Hello Guest it is October 26, 2021, 10:05:25 AM

Author Topic: spindle pause  (Read 985 times)

0 Members and 1 Guest are viewing this topic.

spindle pause
« on: February 19, 2019, 12:21:31 PM »
hi all,    i'm having trouble with the spindle starting and at about 20% it starts making the first XY movement
before spindle fully starts. if i start at Z zero, it scratches the stock. and it has a Z movement BEFORE XY
in the control configuration, spindle, checked = wait on spindle to stabilize to 95 percent. (was 90%)
spindle override delay; 1500ms ... (was 500ms)
THANKS for any help !

Mach4hobby ver. 4.2.0.4082

%
O0100
(PROGRAM NAME - SQUARE.NC)
(DATE - WED. 02/13/2019 ,TIME - 12:18PM)
(POST -  Mach3 )
(TOOL LIST)


T1 (1/8 FLAT ENDMILL - STANDARD)
G90 S4200 M03
G00 Z.2
G54 X0.1875 Y-0.1875
M08
Z0.2
Z0.1
G01 Z-0.1 F4.
Y-1.0625
X1.0625
Y-0.1875
X0.1875
G00 Z0.2
Z0.25
M05
M09
G90 Z0.2
G00 X0 Y0
T1
M30
%
« Last Edit: February 19, 2019, 12:34:29 PM by Kenneth »
Kenneth
Re: spindle pause
« Reply #1 on: February 19, 2019, 01:29:20 PM »
Hi,

Quote
in the control configuration, spindle, checked = wait on spindle to stabilize to 95 percent. (was 90%)

Do you have a spindle index signal?

This setting works only if you have such a signal.

How does Mach know what speed the spindle is doing? It can't know unless there is a feedback signal called an
index signal. A lot of people use either an optical device and a disc with a slot or a Hall device and a button
magnet to generate a pulse once per spindle revolution. That signal is applied to your controller.

Mach measures the time between pulses and can therefore tell the spindle speed.

Craig
My wife left with my best friend...
     and I miss him!
Re: spindle pause
« Reply #2 on: February 19, 2019, 01:56:52 PM »
i'm sorry, should have explained more.
i had the machine over and controller over 5 years now.
everything was working in machine 3. when i installed mach4hobby,
i worked on the motor calibration and got all that working.(in mach4hobby)
the spindle was working as should but i upgraded to mach4hobby 4.2.0.4082
and now spindle not pausing. Thanks joeaverage

p.s. at no time do i mess with the wiring of any kind.
and i'm sorry but i don't know anything about the wiring unless
i ask the manufacturer.
« Last Edit: February 19, 2019, 02:10:21 PM by Kenneth »
Kenneth
Re: spindle pause
« Reply #3 on: February 19, 2019, 02:23:26 PM »
Hi,
so you don't know if your spindle has a feedback pulse?

If you don't know, and you would know because you would have to set up the pulse input to your
controller, then I'm guessing that you dont have one. Therefore the 'Wait until (percentage)' setting
is total irrelevant UNTIL you provide it with a signal.

Craig
My wife left with my best friend...
     and I miss him!
Re: spindle pause
« Reply #4 on: February 19, 2019, 02:26:10 PM »
Hi,
in absence of an index signal you are going to have to increase the delay until the spindle accelerates up to speed.

Craig
My wife left with my best friend...
     and I miss him!
Re: spindle pause
« Reply #5 on: February 20, 2019, 06:34:24 AM »
Thanks joeaverage, i tried 25000ms(started at 25ms) with no noticeable stopping.
i'll have to contact the manufacturer.
Kenneth
Re: spindle pause
« Reply #6 on: February 20, 2019, 04:15:07 PM »
Hi,
is it possible to induce your post to include a specific (Gcode) delay into the Gcocode job?

For example instead of just:
m3....
have the post insert a delay like:
m3
g4 p2500....
for example.

Craig
My wife left with my best friend...
     and I miss him!
Re: spindle pause
« Reply #7 on: February 20, 2019, 06:34:18 PM »
yes i can do that. THANKS
didn't think of that but that is why i'm here :)
Kenneth
Re: spindle pause
« Reply #8 on: February 20, 2019, 07:21:35 PM »
Hi,
I use a program utility that converts PCB artwork into Gcode for isolation routing. One of the settings I can make
is to assign a spindle acceleration time. I specify 3 seonds for my spindle and this is an excerpt of the code it
produces:

Code: [Select]
N00000 G21
N00010 (Absolute Coordinates)
N00020 G90
N00030 G00 X0.0000  Y0.0000 
N00040 M03
N00050 G04 P3.000000
N00060 G00 Z1.0000 
N00070 G00 X66.5519 Y18.1959
N00080 G01 Z-0.4600 F100 

Note line N00050  is the delay instruction. To my knowledge most if not all CAM, or more precisely CAM posts allow
such a setting.

This is one approach, namely have the delay expressed explicitly within the Gcode.

Another approach is to have Mach wait until the spindle is up to a percentage of its ultimate speed. That requires
Mach to have some feedback from the spindle to measure its speed. You do not have that facility evidently.

Yet another approach is to have Mach wait on a signal from the VFD (or speed controller) that indicates that the spindle
is up to speed. Many VFDs have programmable monitoring outputs including two of use in this regard.
Mach itself has two input signals defined (ISIG_SPINDLE_AT_SPEED and ISIG_AT_ZERO) that allow you to utilize that
method if you wish.

The first method is as old a Gcode programming itself and one I use extensively.

For automatic control the second method, namely spindle feedback, is very convenient and accurate. Machs core already has
all the code it requires but it does require an index or encoder signal from the spindle. Depending on your spindle this may or
may not be possible.

For example my highspeed (24000 rpm, 750W) spindle has an enclosed fan and would require me to break open the fan housing
to get to some rotating part to which I could attach an index sensor. This spindle is a high quality German made spindle and
I have no intention of digging it open for a sensor. A simple Gcode delay or using signals from the VFD are more than adequate.

My high torque spindle (1.8kW 6.2Nm 3500 rpm AC servo) however has programmable outputs to which I can assign
either/or an index pulse derived from the actual encoder or one (or even both) of the quadrature channels. So there is no need
to dig into the back of the servo thus the feedback method is as simple as programming the servo drive and running a wire
to an input on my motion controller.

A simple delay is adequate for most purposes. If you were in a production environment you might think otherwise.
Lets say at least one of your tools, a facing tool or boring head, takes 3 seconds to spin up to speed. If however you picked
an endmill it would spin up in 2 seconds. Thus if you programmed your post to allow 3 seconds delay on each spindle start
then there will be occasions when the machine is waiting unnecessarily instead of producing chips and making money.
Thus the demands of business, or lack thereof, will determine the effort and expense that you will devote to the issue.

Craig
My wife left with my best friend...
     and I miss him!
Re: spindle pause
« Reply #9 on: February 21, 2019, 07:20:28 AM »
i inserted the pause in the post and it works great ! 
Thanks Craig
Kenneth