Feedrates and accelerations (fine tuning for Routers with AC Servos)

[Insect]

Hi,
I have noticed that small pocket maneuvers in my gantry router are running slower than the specified feedrates (based on CNC12 display and observation). This is not surprising as acceleration due to physics or normal CNC control will slow down for intricate work, sure... but the following puzzles me.

Understand the following Gcode test file for the following: it does a helical ramp, then a larger one, then a larger one, all set to 1500mm/min.

If I set the accel to 0.2 in the wizard, the attached Gcode will start at 1000 mm/min despite being ordered to 1500. If I set it to a higher value, 0.27, etc, it's the same. If I turn up the feedrate on the control to 180 it increases, so I am not hitting an absolute value within Centroid to no accelerate past ~1000 on these tight arcs if feedrate increases in control actually occur. I also played with the Par 231, saw no change at all.

When the Gcode goes to the larger helical moves it follows the commanded 1500.

The machine runs clearpath servos, but I am reading the display on CNC12, so whether CP is doing some third derivative stuff to slow it further is not relevant to this level of analysis.

Please enlighten me, thanks!

[Nigelo]

I'm guessing but worth checking your Smoothing settings

[suntravel]

Look at Parameter 49-51 in the manual.

Uwe

[Insect]

Uwe, thanks, but my parameters 49-50-51 were all zero. So it must be something else. Smoothing is off also

[cnckeith]

put any parameters you changed back to the stock settings and then adjust delta v max values. Delta V max is conservatively set to a default value that works well with all typical milling machines and routers. With a router sometimes you can speed/loosen things up with a higher delta vmax number. delta vmax is = The maximum instantaneous velocity change that will be commanded on a vector transition. if you have open loop steppers do not adjust this number. if you have AC servos sized properly for the machine you may proceed.

with delta v max set to 127 mm/min from your report amd using your provided g code program; my machine would run the smallest helix around 880 mm/min and the medium size one at around 1200 mm/min and the big one around 1490 mm/min,

i changed delta v max to 200 mm/min for all axes and re ran the job and now it runs the smallest helix around 1200 mm/min and the medium size one at around 1480 mm/min and the big one around 1500 mm/min

in practice adjusting delta v max is a bit of a trial and errror process, but i have succesfully gone up to 380 mm/min on delta v max setting for a few routers with good results. I would only increase this number just to the point where you are satisfied, no need to make it bigger than needed as that would introduce other issues.

[Insect]

That seems helpful and is informative, now, how do I change a user variable such as the 20900x series you are mentioning?

I understand user variables are written as subjects of the code, M functions, etc, but where do I change this one directly?

Thanks,

[cnckeith]

delta v max is set in the jog menu of cnc12,
F1 Setup, F3 Config, type in password "137", F2 Mach, F1 Jog

[suntravel]

Code: Select all

;------------------------------------------------------------------------------
; Filename: mfunc55.mac - To run from VCP AUX 10 key, set p197 = 5511
; M55 macro
; Description: Calculate Vfc for internal thread milling or circ. pockets
; Requires: Machine home must be set prior to use.
; Please see TB300 for tips on writing custom macros.
;------------------------------------------------------------------------------

IF #50010                        ;Prevent lookahead from parsing past here
IF #4201 || #4202 THEN GOTO 1000 ;Skip macro if graphing or searching
#105=0
N100
M224 #101 "Calculate Vfc for\nint. thread milling\nor circ. pockets\n\nMill Diameter"
M224 #102 "Bore Diameter" 
IF #101 >= #102 and #105 == 0 THEN GOTO 900 ELSE GOTO 110
N110
IF #101 >= #102 and #105 >= 1 THEN GOTO 990 ELSE GOTO 200
N200
M224 #104 "Feedrate Vf"
#103=#104/((#102*3.14)/((#102-#101)*3.14))
M225 #100 "Use for:\nMill Diameter: %f mm\nBore Diameter: %f mm\nFeedrate Vf: %f mm/min\n\nCalculated Feedrate\nVfc= %f mm/min" #101#102#104#103
GOTO 1000
N900
M225 #100 "Mill Diameter = %f\n can not be equal or larger then\nBore Diameter = %f\n\n Back to Start" #101#102
#105=1
GOTO 100
N990
M225 #100 "Really?\nThis will also not fit\n\nMill Diameter = %f\n can not be equal or larger then\nBore Diameter = %f\n\n Back to Start you Stupid" #101#102
GOTO 100
N1000                            ;End of Macro

For small circular pockets it is better to reduce Vf, because Vfc will be much higher.
Here is a macro to calculate this, I have this as a button on my VCP.

Uwe

[Insect]

Thanks, solved. I ended up with values of 280, Accel of 0.22,
and deadstart 220. It works there, sounds high, but is well controlled for now.