M6 Dwell Time

[CNCMaryland]

Back when there was an M6 macro I was able to adjust the dwell time between manual tool changes, so that the spindle had time to spool up before cutting. I am trying to find out how I can do this now easily. Not sure if anyone has a copy of the old M6 command from 4.10.

[Gary Campbell]

Put a "G4 P#", where # = seconds you wish to dwell in the M3 (spindle CW) macro. (maybe the M4 if you use reverse operation)

You need to place it right after the spindle on command

[CNCMaryland]

Thank you very next much!

For anyone else interested, the M3 does not have any delay. Here is the modification to the M3 that I made to add a 10 second delay.

;-------
;M3 macro
; Displays message to select auto spindle mode if it is not set
;-------

IF #4202 || #4201 THEN GOTO 200
M95 /2
M94 /1
G4 P10
IF #61058 THEN GOTO 200 ;skip the check if AutoSpindle is on
G4 P.1
#140 = 1.5
N100
IF !#61058 THEN M225 #140 "Please Select Auto Spindle To Continue!" ;61058 = JPO2/SpindleAutoManualLED
G4 P.5
IF !#61058 THEN GOTO 100
N200

[swissi]

For those using Fusion 360 and need a delay after spindle start to let the spindle rev up before the job continues, you can use my modified Fusion 360 Milling Post Processor that has the property to automatically add a dwell command after each spindle start. The actual dwell time will be calculated based on the demanded spindle speed and can be controlled with a factor that depends on the spindle type.

Check the Post Processor User Manual for more details.

-swissi

[ShawnM]

I also modified my Vectric post processor to add in the delay for the spindle so it comes up to speed before it moves back to the workpiece after a tool change.

And of course added a delay in the beginning of my M6 macro to the tool has time to brake to a stop before it moves to my tool change position. It's not quite as fancy as the Fusion PP but it gets the job done.

[Dan M]

I did the same as Shawn and edited the Vectric PP.

Dan

[Gary Campbell]

I take a different approach. In the VFD parms, set one of the outputs to "Up to Speed" or "At Desired Frequency". Connect to an acorn input. Instead of any G4 dwell time, simply check that input (M100, M101) for the state set in the parms …. and Voila! Never wait again.

[ShawnM]

I take a different approach. In the VFD parms, set one of the outputs to "Up to Speed" or "At Desired Frequency". Connect to an acorn input. Instead of any G4 dwell time, simply check that input (M100, M101) for the state set in the parms …. and Voila! Never wait again.

Hi Gary, this sounds interesting and you forced me to read my VFD manual some more. I have an output that is setup for "frequency reached". In fact it's the default setting for one of the VFD's outputs. And I can set the range from 0-100% as the detection range for the frequency. Meaning I can set it to 90% and when the inverter reaches 90% of the frequency called for it'll provide an output to the Acorn. I would want it to be pretty close to 100% as I want the spindle to at the proper speed when it starts cutting.

Can you give and example of the code needed to "check that input" as you mentioned? I'm interested to try this as it'll save the time that I wait for the dwell even when the spindle is not spinning. Since I have a dwell time in the beginning of my m6 before the first tool change the spindle isn't even spinning when it moves to z0, then it waits 3 seconds before moving to the tool change position. This would eliminate this each time, yes?

Thanks,
Shawn

[Gary Campbell]

Shawn...
Look in the manual for the M100 and M101 commands. You will have to use the one that matches the configuration of the VFD output. and there are syntax examples based on input numbers.

As I stated above, I put the M110/M101 commands in the M3 and M5, not the M6. If the spindle is off, the M5 is a blip on the screen. You can also use "IF (input on or off) THEN GOTO to skip the M5 completely when the spindle is shown as stopped if you have a VFD output set to stopped or zero rpm

[ShawnM]

I did see the examples in the manual. I’ll try to sort out what it means. I know not to use it in the m6, I was just saying that’s where I have a dwell now. I like this idea and will experiment. Just another item on my to-do list.