it in programs to reload my previous work offsets.

Noted that there are L-codes that relate to tool offsets - is there also a way (not necessarily G10) to load other tool information via the program, ie the tool type/tool description info, which can then be displayed in 'Current Machining'?

DP

[sinha_nsit]

As far as I know, there is no way a message can be displayed while the machining is being done. It is, however, possible to use system variable #3006 which will halt (but not terminate) the execution and display user-specified message (up to 26 characters) on MESSAGE screen. You have to press CYCLE START again to continue further machining. Details of #3006 are given below:

System variable #3006
System variable #3000 generates an alarm condition and terminates the program execution, whereas variable #3006 causes temporary pause of execution which can be restarted by pressing the CYCLE START button again. In the paused state, pressing the MESSAGE key displays the user-specified message (up to 26 characters). Assigning a number to variable #3006 halts the program execution. There is no significance of this number, as message number is not displayed. So, normally, 1 is assigned. Example:
#3006 = 1 (CHECK THE DIAMETER);
This would temporarily stop the execution, and display “CHECK THE DIAMETER” on the message screen. If no message is typed, nothing would be displayed.

[christinandavid]

Hi again,

Wasn't refering to a message on screen this time.. Was hoping there was a G10 L* and R* command that could load other Tool data such as the tool's shape/orientation for use with the graphic simulation (rather than inputting it directly into tool table). Bizarre request, I know, but there it is.

DP

[sinha_nsit]

The graphic feature of the control does not show tool shape. Only toolpath is drawn. Manual Guide i might be showing more realistic simulation, but I have no experience on that. I have used some third-party simulation softwares, where one has to choose the shape/orientation of the tool(s) being used in the program. It is not a part of the program. This has to be done independently, before simulation.