toolchanging

[zcases]

In my case (Mach2), the problem has been fixed by deleting the text from the default M6end macro.

[zcases]

It could be helpful to see the code around your toolchange, and your M6 mascros.

[bbuonomo]

there is nothing in the m6 file. Should there be?

The code is up a few messages 36_tooth.zip.

I'll try the T0 and G43 HO like you said.

Thanks.

[merl]

bbuonomo,
In your last PM to me you said, only the 1st tool or, the tool you set your Z zero with actualy touches the part and the rest of the tools operate above the part.
1. Do the tools rapid to and start their programed operations at the same highth as each other, say all tools rapid to one inch from the top of the part and start working from there?
2. Or does each tool rapid to a diferent highth and start its operation?

If they act as in case 1. I would ask how do you touch off your tools?
If you use some kind of spacer (1" block ect...) and you don't add or subtract the amount of the spacer ,as the case may be , from your tool length offset that could be causing your problem.

If they act as in case 2. I would say to try entering the offset numbers the opposit of how you do it now. If you normaly input the number as a negitive then try it as a positive or, visa versa.
Having said that I would also caution you that the number may not just be a negitive or positive. It could also be the difference between the tool one offset and the offset of each of the following tools as compared to zero.
This is kind of a complicated thing to explane and I don't want to send you on a wild goose chase as it may not be your case at all.
As Hu Flung said try putting the tool calls on their own line and see what that does also, try canseling the previous tool offset befor you call the next tool.
I find that when I start to have problems with a straight G code program it somtimes helps to really spell it out for the controle, one operation per line and no fancy short cuts.
When I do this I force myself to look at every thing I'm writing in and that's when I usualy find it was somthing I did wrong.
If you have the programing manual it should tell you in there.
If you got voo doo in da macheene call a witch doctor!!

[bbuonomo]

well after lots of trial and error, we figured out it was a gcode error. The G91 (incrimental), needed to be G90 (absolute).

that was my fault for not knowing mastercam or how to program gcode all to well :-/

thanks for the help!

sprocket cut this afternoon!!! :-)

[Art Fenerty]

Hi Guys:

I dont get here often. (Like every couple months.. ), but let me explaina bit about G43 so you understand how it works. SOem of the above is due to misunderstanding its effect. Sorry I was too late with the solution..

The M6Start macro is called when the M6 is seen. The position of the Tx isnt important, as long as its on the same line or previsou lines. IT selects what the M6 will change to. The GetSelectedTool() call gets the last T's variable, so any T7 woudl make that return 7. Never exect the M6 macros to see a toollength. That is instatiated after M6start and M6end have run when the G43 is seen. G43 will cancel the previosu tool length, and put the new one in effect. IT willnot move until next move. By specification, the move foolowing a G43 should always be a Z move. This is called the correction move. If you have a tool loaded and do an MDI of G43H1 , youll see the DRO for th eZ change to reflect the new tool tip location. The next move is meant to allow the interpreter to correct its know position of Z to proper point.
Mach3 , over the last 2 years has made this safer by not requireing the Z move following, it updates it trajectory locations internally so if the next move is g1x10, the Z will not move. (Thats the danger of not correcting after a G43..). The A line of moves like..

G1X10Z0
G43H6
G1X20
woudl sometimes make the Z move on the G1X20 line, beacuse the controller woudl think the last Z command was zero, but with the offet its now -30 or whatever, so it woudl unexpectantly move. This can happen in Mach2 for example. In Mach3 you shoudl be OK and no movement should occur.

Be carefull of the moves int he macros M6start and end, as they occur before any G43 is applied.. (Unless you do G43Hx before the M6Tx line..
'
Thanks
Art