CNC waits between toolpaths

[galaxyman7]

Hi, I have built a CNC machine, and I am using Mach 3 to control it. I want to make multiple of one part, and I am using Master Cam X with the translate toolpath command in order to copy one part 49 times. When I review it in master cam, it doesnt show the pauses between toolpaths, but when i open the gcode on mach 3, it shows pauses in between each toolpath group, where I have to tell it to go again each time. I want it to run continuously, so how do I get rid of the pauses?

[ger21]

What do you mean it "shows pauses"?? Is there some message on the screen?

[galaxyman7]

It moves to its home position and then waits until you press "cycle start" to go to the next toolpath. It does this after every toolpath, and it goes to the same position each time.

[CNCadmin]

Try checking off Ignore Tool change, on the settings page.

[TOTALLYRC]

If there is a G28 followed by at m00 or m01 at each pause the machine is doing what it was told to do.

Post a section of the code as it will help with the diagnosis.

Mike

[Superman]

I am using Master Cam X with the translate toolpath command in order to copy one part 49 times. When I review it in master cam, it doesnt show the pauses between toolpaths, but when i open the gcode on mach 3, it shows pauses in between each toolpath group, where I have to tell it to go again each time. I want it to run continuously, so how do I get rid of the pauses?

There is a standard we try to follow for CNC language, a pause is a timed event controlled by a G-code, M0 is "machine stop", M1 is "optional stop" ( leading zeros can be omitted on most controls ie G00=G0, G01=G1, M03=M3 and so on ).

If your machine is "pausing" on an M01 , this is an "Optional Stop", you have the option of ignoring this code while running, it is good code to have in your program for setting up the 1st run, but when all is good, turn the "Optional Stop" OFF ( this is a machine function on the control )

You said Mastercam X "Translate", go to the original operations that you translated, open the operation, and click on and open the "Misc Int" button. Is there a line regarding using M00/M01 outputs ? My guess is that it is set to 1. Reset it to 0(zero), which means "do not use M00/M01s" . Re-post the operations and the M0/M1's should not be in the file.

NOTE---the "Misc Interger" section only applies to that operation, you will have to check all operations

[galaxyman7]

Ok, i have tried looking under misc values for each toolpath, but there are no options for M00 or M01. Here is a section of code with the M00 in it.
N6510 G0 Z.255
N6520 M5
N6530 G91 G28 Z0.
N6540 M00
N6550 T232 M6
N6560 G0 Z.255

M5 is stop spindle (i dont have spindle control anyway)
G91 is incremental mode
T232 ???
G28 must be home position.
If I delete all the lines except the first and last I should be where I started, then it can go onto the next toolpath(hopefully). I just have to do find and replace on all of these lines in notepad or mastercam editor