[springer82]

Hi Everyone. I'm one of the NEW guys on the block from Mn. Just starting to learn about macro programming. WOW!!! I have been lurking here for a while. There are a lot of smart people here. I hope I have a chance to learn from ya. Scott,,, I enjoy using your back plotter. We have nothing at work that will do the job. Thanks for your time.

Now for the Newbie question. I am doing a family of parts program. I have 8 programs into 1. Ok,, Ok,, simple for you. Way cool for me. This is fun!!! The body is all the same. The changes come in with I/D bore size. I have 5 drills and 5 reamers.
N5IF [#101NE1.] GOTO6
#7=#2003
When I set the TLO using #2003 for tool #3 and #2004 for tool #4,,, I get an error message. "Can not find Number” Something like that anyway. I am setting #7 to whatever tool I am using then using #7 as my H# in the program. In my manual (Fanuc 16i-M) it tells me that the TLO #'s are stored in these variables. With the alarm that I get I wonder if I have the right location??? Can anybody point me in the right direction. That would be great. Thanks for your time.

[MetLHead]

Hi,

NCPlot doesn't use tool length or radius offsets, but you should still be able to set the variables for them. Can you post or email your program with the error?

Thanks,
Scott

[springer82]

Hi Scott,
That must be why my program runs on NCPlot with out a problem. I will have to wait until Monday to check the error message off my machine. Thanks for your time. Have a great day.

[Andre' B]

The line
#7=#2003
is going to set #7 to whatever the value of tool length offset 3 is, which depending on how your shop does offsets may be somthing like -5.236 etc..
If you are then doing H#7 the control is going to be confused.

You have 5 drills and 5 reamers so I would use offsets 1 thru 5 for the drills and 11 thru 15 for the reamers.
Assuming the tool changer on the machine can handle 15 tools then the tool number can be the same as the length offset.
You then just need some code at the top of your program to set which tools you want to use.

#1=3(DRILL TO USE)
#2=#1(REAMER TO USE)
(DO NOT EDIT BELOW THIS POINT)

G0G17G20G40G49G80G90G94

N1M1(DRILL)
T#1
M6
M1
T#2 (PRELOAD IF IT APPLIES TO YOUR MACHINE)
G0G90G54X0.0Y0.0
S500M3 (THIS IS WHERE YOU CAN GET FANCY )
(AND USE #1 TO GET A TOOL RADIUS/DIAMETER )
(AND CALCULATE THE RPM TO THE DESIRED SFM )
(WHICH COULD BE HARD CODED INTO THE )
(CALCULATION OR SET AS ANOUTHER VARIABLE )
(AT THE TOP OF THE PROGRAM)

G43Z1.0H#1
M8

G83Z-2.5R0.1Q0.2F6.0L0(NOTE FEED COULD ALSO BE CALCULATED)
.
.
.
G80
M9
G91G28Z0M5 

N2M1(REAM)
(SEE DRILL JUST SWAP THE #1 AND #2)