Laser/spindle combo

[sngatlanta]

What about Z in the post processor?

[sngatlanta]

OK changing the M3/M5 to M10/M11 in the PP doesn't power on and off the laser while running a file.
with the new PP from V carve.

[cncdrive]

With the M3/M5 you can control the spindle relay output (on/off).
The M3/M5 is not a fast syncronous output, so when you switch the relay the motion always deccelerate first to a stop then the relay switches and then the motion continues, so using these codes is not ideal for laser control.
So, the M3/M5 control pin is the spindle relay output pin setting and not the laser pin setting. You have to configure that if you using the M3/M5 codes.

The M10/M11 gives motion syncronous output, so when you code M10 or M11 then the output switches without motion decceleration, it switches in syncron with the motion while the motion is ongoing, so these codes are good for laser control.
The M10 gives a PWM signal. You can vary the signal duty cycle with the Q parameter of the M10 command like M10 Q128, which gives an 50% duty cycle.
If the Q parameter is not programmed then the duty cycle is 100%, so it acts as a digital on/off switch similar to the M3/M5, but it is still motion syncronous.
The M10/M11 is on the laser output pin, you have to configure that port/pin if you using the M10/M11 codes.
One more important thing is that the M10 command requires the M3 to be active for the M10 to work. In other words the M3 acts as a safety enable signal for the M10.
So, code M3 once in the beginning of your g-code file or switch the spindle on with the spindle CW (M3) button on the screen if you will code M10 in your g-code file or via MDI.

[sngatlanta]

CNCDRIVE-
I have everything working Manually.
I'm sure it in my postprocessor or the way I'm setting the laser up in v carve.

Here is the changes to the Laser PP for rapid moves I made:
begin INITIAL_RAPID_MOVE
"M10"
"G0[X][Y]"
"G0[Z]"

begin RAPID_MOVE
"M11"
"G0[X][Y][Z] "

Is that right?

[cncdrive]

I'm not familiar with the post processor syntax of the CAM program you using, so I don't know if it is OK or not.
It would be more helpful if you post a short example g-code file which was output by the post processor you've made.

And again, you have to have the M3 on for the M10 to work. The best way for that is to place (post) an M3 once at the beginning of your g-code file,
because if the M3 is not active then the M10 will not switch as the M3 is a safety enable signal for the M10.

[sngatlanta]

LASER TEST 1.txt

Laser G Code

(28.42 KiB) Downloaded 963 times

I do have the M3 command in place. With the attached code the laser comes on upon first move then off at first rapid and never comes back on.
Thanks in advance for all the help you guys are giving. I cant do it alone.

[sngatlanta]

I found the problem. I needed the following in the PP
+---------------------------------------------------
+ Commands output for rapid moves
+---------------------------------------------------

begin INITIAL_RAPID_MOVE
"M11"
"G0[X][Y]"
"G0[Z]"

begin RAPID_MOVE
"M11"
"G0[X][Y][Z] "

+---------------------------------------------------
+ Commands output for the first feed rate move
+---------------------------------------------------

begin FIRST_FEED_MOVE
"M10"
"G1[X][Y][Z][F]"

Thanks everyone so far. I may need help on the "Q" commands but right now it working.

[sngatlanta]

OK laser is set up and working, installed alongside the spindle. I have never worked with a second "head" so to speak.
Do I set up an offset to make the laser go to x0,y0?

I've never set up an offset so I may need some help.

The laser is +.25 from spindle in the X direction and +2.25 in the Y direction.

[dezsoe]

If you have your X and Y zeroed to your workpiece then you can apply a temporary offset by

Code: Select all

G52 X-.25 Y-2.25

and when you finished with the laser, just reset G52 with

Code: Select all

G52 X0 Y0

[sngatlanta]

When using the laser power off the spindle (VFD), because the laser output needs (for security) M3 to be turned on and you don't want your spindle to run.

... or run two profiles... one for milling .... one for laser, that way M3 can be assigned for other pins in the different profile

I set up a second profile for the laser. I coppied all the settings to a new profile and everthing was good. Then assigned my M3 to pin 3 port 3 as needed for the laser. Now when the machine is idle and the spindal is off the laser comes on. When I run a file it goes off then operates as needed. At the end of the file it comes back on. What am I missing?