[ducatidragon916]

I created a simple path to cut some plastic and everything worked fine except the cutter plunges too deep than what was expected. i think maybe the NC code is wrong for the machine? Here is the NC code Listed...why would it plunge deeper than the set surface material? Please help!!???

%
O0000
(PROGRAM NAME - FRONTCOVER )
(DATE=DD-MM-YY - 20-09-13 TIME=HH:MM - 19:48 )
N100 G20
N110 G0 G17 G40 G49 G80 G90
/ N120 G91 G28 Z0.
/ N130 G28 X0. Y0.
( 1/8 FLAT ENDMILL TOOL - 232 DIA. OFF. - 0 LEN. - 0 DIA. - .125 )
N150 T232 M6
N160 G0 G90 X3.2625 Y-3.43 A0. S4278 M3
N170 G43 H0 Z.25
N180 Z.1
N190 G1 Z-.09 F6.16
N200 Y-4.35
N210 G2 X3.2 Y-4.4125 R.0625
N220 G3 Y-4.5875 R.0875
N230 G2 X3.2625 Y-4.65 R.0625
N240 G1 Y-5.57
N250 G3 X3.33 Y-5.6375 R.0675
N260 G1 X5.57
N270 G3 X5.6375 Y-5.57 R.0675
N280 G1 Y-4.65
N290 G2 X5.7 Y-4.5875 R.0625
N300 G3 Y-4.4125 R.0875
N310 G2 X5.6375 Y-4.35 R.0625
N320 G1 Y-3.43
N330 G3 X5.57 Y-3.3625 R.0675
N340 G1 X3.33
N350 G3 X3.2625 Y-3.43 R.0675
N360 G1 Z.01
N370 G0 Z.25
N380 X-3.8175 Y-2.64
N390 Z.1
N400 G1 Z-.09
N410 Y-3.24
N420 Z.01
N430 G0 Z.25
N440 X-1.5625 Y1.7
N450 Z.1
N460 G1 Z-.09
N470 Y-2.42
N480 G3 X-1.425 Y-2.5575 R.1375
N490 G1 X1.425
N500 G3 X1.5625 Y-2.42 R.1375
N510 G1 Y1.7
N520 G3 X1.425 Y1.8375 R.1375
N530 G1 X-1.425
N540 G3 X-1.5625 Y1.7 R.1375
N550 G1 Z.01
N560 G0 Z.25
N570 M5
N580 G91 G28 Z0.
N590 G28 X0. Y0. A0.
N600 M30
%

[WOTDesigns]

Not really enough info.
When does it plunge in?
How deep does it go?
Why are you calling a tool number (232) in line 150 then calling height for tool zero on line 170? That may be your cause.
How did you set your part zero?

You are using tool 232 and calling tool H0 (zero). Is tool 232 referenced as tool height at zero

Brian
WOT Designs

[ducatidragon916]

I got this nc code from using mastercam software and used it in the unit to cut. I thought maybe an offset tool height was wrong but I think that the MDX 500 ignores this command 49. The cutter plunges right after it gets to the first cut xy coordinate line N170. Even though i used the zero sensor to zero the z axis and it does register as 0 just touching workpiece, still goes about 1/4 inch down into the material. The number on the lcd screen after the plunge is -1186. I am not sure about the tool reference as it is what the software has set from using a 1/8 end mill etc...Thanks for your desire to help me out on this much appreciated!!

[ducatidragon916]

sorry correction maybe about .5 inches plunge from visual....which corresponds to a metric of 1186 um or 11.86mm etc...hope that helps?

[WOTDesigns]

Is the tool abut the same distance longer than the reference tool?

I remember having to set the default in Mastercam to (add to tool length=0) in a setting for the machine. It must output matching (T) and (H) numbers. Something wrong in the post or Mastercam.

G43 H0 tells the machine you are cutting with tool #0 tool, not the tool 232.

I'm not familure with that control but T and H numbers matching is the standard

Brian
WOT Designs

[ducatidragon916]

is that under control definitions machine type under tool tab?

[Superman]

I got this nc code from using mastercam software and used it in the unit to cut. I thought maybe an offset tool height was wrong but I think that the MDX 500 ignores this command 49. The cutter plunges right after it gets to the first cut xy coordinate line N170. Even though i used the zero sensor to zero the z axis and it does register as 0 just touching workpiece, still goes about 1/4 inch down into the material. The number on the lcd screen after the plunge is -1186. I am not sure about the tool reference as it is what the software has set from using a 1/8 end mill etc...Thanks for your desire to help me out on this much appreciated!!

WOTDesigns is 90% there

A few problems with your use of Mastercam & the machine, that you need to familiarise yourself with
- setting part origin in the machine
- tool offset registers & their use ( not sure if your machine uses H offset )


There is no part origin call-up in your program, ie missing G92 or G54---these are methods to set the part origin in respect to the machine origin (machine home)
( G54 is output to the NC code when "Miscellaneous Integer #1" = 2 , in the Mastercam operations)

T232 = tool number 232
H0 = H0 can only be zero, usually it must be greater than one, it looks up the value in the offset tables to set tool length
D0 = H0 can only be zero, usually it must be greater than one, it looks up the value in the offset tables to adjust tool diameter when using G41/G42
H0 & D0, in the machine, are set to zero & cannot be altered.

Just glanced thru the NC Code manual for the machine. it ignores any unsupported M-codes
- it seems to set G54 as the default in the machine ( even if not stated in the NC code) , so you did set G54(XY) at the beginning & then set G54(Z) after each manual toolchange ( unless they are all set to the same distance out )
- did you use "sensor mode" correctly ? .....for each tool ?
- G43 H0 seem to be not used, try running the program with those items deleted from the NC code
- use "Single block" & a slower feedrate (at the beginning) to make sure your tool runs to the correct height ie cycle thru to line N170, is tooltip at Z0.25" ?.....yes.....then remove single block & increase feedrate, & continue the program

 / N130 G28 X0. Y0.
 ( 1/8 FLAT ENDMILL TOOL - 232 DIA. OFF. - 0 LEN. - 0 DIA. - .125 )
 N150 T232 M6
 N160 G0 G90 X3.2625 Y-3.43 A0. S4278 M3
 N170 G43 H0 Z.25
 N180 Z.1
 N190 G1 Z-.09 F6.16

[ducatidragon916]

got it.. I had deleted that function and when i added back it worked like a champ no unusual z axis plunge cutting etc... However the XY zero is not setting on the machine. I go to set origin and it calls us G54 set (XY) which is cool but when I set it in the center it is slightly off etc... Maybe I am not doing something right again.. Boy i feel like a kindergarten kid.....Thanks for all your help and appreciate the patience!!!!

[ducatidragon916]

it worked and then when I placed a new sock in and re zeros everything to the origin etc. I stared to cut and damn if it didn't plunge again in the new piece again!??? Wow I am really at a loss.... Here is the nc code i used.....

%
O0000
(PROGRAM NAME - FRONTCOVER3 )
(DATE=DD-MM-YY - 24-09-13 TIME=HH:MM - 09:15 )
N100 G20
N110 G0 G17 G40 G49 G80 G90
/ N120 G91 G28 Z0.
/ N130 G28 X0. Y0.
/ N140 G92 X10. Y10. Z10.
( 1/8 FLAT ENDMILL TOOL - 232 DIA. OFF. - 0 LEN. - 0 DIA. - .125 )
N150 T232 M6
N160 G0 G90 X9.2625 Y2.57 A0. S4278 M3
N170 G43 H0 Z.25
N180 Z.1
N190 G1 Z-.09 F6.16
N200 Y1.65
N210 G2 X9.2 Y1.5875 R.0625
N220 G3 Y1.4125 R.0875
N230 G2 X9.2625 Y1.35 R.0625
N240 G1 Y.43
N250 G3 X9.33 Y.3625 R.0675
N260 G1 X11.57
N270 G3 X11.6375 Y.43 R.0675
N280 G1 Y1.35
N290 G2 X11.7 Y1.4125 R.0625
N300 G3 Y1.5875 R.0875
N310 G2 X11.6375 Y1.65 R.0625
N320 G1 Y2.57
N330 G3 X11.57 Y2.6375 R.0675
N340 G1 X9.33
N350 G3 X9.2625 Y2.57 R.0675
N360 G1 Z.01
N370 G0 Z.25
N380 X2.1825 Y3.36
N390 Z.1
N400 G1 Z-.09
N410 Y2.76
N420 Z.01
N430 G0 Z.25
N440 X4.4375 Y7.7
N450 Z.1
N460 G1 Z-.09
N470 Y3.58
N480 G3 X4.575 Y3.4425 R.1375
N490 G1 X7.425
N500 G3 X7.5625 Y3.58 R.1375
N510 G1 Y7.7
N520 G3 X7.425 Y7.8375 R.1375
N530 G1 X4.575
N540 G3 X4.4375 Y7.7 R.1375
N550 G1 Z.01
N560 G0 Z.25
N570 M5
N580 G91 G28 Z0.
N590 G28 X0. Y0. A0.
N600 M30
%

[ducatidragon916]

I think I found the answer to all my troubles on this machine for the z-axis problems... You need to zero out on the line G54 set on the machines lcd screen even though you sensor the zero surface point with the sensor. Apparently the machine doesn't recognize the sensor mode etc.. Once i did that it went to exactly where it was suppose to go ....Thanks guys for all your help!!!!!I am such a knuckle head.....