Cycle Programming

Some parts are a list of holes: a drilled plate, a bolt circle, a grid of tapped holes.

Cycle Programming lets you type that list instead of taking it through CAM. You say how the hole is made and where the holes are; the control writes the program. When you save, it becomes an ordinary NC program. It shows up in the program list and runs, single-blocks and searches like any other.

This is the panel form. If you are writing the cycles by hand in G-code, that is Canned Cycles.

How a program is built up

Two kinds of block, in the order they will run:

• A cycle says how a hole is made: tool, depth, feed, speed.
• A pattern says where: a list of points, a line, a grid or a circle.

Patterns belong to the cycle above them. Add a cycle, hang one or more patterns under it, then add the next cycle for the next tool.

PROGRAM        work offset, retraction plane, return mode
  DRILL        6.8 mm, 12 deep, T3
    POINTS     4 holes you typed
    LINE       6 holes in a row
  TAP          M8, T5
    GRID       3 × 4 holes
END

Holes are cut in the order you entered them. The control never rearranges your work to save a tool change. If you put the drill before the tap, that is what runs.

Writing one

1. NEW PROGRAM, then tap the CYCLE / UNNAMED bar at the top and give it a name.
2. Select PROGRAM in the list and set the three header values (below).
3. + DRILL or + TAP, then fill in the fields on the right.
4. + POINTS, + LINE, + GRID or + CIRCLE, then give it its geometry.
5. Repeat 3 and 4 for the next tool.
6. SAVE PROGRAM. The line under the keys tells you which program it became.
7. LOAD sends that program to the machine, ready to start.

DELETE STEP removes whatever is selected. CLOSE asks first if you have unsaved changes.

The picture in the middle updates as you type. Holes are drawn at their real diameter, tapped holes are marked, and the line between them is the order the tool will travel. A radius typed as 500 instead of 50 is obvious there straight away.

The header

Select PROGRAM to set the three things that belong to the part:

Setting	What it does
Work offset	G54 … G59, the datum the coordinates are measured from
RP Retraction plane	how high the tool sits between operations
Return mode	G98 lifts to the retraction plane between holes, G99 only to the R plane. Use G98 if there is a clamp in the way

Everything is in millimetres. The mm badge on the name bar is there to say so.

The cycle fields

Field	What to enter	Unit
TOOL	the tool that cuts these holes	tool number
DIA	hole diameter; this is also what the picture draws	mm
DEPTH	how deep the hole is. Enter it as a positive number	mm
R PLANE	how far above the surface the tool starts feeding	mm
F	feed	mm/min
SPEED	spindle speed	rpm
PECK	peck depth. Leave it empty to drill in one go	mm
DWELL S	pause at the bottom of the hole	seconds

Enter depth as a positive number: 12 mm deep is 12, not -12. You are describing the hole, not the direction the tool moves.

The fields choose the drilling cycle

You do not pick a cycle from a menu. What you type decides it:

What you entered	What runs
a DRILL, nothing extra	G81, straight drilling
a DRILL with DWELL S	G82, drill and pause at the bottom
a DRILL with PECK	G83, peck drilling
a TAP	G84, tapping

The selected block shows which one you got, like DRILL (G83). Filling in a peck depth is what makes it a peck cycle, so there is nothing else to switch on.

The patterns

Pattern	You enter
POINTS	each X and Y in a table. ADD POINT adds a row, DEL POINT removes the selected one
LINE	start point, direction angle, spacing, how many
GRID	start corner, spacing and count along X, spacing and count along Y
CIRCLE	centre, radius, start angle, how many holes

Patterns are a way of entering positions quickly. Once the program is saved, a circle is stored as the holes it produced. Reopen it and you will see the points, not the circle. Change one and you re-enter the pattern.

After you save

Saving writes a normal NC program. You can open it in the editor and read it, and it is plain G-code:

O17 (COVER PLATE)
G17 G21 G40 G80 G90
G54
G80
T3 M06
G43 H3
G00 Z120.
S2000. M03
G98 G83 Z-12. R2. Q3. P0 L0 F250.
X10. Y20.
X30. Y20.
G80
M05
G00 Z120.
M30

If you edit that program by hand, the panel will no longer show it as a form. It tells you so and opens it in the editor instead, rather than showing you a tidy form that no longer matches what the machine is going to run.

What the machine already knows

Coolant, how the tool length is applied, and the exact shape of the program above are not yours to set here. They come from a setting that belongs to the machine, and your machine builder chooses them once.

That is also why the fields on your machine may differ slightly from the list above. If your machine has a rotary axis that can tilt the part, you will see an extra angle field; a three-axis mill does not show one, because there would be nowhere to put it.

Limits of this screen

• Tapping needs a compensating (floating) tap holder. The cycle feeds in, reverses the spindle and feeds back out.
• Drilling and tapping. Boring and reaming are not offered on this screen; write them as Canned Cycles.

Where to go next

• External Program Selection: pick the program by scanning a label instead of finding it in the list.