2012-08-06 15:52:15 (CET)

Nominal Path Contour

When the contour is a nominal path contour (the path a tool with exactly the intended diameter would take), the tool path is described in the NC program. It is expected that (except for during the entry moves) the path is intended to create some part geometry. The path may be generated manually or by a post-processor, considering the part geometry which is intended to be made. For the Interpreter to work, the tool path must be such that the tool stays in contact with the edge of the part geometry, as shown on the left side of Figure A-1. If a path of the sort shown on the right of Figure A-1 is used, in which the tool does not stay in contact with the part geometry all the time, the Interpreter will not be able to compensate properly when undersized tools are used. A nominal path contour has no corners, so the simple method just described will not work.


For a nominal path contour, the value for the cutter diameter in the tool table will be a small positive number if the selected tool is slightly oversized and will be a small negative number if the tool is slightly undersized. If a cutter diameter value is negative, the Interpreter compensates on the other side of the contour from the one programmed and uses the absolute value of the given diameter. If the actual tool is the correct size, the value in the table should be zero. Suppose, for example, the diameter of the cutter currently in the spindle is 0.97, and the diameter assumed in generating the tool path was 1.0. Then the value in the tool table for the diameter for this tool should be -0.03.


The nominal tool path needs to be programmed so that it will work with the largest and smallest tools expected to be actually used. We will call the difference between the radius of the largest expected tool and the intended radius of the tool the "maximum

radius difference." This is usually a small number.


The method includes programming two pre-entry moves and one entry moves. See Figure A-4. The shaded area is the remaining material. The dashed line is the programmed tool path. The solid line is the actual path of the tool tip. Both paths go clockwise around the remaining material. The actual path is to the right of the programmed path even though G41 was programmed, because the diameter value is negative. On the figure, the distance between the two paths is larger than would normally be expected. The 1-inch diameter tool is shown part way around the path. The black dots mark points at the beginning or end of programmed moves. The corresponding points on the actual path have not been marked. The actual path will have a very small additional arc near point B unless the tool diameter is exactly the size intended. The figure shows the second pre-entry move but not the first, since the beginning point of the first pre-entry move could be anywhere.


First, pick a point A on the contour where it is convenient to attach an entry arc. Specify an arc outside the contour which begins at a point B and ends at A tangent to the contour (and going in the same direction as it is planned to go around the contour). The radius of the arc should be larger than the maximum radius difference. Then extend a line tangent to the arc from B to some point C, located so that the length of line BC is more than the maximum radius difference. After the construction is finished, the code is written in the reverse order from the construction. The NC code is shown in Table A-2; the first three lines are the entry moves just described.


Table A 2 NC program for Figure A-4

N0010 G1 X1.5 Y5 (make first pre-entry move to C)

N0020 G41 G1 Y4 (turn compensation on and make second pre-entry move to point B)

N0030 G3 X2 Y3.5 I0.5 (make entry move to point A)

N0040 G2 X3.5 Y2 J-1.5 (cut along arc at top)

N0050 G1 Y-1 (cut along right side)

N0060 G2 X2 Y-2.5 I-1.5 (cut along arc at bottom right)

N0070 G1 X-2 (cut along bottom side)

N0080 G2 X-2.9 Y0.2 J1.5 (cut along arc at bottom left)

N0090 G1 X1.1 Y3.2 (cut along third side)

N0100 G2 X2 Y3.5 I0.9 J-1.2 (cut along arc at top of tool path)

N0110 G40 (turn compensation off)


Figure A 4 Cutter radius compensation entry moves

Cutter radius compensation is turned on after the first pre-entry move and before the second pre-entry move (including G41 on the same line as the second pre-entry move turns compensation on before the move is made). In the code above, line N0010 is the first pre-entry move, line N0020 turns compensation on and makes the second pre-entry move, and line N0030 makes the entry move.