Need Help!- Adjusting Accel & Decel on spindle drive

[gandp]

Hello again,

I know I'm asking a stupid question here but here goes......I understand your spindle drive will last longer if you can give it more time to ramp up or ramp down. What potentiometers on the drive are the accel/decel? Mine says slow down time and gain but no "accel or decel". Also there is some that says "reference" so I didn't mess with any of it. Also, which way would you turn the potentiometers....CW or CCW to make these adjustments and how much of a turn? Looking in the maintenence manual I cannot find any info so that's why I'm posting this here. Thanks

[cncserveng]

I wouldn't advise messing about with these, if you must, then program the speeds in steps if you feel the need.

Personally, unless you are running flat out non stop up and down, there will be little benefit it doing what you suggest.

[hrh]

Not available and not advised because many settings are "factory" adjusted or adjusted with specific procedures involved.

Try to control the spindle with G96. This will cause the spindle to accelerate "slowly" as the X-axis is moving towards the workpiece and decelerate as the X-axis moves away from the workpiece.

When running in G97, the spindle is required to reach "instantaneous" commanded speed.

[gbowne1]

I use G96 and G97, albeit very carefully.. although I don't use G97 very much. I just use G96 when I want a nice smooth motion.

[angelw]

Originally Posted by hrh Try to control the spindle with G96. This will cause the spindle to accelerate "slowly" as the X-axis is moving towards the workpiece and decelerate as the X-axis moves away from the workpiece.

This is only the case if the move is not in rapid mode. In a block containing a G0 or G00 command, the surface speed is not calculated according to the change in tool position, but on the basis of the end position of the block. As most moves towards and away from the workpiece are made in rapid mode, programming G96 wouldn't alter the acceleration/deceleration characteristic associated with the target diameter.

I agree with cncserveng in that unless the machine is running a program where large variations in spindle speeds were being cycled quickly and often, there will be little advantage in making the acceleration/deceleration less responsive.

Regards,

Bill

[gandp]

Originally Posted by angelw This is only the case if the move is not in rapid mode. In a block containing a G0 or G00 command, the surface speed is not calculated according to the change in tool position, but on the basis of the end position of the block. As most moves towards and away from the workpiece are made in rapid mode, programming G96 wouldn't alter the acceleration/deceleration characteristic associated with the target diameter. I agree with cncserveng in that unless the machine is running a program where large variations in spindle speeds were being cycled quickly and often, there will be little advantage in making the acceleration/deceleration less responsive. Regards, Bill

Thanks everyone,

I forgot to mention I had in mind changing the accel/decels on my drive for my VMC but I haven't done so because there has been no problems here. I just don't run them balls out for there is no need......yet. So basically, what's not broke-don't fix is the suggestion here and I agree. I'm glad I posted and thankful you all responded so well. However, I've had problems on my lathes with spindles ever since running on phase converter so I blame this totally on that respect. I can make parts but I have to be careful with my spindle commands.

Bill, thanks for your reply but not to argue, there is a parameter that I changed (Fanuc 6T) in respect to how the drive reacts to rapid commands in regards to spindle speed in G96. I changed it to look at the actual position instead of anticipated position. I don't remember which one it is but I should post it because my bigger lathe runs very smooth now when I use the G96 command. I would hope anything beyond Fanuc 6 would have this same parameter option.

For Fanuc 6's, the parameter to change is #9 bit #4 (5th from the right) changed it to 0.

[angelw]

Originally Posted by gandp Thanks everyone, I forgot to mention I had in mind changing the accel/decels on my drive for my VMC but I haven't done so because there has been no problems here. I just don't run them balls out for there is no need......yet. So basically, what's not broke-don't fix is the suggestion here and I agree. I'm glad I posted and thankful you all responded so well. However, I've had problems on my lathes with spindles ever since running on phase converter so I blame this totally on that respect. I can make parts but I have to be careful with my spindle commands. Bill, thanks for your reply but not to argue, there is a parameter that I changed (Fanuc 6T) in respect to how the drive reacts to rapid commands in regards to spindle speed in G96. I changed it to look at the actual position instead of anticipated position. I don't remember which one it is but I should post it because my bigger lathe runs very smooth now when I use the G96 command. I would hope anything beyond Fanuc 6 would have this same parameter option. For Fanuc 6's, the parameter to change is #9 bit #4 (5th from the right) changed it to 0.

I like other assumed that it was a lathe control being discussed, as its with a lathe where there is a considerable amount of dynamic braking involved, compared to that of a machining center.

On some controls, and not others, the control looks for a spindle speed confirm signal before executing the next block. Accordingly, when using relatively high spindle speeds, the machine will sit and wait for what seems to be a long time. Its in this circumstance of the spindle going from zero to the high commanded spindle speed, where there is the greatest load on the spindle drive. Its quite common in the case of a control that waits for the speed confirmation, and where a high spindle speed is involved, to obtain the target speed in a couple of steps without any compromise on cycle time. For example, one step after the tool change and another just before the Z approach.

With regards to the CSS calculation during a rapid move, no argument there. There is plenty of reference to a parameter setting for controls pre "O" series; for series 10,11,and 12 its bit 6 of parameter 5602, but from "O" series on there is no such reference and it seems that the CSS is calculated on the target diameter. Perhaps someone else may have some further information on the later Fanuc controls.

Regards,

Bill

[Deltic_Engine]

I don't think there is a G96 option for thoser of us with older controllers.

In that case there is usually a separate 'Spindle Board' in the cabinet that
usually has a few pots on it.
Rather than marked "Accel" the pots sometimes might be labeled 'Current'.

The 'Current' pot literally limits the amps sent to the servo.
This can be a handy adjustment not just to reduce peak loads on the drive train
but can can also help you run a machine without causing power dips
on your building's electrical grid every time the machine starts or stops.

Power dips can cause controller problems not just on the machine in question
but can play havoc with any other electronic device plugged into your building.

I run a 15-hp VMC on only 100-amp HOME service and I owe allot of that
to that "Current Pot' adjustment along with a soft-start controller
that I added for my air compressor.

Jeff Krause
EVA CASES, EVA CASE DESIGN, Custom Protective Cases by Designer Jeff Krause