Cycle Time Reduction takes an already existing, running program and speeds it up by eliminating non-value-added time. The software evaluates the program and eliminates anything that can help make up time without affecting the actual cutting process. This means more cutting time and more profit for your shop.
One of Okuma’s most underutilized technologies–Cycle Time Reduction. The intent of utilizing cycle time reduction is to take an already existing, running program and speed it up by eliminating non-value-added time. The software evaluates the program and eliminates anything that can help make up time without affecting the actual cutting process.
For example, if you were to program the spindle at 10,000 RPM, normally the axes will not begin moving until the spindle confirmation shows 10,000 RPM. That could be anywhere from three to five seconds of lost time with the use of cycle time reduction codes, the axes will start moving before the spindle hits 10,000 RPM. By the time the spindle gets to the part, it will have hit 10,000 RPM, and there was no wasted time in the process.
It might sound small, but saving seconds for each tool can add up to a lot. With the easy setting version, you’ll just make some selections from a menu, and the machine will automatically speed up wherever it can.
You also may not need cycle time reduction in every instance. If your program mainly involves cutting with very few tool changes or canned cycles, there will be limited areas for the software to speed up your process. This functionality is best suited for when you have multiple cutting tools, canned cycles, or the parts travel a considerable distance. With the easy setting version, you’ll make a few selections from a menu, and the machine will automatically speed up wherever it can.
Okuma’s cycle time reduction is easy to use and in most cases can save you valuable time and money.
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.
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.
G97 S3000 M03 G00 X100 Z200
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.
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).
Cycle time reduction part 1v2
3. M57 command
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.
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.