Cycle Programming

Some parts are a list of holes: a drilled plate, a bolt circle, a grid of tapped holes, a beam drilled on two faces. Cycle Programming lets you type that list instead of taking it through CAM. You say how a hole is made and where the holes are; the control writes the program. Saved, it is an ordinary NC program: it is in the program list, and it 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.

The list and the editor

The app opens on the list of cycle programs. Each row shows the program’s name, the program it compiled to, and how many positions it holds. Tap a row to open it in the editor; NEW PROGRAM starts a new one and asks for its NAME first. The bin at the end of a row deletes the program after asking Delete <name>?.

The editor has the program’s steps on the left, the picture in the middle and the selected step’s fields on the right. The keys above add steps; DELETE STEP removes the selected one. The back arrow returns to the list without losing anything: the list then shows EDITING <name> - unsaved changes with a CONTINUE › row that takes you back.

How a program is built up

Three kinds of step, 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.
• A rotate step turns the part, on a machine that can.

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

PROGRAM        work offset, retraction plane, return mode
  DRILL        12 deep, T3
    POINTS     4 holes you typed
    LINE       6 holes in a row
  TAP          T5
    GRID       3 × 4 holes
  ROTATE       A90
  DRILL        12 deep, T3
    POINTS     2 holes on the second face

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, and type the name when asked.
2. Select PROGRAM and set the three header values below.
3. + DRILL, + TAP or + COUNTERSINK, then fill in the fields on the right.
4. + POINTS, + LINE, + GRID or + CIRCLE, then give it its positions.
5. Repeat 3 and 4 for the next tool. If the part has to turn, + ROTATE first, then a new cycle for the holes on that face.
6. SAVE PROGRAM. The strip at the top says compiled to and the name the machine gave it.
7. LOAD sends that program to the machine, ready to start.

The header

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

Setting	What it does
Work offset	G54 to G59, the datum the coordinates are measured from. Tap it to step to the next
RP Retraction plane	the height the tool goes to after a tool change, before the part turns, and at the end, in mm
Return mode	where the tool returns between holes: G98 to the initial point, G99 to the R point. Use G98 if there is a clamp in the way

Everything is in millimetres.

The cycle fields

Field	Asked for	What to enter	Unit
TOOL	all	the tool that cuts these holes	tool number
DEPTH	DRILL, TAP	how deep the hole is, as a positive number	mm
CHAMFER DIA	COUNTERSINK	the diameter left at the surface	mm
R PLANE	all	how far above the surface the tool starts feeding	mm
F	all	feed	mm/min
SPEED	all	spindle speed	rpm
PECK	DRILL	peck depth. Leave it empty to drill in one go	mm
DWELL S	DRILL, TAP	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 hole’s diameter is not asked for. It is the tool’s, from the tool table, and it is shown beside TOOL as Ø8.00. A tool with no radius in the table shows not defined.

A countersink’s depth is not asked for either. It is worked out from CHAMFER DIA and the tool’s tip angle, and shown as DEPTH with from the tool beside it. If that row reads set the tool's tip angle in red, the tool table has no tip angle for this tool: enter it on the TOOL page, see Tool & Work Offsets.

Which cycle runs

You do not pick a cycle from a menu. The step and what you type decide it:

Step	What runs
DRILL, nothing extra	G81, straight drilling
DRILL with DWELL S	G82, drill and pause at the bottom
DRILL with PECK	G83, peck drilling. With both filled in, PECK decides
TAP	G84, tapping
COUNTERSINK	G82, with the depth from the tool

The selected step shows which one you got, as DRILL (G83).

The patterns

Pattern	You enter
POINTS	each hole’s X and Y in the table under the form. ADD POINT adds a row, DEL POINT removes the selected one
LINE	START X, START Y, DIRECTION in degrees, PITCH, COUNT
GRID	START X, START Y, then PITCH and COUNT along X, PITCH and COUNT along Y
CIRCLE	CENTRE X, CENTRE Y, RADIUS, START ANGLE in degrees, 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. To change one, enter the pattern again.

Turning the part

On a machine with a rotary axis, + ROTATE adds a step that turns the part. Its form has one angle per rotary axis, A ANGLE and B ANGLE on a machine with two, and every axis is written into the program even if you only changed one.

The holes after a rotate step are drilled after the turn. The cycle is cancelled and the tool retracted to RP before the part moves, so the holes on the new face need their own cycle step: + ROTATE, then + DRILL, then the pattern.

The picture shows one face at a time, the face of the selected step. A FACE 2/2 badge in its corner says which, with the angle the part stands at on that face. Select a step on the other face and the picture follows. A face with no holes on it says NOTHING ON THIS FACE.

The picture

Holes are drawn at their real diameter, tapped holes are marked, and the line between them is the order the tool will travel. The size in the corner is how much room the holes on this face take, width by height in mm, and how many positions there are. A radius typed as 500 instead of 50 is obvious there straight away.

Saving and loading

SAVE PROGRAM stores the program and compiles it. The strip at the top then says compiled to and the name the machine gave it, and that is the name you will find in the program list. If it could not be compiled the strip says why, and the row in the list reads not compiled.

LOAD is on once the program has been saved in this session and the machine is free. It sends the program to the machine; cycle start is still yours. Edit anything after saving and the strip reads unsaved changes; LOAD goes off until you save again, so the machine never gets a version older than the one on the screen.

Two things to know about names:

• A cycle program is found by its name. Saving one under a name that already exists gives the new one a (1) after its name.
• If the compiled program was edited by hand on the machine, opening it here shows the program as you saved it, marked save_to_rebuild_machine_copy. SAVE PROGRAM writes the machine’s copy again from what you see.

Limits of this screen

• Tapping needs a compensating (floating) tap holder. The cycle feeds in, reverses the spindle and feeds back out.
• Boring and reaming are written by hand as Canned Cycles.

Where to go next

• Tool & Work Offsets: the tool table, where the diameter and the tip angle come from.
• Selecting & Loading a Program: what LOAD does and what happens next.
• External Program Selection: pick the program by scanning a label instead of finding it in the list.