Centroid Community CNC Support Forum

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!

I'm guessing but worth checking your Smoothing settings

Look at Parameter 49-51 in the manual.

Uwe

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

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 and 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 error process, but i have successfully 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.

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,

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

Deadstart: Determines the speed that an axis will decelerate to before stopping or reversing direction. A low setting
will cause a large slowdown before a reverse in direction, causing your machine to be more accurate. A high
setting will cause less slowdown before reversals, but this may cause your machine to “bang”, which may cause
a decrease in accuracy. This parameter should not be changed

15.3.120 Parameter 165 – Acceleration/Deceleration Options
This is a bit field parameter which modifies certain details of axis acceleration and deceleration when an axis stops
moving, changes direction, or starts moving. The Jog Parameters screen in Machine Configuration sets the original
DeadStart values for each axis. This parameter allows you to modify these DeadStart settings under certain
conditions. Note that if both bit 0 and 1 are turned on (value = 1+2 = 3), then the effect is cumulative, i.e. the net effect
will be that 1/2 of the DeadStart value will be used when a slave axis stops or starts up from a stop. Likewise, if both
bit 2 and 3 are turned ON, the effect will also be cumulative. Note that this feature has no effect for movement
commands handled by G64 Smoothing (P220=1).

other related guidance

Router Vibrations Causes, starting with most common

Router Vibrations / Wobbling causes starting with most common

1.) #1 is undersized servos (servos don't have enough power to hold position with the gearing, weight, speed and inertia involved in the move). Note: a Yaskawa 750 and a Leadshine 750 are not going to perform the same when it comes to power, control and torque at speed.
2.) Mechanical issues excessive backlash present, loose drive pulleys, binding, racking, and sticking issues.
3.) Servos tuned on a machine that has mechanical issues, see #1
4.) Axis Servos not tuned properly (use the drive software tuning first and multiple times and then Centroid delay tune).
5.) Poor quality ratty saw tooth looking G code. unnecessarily short vectors such as vectors .0001 - .0005" long, and or a CNCPC not up to the task if using G64 smoothing.
6.) CNC12 configuration issues.

If and when #1-5 have been thoroughly vetted and ruled out then and only then look to CNC12 setup issues.

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

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.