what do you enter in your machine offset if you run G41 and the program follow actual path the diameter or radius?
Hello M Code,
In theory, a Zero Value would be registered, but because of tool run-out, tolerance of the diameter of the cutter and tool spring, its common to have some small value, either plus or minus, to adjust the size of the feature.
When using Centre Line of Cutter, plus TNRC (G41/G42) and when running a part program for the first time, or with a change to a new tool, it's common practice to add a small positive Tool Radius Comp value so as to not cut the part out of tolerance. In this case, the feature is measured and the small Tool Radius Comp value adjusted to cut the feature in tolerance.
The same Tool Radius Compensation interference errors exist with programming centre of tool and using small values in either Tool Radius/Diameter, or Tool Wear specifications. as exists when programming using the Work-piece coordinates and full radius tool Radius/Diameter specified.
Lets say that a Concave Radius Feature has a radius close to that or the cutter being used. Its common and prudent to use the biggest cutter that the geometry of the part will permit (to minimize push off of the tool). So, in this example part, there is a concave feature of 10.15 radius and the cutter being used is diameter 20.0. If a Wear or Geometry TR Comp radius of 10.15 or greater (when part coordinates programming is employed) so as not to cut the overall feature out of tolerance, a TNRC Interference alarm will be raised.
Similarly, if Centre Line programming was being used, with a 10.0mm radius cutter specified when creating the program, the Concave Radius feature will now appear in the program as a 0.15 radius Concave Feature. If a TR Comp value of 0.15 or greater is used, the same TR Comp alarm will be raised as in the example using Part Coordinate programming.
When using Centre Line programming, plus TR Comp, the TR Comp value can become a Minus Value when adjusting the size of the feature. When Minus Values are used as the TR Comp value, the TR Comp "G" Code is effectively flipped; the Control sees G41 as G42 and visa versa.