Click
here to read more
about our BEST-SELLING CNC Programming
Courses. They cover just about everything you'll
ever need to know, whether you're advanced or a beginner...
Click
here to read more about them NOW -- |
Verify CNC Program
Correctness - STEP 2
Author: Mike Lynch
Step two is to verify the correctness
of the setup with proven CNC programs that have been successfully
run before (there shouldn't be anything wrong with the program's
movements). This will be true as long as you're sure that you have
the current version of the program, as long as nothing has changed
since the last time the job was run. However, with new programs,
there could be serious mistakes still in the program.
A setup person can make mistakes
that will cause serious problems, even when running a proven program.
Examples include incorrect placement of the workholding device;
improper cutting tool assembly; incorrect loading of cutting tools
into the machine's turret or magazine; incorrect measurement of
cutting tools (length and radius for machining centers program zero
assignment values on turning centers); and incorrectly entering
the offset values.
A secondary objective is to find
serious mistakes that still exist in the program. This objective
only applies to new programs or programs that have been changed
since the last time they were run. There are some things that even
current off-line program verification systems cannot show. Most,
for example, will ignore offset use.
For a machining center, if you
instate the wrong tool length compensation offset in the pro gram,
most off-line systems will not show it. Again, it takes a watchful
eye to catch motion mistakes when verifying a program off-line.
Any serious mistakes that slip by during step one must be caught
during step two.
Step two is done after the setup
has been made and the program has been loaded into the machine.
Clamps and other potential obstructions should be placed in position.
This step involves running the program on the machine, minus a workpiece
in the setup. Often referred to as a dry run, this procedure is
basic. Although it is taught in the most basic CNC classes, I'm
amazed by the number of companies that skip this step.
To safely perform a dry run, you
must take complete control of the motion rate for all motions the
machine makes, including rapid motions. Almost all machine tool
builders provide a way to do so, but the related buttons and switches
vary from builder to builder.
Many machine tool builders use
the dryrun switch to provide this control. For these machines, when
dry run is on, one multiposition switch controls motion rate for
all movements. Many machine tool builders use the feed rate override
switch or the jog feedrate switch for this purpose.
The dry-run function may slow rapid
motions and speed up cutting motions, so never allow a cutting tool
to machine the workpiece under the influence of dry-run. But this
is exactly the kind of motion-rate control needed to perform step
two.
Two other machine functions are
involved in step two:
Feed hold button: This is your
panic button. Feed hold will cause axis motion to stop. You can
press it when you are worried about a machine motion. We recommend
having a finger ready to press feed hold at all times when performing
a dry run.
Distance-to-go display: Almost
all current CNC machines provide this function which gives you the
ability to determine how much further the cutting tool will move
in the current command.
Again, step two is primarily being
done to confirm the correctness of the step. While the machine is
running the program during this step, you're looking first and foremost
for severe problems that will cause a crash.
As each tool is approaching the
workpiece, you can slow motion rate with the multiposition switch
(again, usually feed rate override). When the cutting tool is clear
of the workpiece (during a retract motion to the tool change position),
you can speed things up. If you're worried for any reason, you can
press the feed hold key and check the distance-to-go display.
Let's say, for example, that you're
performing a dry run on a machining center. One of the cutting tools
is approaching the setup in the Z axis, but it seems to be moving
too far. It seems well past the work surface (which may be difficult
to discern because there is no workpiece in position).
But you're worried, so you press
the feed hold button. You look at the distance-to-go display. It
shows that the current motion will cause the tool to move another
8.3762 inches. When you look into the work area, you realize that
there is not enough room for the tool to move this much farther
before it contacts the fixture. You've just found a serious problem
that would have caused a crash.
When you look at the tool length
compensation offset for this tool, you find that its value is zero
(you forgot to enter it). This is an example of the kind of mistake
you must find in this step.
About the Author
See Mike Lynch on MODERN MACHINE SHOP Online at: www.mmsonline.com/experts/lynch.html
|