Tips for Cycle Time Reduction: Spindle/M-Spindle

Time, in the manufacturing world, is a constant rate we use to measure how productive we are; we design buildings, machines, and processes to help us do more in a given amount of time. In the machine tool world, we increase production with automation, multiple turrets and pallets, and faster spindles and acc/dec rates, to name a few. Below, I will highlight a few ways to increase production on your current Okuma CNC lathe using “Cycle Time Reduction” on the OSP-P300L/P300S control, without spending a dime on hardware!

Here are a few tips from the OSP-P300L/P300S(LP) Operator’s Handbook to help save time when spindle/M-spindle commands are given.

1. Spindle rotation and turret indexing can be performed simultaneously
   By issuing a T command and an M03/M04 command on the same line, you can index the turret and begin spindle rotation at the same time, reducing cycle time.
   
   Example 1:
   
   G97 S1000 M03 T010101
   
   
2. M63: “Ignoring spindle rotation M code answer”
   Adding M63 to the end of a block will ignore the spindle/M-spindle answer signal and allow the spindle/M-spindle rotation and feed axis operations to be performed simultaneously.
   
   Example 2:
   
   Instead of:  G97 S3000 M03
                        G00 X100 Z200 
   
              Use:  G00 X100 Z200 G97 S3000 M03 M63
   
   Additionally, M63 can be used to perform operations during the waiting time for the spindle to reach a specified speed, such as when retracting the turret to change tools and increasing the spindle speed from 1000 rpm to 3000 rpm for the next tool or operation.
   
   Example 3:
   
   G97 S1000 M03 T010101
   …
   G00 X100 Z100 S3000 M03 M63
   T020202 …
   
   NOTE: By default, M63 only ignores the spindle/M-spindle answer signals for the commands given on the same block or line. To change M63 to be modal, go to the OPTIONAL PARAMETER – OTHER FUNCTION screen and change “M63 command effective by 1 block” to “modal” (see Figure 1).

3. If using M63 as modal, it can be cancelled with the M57 command and a change in spindle direction or speed. For rapid moves, M57 must be on the same block. For feed moves, M57 can be on the same block, or a block before the feed move, and the answer signal will be considered for a single instance, then modal M63 continues afterward.

4. M61: “Ignoring fixed speed arrival in constant speed cutting”
The answer timer for constant surface speed can be ignored so that the next block is performed during the acceleration of the spindle which will help save time as well as prevent marks on parts due to a stop in the axis feed motion. M61 is modal, therefore only needs to be commanded once per program, and it can be cancelled with M60.

Example 4:

G96 S850 M03
G02 X10 Z20 L2.5 M61
G02 X0 Z25 L1.5

These three useful tools will help reduce your cycle time when you’re giving commands to your spindle/M-spindle. If you make a habit of using these techniques safely, all the seconds saved will certainly add up over time. Similar techniques can also be used when indexing the turret, within fixed and LAP cycles, and when using a loader. I’ll cover these techniques in future blog posts, but feel free to comment below or ask questions in the meantime.

Cooper Ferguson is Applications Engineer, Okuma America Corporation.

Please Note: As with any parameter setting, G-code, or M-code, improper use can result in “troubles, losses or damages.” Take all possible precautions when using cycle time reduction techniques.