Dear Shop Doc,

We need to make multiple passes back and forth to clean a part, but we need to compensate for brush wear. Cutter compensation has so many stops and starts and weird movement limitations regarding rotation direction and feed direction. There has to a better way.

Done Compensating

Dear Done,
I too have experienced irritation when dealing with cutter compensation. There may be another way, but it depends on your machine.

Some machines have what are called “common variables.” They are variables you can use for part counting, tool life tracking, or other uses. How the machine uses these variables is defined by the program.

I used variables in a similar situation on a RoboDrill machine with a Fanuc control.

My repetitious move was to be along the X axis, so I needed to define the location of the surface on the Y axis. This was programmed in a G57. If I called up the G57 and Y zero, the machine would bring the wheel to a location where the edge of a new wheel would lightly touch the part surface if moved across the part. When the brush wears, it no longer performs adequately.

To compensate for the change in wheel diameter we need to modify the Y position. I chose to use variable 514 for the wear compensation. In the following program excerpt, the program calls up the work shift, subtracts wear value 514 from the Y zero position, stores the result in 524, then moves the part to the new Y location stored in 524. Using the variable in this manner allows the machine to move in both the X+ and X- directions without stopping the spindle. This method can be used for any side of the part with minor changes to the program and math.

G57X0Y0
#524=0-#514
Y#524
G0Z-30.0
G1X100.0 F250.0
X0
X100.0
X0
X100.0

There are some risks involved with this method. For example, if a mistake is made when entering the value into the variable cell, a machine crash could result. An easy solution to this problem is to have the program check the value of the variable against a predetermined min/max value before making any tool move.
In the program example below, the value in cell 514 is checked to make sure it is between zero and 7.01. If the variable check is false, the program jumps to block 778, which stops the program and prints the following message to the screen: #514 OUT OF RANGE

Locate near top of program:
IF[#514GT7.01]GOTO778
IF[#514LT0]GOTO778

Locate after the M30:
N778#3006=1(#514 OUT OF RANGE)

The method as detailed above requires the machine operator to maintain the proper amount of variable value required for acceptable performance results. An automatic method is also possible, but only if the tool wear is predictable and consistent. In the example below, the value in cell 514 is incremented by 8 microns each time the program runs. The increment value can be whatever the expected wear-value per part is. This method also allows the machine operator to override this value by changing the 514 value manually.

#534=#514+.008
#524=0-#534
#514=#534
Y#524

The common variables and math functions can be used for many things. Read your machine manual or contact your machine service company for more information on your machine.

A longer more detailed version of this “Shop Doc” can be found at www.todaysmachiningworld.com.

Mark Bos
Robert Bosch Fuel Systems

Mark Bos is a manufacturing process engineer with Robert Bosch Fuel Systems in Grand Rapids, Mich.

Dear Shop Doc,

We have a machine that occasionally frustrates us to no end. Sometimes a dimension goes out and we can’t get it back unless we touch all the tools off again. Then it works fine. I’ve had it, I’m almost ready to sell the machine. Can you help?

Touched-off in Dayton, Tenn.

Dear Touched-Off,

I’ve had similar experiences with CNC machines. Normally, when the wear offset value is adjusted, the dimension on the part closely follows the offset change. Life is good when this is happening. Unfortunately, I’ve had some experiences when it didn’t work quite this way because certain offset changes led to a condition where there was not enough material to make the complete part. Basically, I’m referring to a non-cleanup condition, which can be difficult to detect on parts made from a solid bar.

My most-recent experience with a similar problem was on a Takisawa lathe. It cut the OD and right end of the part from a bar, then the pickoff spindle moved over, clamped the part, fed the bar out for the next part, cut the part off the bar, and returned home to finish the part ID and left end.

After a relatively new operator had been running the machine for a few hours and making miscellaneous offset adjustments, he ended up in a situation where he couldn’t bring a specific dimension back in. The offsets, which were supposed to control the surface, no longer had any effect. He had no idea what he did to make this happen and attempts at resolving the situation made things worse.

Working with a more experienced operator, we inspected the tools in the machine to make sure none had built-up edges or other problems. They were all fine. Next, we tried to paint the end of the bar with layout dye and verify that the tool was actually cutting the part. We found that it wasn’t even touching it anymore. This was an example of the proverbial “I keep cutting it, but it’s still too short.”

The machined surface on the end of the part was the same surface that was left over from the previous part cut-off. The bar was no longer coming out far enough to allow for full clean-up of the surface.

To find out why, I looked at the program to determine how far the bar was fed after cut-off and calculated how much cleanup stock was available on the ends. The total cleanup stock was only 0.335 mm, or about .0065” per end. It was small enough to increase the chances of this problem occurring.

As it turned out, the operator had made a Z- change to the cut-off location. By making this change, he actually reduced the bar protrusion past the main spindle. The machine relied on a certain amount of bar-length from the main spindle to ensure enough clean-up stock on the right side of the part.

The solution was to simply move the cut-off tool 0.2 mm in the Z+ direction, which allowed a full cleanup of both ends of the part.

In this example, the problem was with both the roughing and finishing tools. I have seen other instances where the rougher removed too much material and the finisher didn’t have enough clean-up stock remaining.

A relatively inexperienced operator may not have had a full understanding of how the program and machine functioned.
The problem of too little clean-up stock can be fixed easily, as can creating some type of visual reference for the operators to use.

If you are having this type of problem with your dimensions and wear offsets, pull out the layout dye and make sure the tools are actually cutting the surfaces as intended. Give the operators training on how to identify and remedy this situation. Make some changes to the program to reduce the chances of this problem occurring.

Mark Bos
Robert Bosch Fuel Systems

In today’s difficult economy, we are all trying to make parts faster and cheaper. Unfortunately, making parts faster is sometimes at odds with making them cheaper.

I have learned from experience that sometimes a machine will consume less money if you slow it down a little and try to find the proverbial “sweet spot.” The fastest spindle speeds and the highest feed rates may not be the best way to run the machine. It may be difficult to convince your boss that this is true, but having real data to prove it can be helpful.

Tooling costs or machine repair costs are examples of costs that could go up significantly if the machine is pushed too hard when trying to reduce cycle time. When I get involved in a process, I like to track tool life. If I don’t know what my tool life was before I make a change, I can’t accurately measure the performance gains or losses caused by the change. I always share my tool log results with the machine operator, as part of his or her involvement in the process improvement.

The following is a good example of slowing a machine down to get better performance. The part was made on an Index ABC lathe. This machine was plunge-roughing the OD of a cylindrical part made of 8620 steel, using a .3” wide carbide insert-type OD roughing tool. The tool had problems with durability. The average tool life for this tool was little more than 200 hits per edge. When the edge went bad, it happened quickly and would cause problems for the finishing tool that followed it. This roughing tool is one of 11 tools used to make this part on this machine.

The first thing I checked was feeds & speeds. The actual surface speed for the roughing tool was 1100 ft/min, while the recommended surface speed range, per the insert manufacture’s catalog, was 250 to 600ft/min. After reducing the spindle speed by 50 percent to obtain a more suitable surface speed, I steadily increased the plunge feed rate to a value 60 percent higher than it was. After these adjustments the chips curled up tightly, with a nice sizzle when they came off.

The net effect of my changes on the cycle time was an increase in cycle time of less than 1 percent. I was lucky that I was nearly able to completely compensate for the decrease in surface speed by increasing the feed rate.

The tool life results went from little more than 200 hits per edge, to more than 1200 hits per edge. This resulted in a $330 reduction in tooling costs per month. Additionally, we reduced tool change time by 15 minutes per week.

This was a time where a slower cycle time actually enabled me to make similar quantities of parts per month and reduce tool usage costs. If someone forgot their machining 101 lessons, there may be room for improvement.