In the May Tech Talk column, I discussed a method of determining cutting motion time in a program. A certain amount of cutting motion time is air cutting time. This occurs when the cutting tool moves from its approach position until it contacts the workpiece. It is also time when the tool feeds off a surface until it reaches a safe clearance position.
Most programmers use a standard feed-off distance of 0.100 inch (or 2.5 mm). If you performed the test in the May issue, you may have been surprised at how much cutting motion time is air cutting time. Consider center drilling 50 holes on a machining center at 5.0 inches per minute. If you are using a rapid approach distance of 0.1 inch, there will be 5.0 inches of air cutting motion in the program (50 holes times 0.1 inch). At a feed rate of 5.0 inches per minute, this equates to 1 minute of air cutting time. Next, the holes must be drilled. After that, there may be more operations on these holes (counter boring, tapping, reaming or other operations). If each of these tools uses a 0.100-inch rapid approach distance, then at least five more inches of air cutting time will occur per tool.
While 0.100 inch is a safe rapid approach distance, you must consider the impact it can have on air cutting time. There are times when 0.100 inch may be an excessive rapid approach distance, at least when the surface the tool is approaching is qualified and when the tool being used has been accurately set. By qualified, I mean that the surface is not varying by much. Perhaps the surface has been machined (varying by less than a few thousandths of an inch), or the surface has been cold drawn (varying by 0.005 to 0.010 inch). Possibly, the tool has just machined one surface and is about to machine another.
In these cases, you can safely reduce rapid approach distance. Make your rapid approach distance about ten times the total of the surface variation amount plus the total possible imperfection in tool setting. For example, if the surface is varying about 0.003 inch and the cutting tool setting could vary by as much as 0.002 inch, then a 0.050-inch rapid approach distance should be sufficient.
In the case of the 50 center-drilled holes, this would allow us to cut the rapid approach distance and air cutting time in half. Instead of taking 1 minute, air cutting time will take only 30 seconds (based on the 5.0 ipm feed rate mentioned above).
There are two safety-related points about this technique. First, the surface must be qualified. Don’t try to reduce rapid approach distance for sand castings, forgings or other workpiece blanks that vary from workpiece to workpiece or lot to lot. In these cases, a rapid approach distance of 0.25 inch or more may be necessary. Second, your tool setting positions must be accurate. For machining centers and when approaching in the Z axis (as with hole-machining tools), this means that tool length compensation values must be accurately measured and entered. When approaching in XY (as with an end mill), the cutter cannot be larger in diameter than expected. For turning centers, this means that program zero assignments for each tool must be correctly measured and entered.
Let’s say you have been setting tools accurately. I contend that if you would have started your CNC career using a 0.050-inch rapid approach distance for qualified surfaces, you should have had no problems approaching with cutting tools that you haven’t had using the 0.100-inch rapid approach amount. You have the same program verification functions that you currently use when approaching with a new tool. These include dry run, single block, rapid override, distance-to-go and feed hold. If you’ve had problems with crashes, they’ve probably not been related to the size of your approach distance.
These points apply when you feed a tool away from a surface after cutting. If anything, it will be safer to reduce feed-off distance because the tool is not moving at rapid prior to this motion, and during this motion, the tool is still at its cutting feed rate.
An example of when you can reduce rapid approach distance on turning centers is when you rough face and rough turn with the same tool. Say you rapid the face-and-turn tool within 0.100 inch of the diameter to be faced (on the side). You then face the end of the workpiece to center. Next, you retract the tool 0.100 away from the workpiece in Z. You then rapid the tool straight to the first diameter it will rough turn, maintaining the 0.100 clearance. Finally, you program the tool to rough turn its first diameter. The very tool that rough faced the workpiece is being used to rough turn the workpiece. The variation in the surface being approached (workpiece face) will be next to nothing. Maintaining the 0.100 approach distance for the rough turning pass(es) will be wasteful.blog comments powered by Disqus