KNOWLEDGE BASED MACHINING
For Agie Wire EDM Machines
Straight talk about programming Agie wire EDM machines. In todayís world of
catch phrases and acronyms, it is unlikely that any honest discussion of
programming requirements and capabilities will take place. That is exactly what
this document intends to do.
Agie Wire EDMís have used 3 basic control types, the CNC 100, CNC 123, and
the Agievision. We will discuss the CNC 123D and newer controls including the
AgieVision. The newer generation of Agie controls use multiple types of programs
to machine a workpiece. The CNC 123 uses .GEO (part geometry), .JOB (job
parameters), and .TEB, .TEC or .TED (machine technology). The Agievison uses .ISO
(part geometry), .SBL (script/workpiece parameters and instructions), and .SBR
(file list). These controls use these three distinct types of programs
to allow for complete control of the machining process by offline programming
systems. To effectively program these machines a CAM (computer aided
machining) system should address all three types. Let us look at each type and
itís significance to the machining process.
The technology file contains the machining parameters (generator or
power, strategy, and wire offsets). The technology file on the CNC 123
The geometry file (.GEO) for the CNC 123 is the actual NC code file which
contains the "G", and "M" codes as well as the "X", and "Y" coordinates. Agie
has maintained backward compatibility with previous generations of controls,
because of this fact the geometry file has several unique requirements.
The file must be programmed in incremental.
To achieve the best possibility accuracy the file should be programmed in
No decimal points are allowed. Trailing zeroes must be programmed.
Entry and exit moves from the contour should be perpendicular.
The entry move (lead in) and the first contour move are in reversed order.
A "dummy move" which is tangent to the last contour move must be programmed
before the exit move (lead out).
All intersections must be tangent. A fillet radius must be programmed in
All inside corner radii must be larger than the largest programmed wire
offset or overcutting may occur.
When alternating directions are to be used to trim a part the offset for
the reverse cuts will be negative.
Any CAM system which is going to create programs for an Agie should address
each of these requirements to ensure proper cutting of the workpiece on the
Agie. There may be several solutions for each of these requirements. The
following is a list of acceptable procedures for each:
INCREMENTAL coordinate values can be obtained by several methods. The
previous absolute value can be subtracted from the current absolute value.
This is not the best method due to rounding errors that can occur with numbers
that are not exact at the programmed number of decimal places or due to the
metric conversion. The better method is to subtract the accumulated
incremental values from the current absolute value. This method will eliminate
the potential for rounding errors.
METRIC values can be used when creating the geometry and the tool path.
If the part drawing is not in metric this can lead to manual translation
errors. The data can be input in inch and converted to metric during the post
processing. Please see the note about incremental rounding errors in the
NO DECIMAL POINTS should not be a problem for any system which is
capable of programming trailing zeroes.
PERPENDICULAR ENTRY & EXIT MOVES can be calculated manually by the
programmer. A better method would be if the CAM system provided a method of
creating perpendicular entry and exit points. An additional concern is created
if you wish to enter or exit the contour via a radius. Many system will move
directly from the start point to the entry radius forming a tear drop entry.
This method will not provide a perpendicular entry move from the start point
to the beginning of the entry radius. The same situation occurs at the exit.
You must either manually offset the entry/exit point by the amount of the
entry/exit radius, or the system can automatically insert an additional move
thus creating the necessary perpendicular move. If perpendicular entry/exit
moves are not programmed an incremental offset error may accumulate.
REVERSAL OF ENTRY & FIRST CONTOUR MOVES should be handled automatically
by the programming system. If not then the programmer must remember to
manually edit each set of moves on all cuts.
"DUMMY MOVE" before the exit move must be programmed. The last move of
the program can be duplicated. Since the program is incremental this will
result in the move being tangent only if the contour ended with a
linear segment. If the contour ended on an arc then a tangent linear move must
be calculated by the software. If this move is not tangent an incremental
offset error may accumulate.
ALL INTERSECTIONS MUST BE TANGENT if corner gouging is to be avoided.
The programmer can manually check each intersection and insert a fillet radius
if necessary. The better method would be if the CAM system offered a method of
automatically checking and inserting a specified size fillet radius. If a
different size could be given for inside and outside corners it would be best.
Whatever method is used the software should warn of any nontangent
INSIDE CORNER RADII MUST BE LARGER THAN THE OFFSET to avoid overcutting.
If inside corner radii smaller than the largest offset are necessary the
programmer can develop different geometry with larger radii for the cuts with
larger offsets. This is only possible with offline technology. The system
should alert the programmer to the problem. If possible the system should
automatically modify the inside corner radii so that they are 5 microns larger
than the programmed offset.
NEGATIVE OFFSETS ON REVERSE CUTS can only be achieved by setting the
offsets in the Job or Technology file. The better method would be to use the
Job file because if the Technology file is altered it will remain that way
until changed back. This can cause a problem on another part using the same
file but not requiring negative offsets. If the system automatically creates
the Job file then the negative offset should be set appropriately. The system
could also call each cut individually from the Job file thus eliminating the
need for the negative offsets. Very few systems offer this technique. If the
Job file is not automatically created it will be up to the operator to verify
which offsets need to be negative and properly set them.
If an offline system is only going to create the geometry file (most common)
all of these requirements should be addressed. If not, then the
programmer/operator will be responsible for ensuring that they are.
The CNC 123 uses the .JOB file to set many of the features that on other
machines are set by manual data input. If the programming system does not create
a Job file then the operator can create one manually at the control using the
editor. The Job file is used to set the following parameters:
The Technology file(s) to be used.
The wire break parameters.
The taper values if necessary
Z heights (H1/bottom, H2/land, H3/top)
Special offsets (negative).
Die face up or down (land top or bottom) for tapering.
Offset direction for contouring.
Positioning moves if not programmed in the .GEO file. Fast positioning can
only be programmed in the Job file. Z axis positioning can only be programmed
in the Job file.
Which geometry file(s) and cuts are to be used.
If a system does not create a Job file then in most cases a single geometry
file is created which eliminates the possibility of multiple technology files,
multiple Z heights, fast positioning, and Z axis positioning. Although these
features are not necessary in many cases they do allow more flexibility in
achieving the maximum potential from your machine tool. If you choose a CAM
system without Job file capability you will greatly increase the chance for
The ISO file is the AgieVisionís equivalent to the .GEO file with several
major differences. It can be programmed in absolute. It can use decimal places.
No reversal of entry and first contour moves, actually no entry or exit moves at
all. No dummy blocks. Tangency is not necessary.
In the AgieVison each contour will have itís own ISO file. In addition these
files can be programmed with greatly increased decimal accuracy eliminating many
of the rounding errors.
The script file is the most significant file type associated with the
AgieVision. It has all of the capabilities of Job file and many more. A few of
the functions are listed below.
Establishes the quality target to be obtained or sets a specific technology
The taper values and which cuts they are to be used on.
Z heights and die face up or down.
Clearance if necessary.
Trim direction (forward or reverse).
Separation cut amount (glue stop or tab).
Entry and exit moves. These may be specified tangent or perpendicular.
Entry and exit points.
Conical or cylindrical corners.
Order of cuts.
If the script file is not generated by the offline system these functions can
be set at the machine using the part editor. This will require that the
programmer to create a separate program to create each ISO file on the CAM
system. These files can then be read individually from a floppy disk and they
can be manually integrated into the part using the part editor.
There are many other features of the script file not mentioned here. Only the
most common have been listed to lessen confusion.
The SBR file is simply a list of all of the .ISO files that are used in
this program. The control reads this file when the Script file is imported and
then automatically copies all of the necessary .ISO files.
There are a number of situations which have the potential to create problems
in an Agie programs. The following are sum of the most common examples.
A DXF file is imported from Autocad and all of the corners have a common
.01 in. radius according to a note on the drawing. In reality two of the
corners have been left sharp. If these are inside corners the machine will
gouge these corners. Solutions; 1. Manually check each corner after the Cad
import and insert fillet radii where necessary. 2. Use an automatic filleting
function to insert a fillet radius at any nontangent corner.
The system should warn of any nontangent intersections,
whichever method is used.
The part requires that all inside corners be no larger than a .006 in.
radius. To keep machining time to a minimum, .010 diameter wire will be used.
Overcutting will occur on the main (rough) cut and the first trim cut. The
corners will not clean up with the final trims. Solution; 1. Develop different
contour geometry for each cut with an offset larger than .006. The overcutting
problem will only occur on the Agie 123 controls, not the AgieVision
control. The system should warn you that the overcutting
A punch is being cut using multiple trims. Reverse trimming will result in
the shortest cycle time. If a reverse trim is programmed the associated offset
must be set negative or the wire will cut on the wrong side of the line.
Solutions; 1. The operator will manually edit the Job file to set the offsets
2 & 4 to negative values. 2. The system will automatically create a Job file
and set the appropriate offsets negative. If the
system does not create a Job file then the operator must remember to properly
edit the Job file at the machine.
A punch is being cut using an even number of cuts. When the tab is being
cut the rough cut parameters are normally used. In this case the most
convenient way to cut the tab would be from the start point in a reverse
direction. This will cause a problem because offset number 1 is a positive
offset. Solutions; 1. The programmer will use a previously unused offset (No.
5), and the operator will have to manually edit the Job file to add this
offset. 2. The system will automatically create a Job file which will
automatically reverse the offset direction for the reverse cut..
If the system does not create a Job file then the
programmer must remember to use a different offset for the tab cut and the
operator must remember to properly edit the Job file at the machine
A plate is being cut in the opposite orientation (die face down) from
normal (die face up). The generic Job file that is edited at the machine has
the command for die face up. Solutions; 1. The operator will edit the die face
up command at the machine. 2. The system will automatically create a Job file
for this job with the die face up command. If the
system does not create a Job file then the operator must remember to properly
edit the Job file at the machine.
These are only a few or the most common problems and mistakes that can cause
a part to be scrapped. If the CAM system provides a complete programming
solution (.JOB & .GEO files) all of these potential problems can be eliminated.
As you can see there is clearly more to properly programming an Agie than
meets the eye. Most of the items discussed here are ignored in promotional
literature and sales discussions. Because quite frankly most systems donít deal
with many of these requirements or may not even be aware that they exist. It was
my intention to educate you, the potential buyer of a CAM system to the special
needs for programming an Agie wire EDM machine. I believe you would be wise in
using this document to evaluate the systems you will be considering. Discuss
these potential problems with your sales representative. If he or she is unaware
of these problems or does not wish to discuss their method of coping with them
then perhaps you should look elsewhere.
About the Author
Randy Mell is the President of CAM-1 and has been involved in NC/CNC
programming since 1976. His experience includes working as the Sr. CNC
Applications Engineer for KGK International for 5 years and Sales Manager for
Camtek USA for 3 years. He has extensive experience in the programming of wire
EDM machines and has been instrumental in the development of several CAD/CAM
software packages specializing in wire EDM.
You may contact Randy directly at the following e-mail link
rmell@CAM-1.com with any further questions
you may have.