Re: [CAD_CAM_EDM_DRO] emc g92

John Dammeyer wrote:

>
>So that brings up an interesting question alluded to by some of
>the posters. I can see installing each milling cutter in a
>removable insert pulled automatically off a tool tray. I can
>see setting up the insert so the machine knows where the end of
>the tool is. Then each time the tool is grabbed it uses the
>correct offset and all works well.
>
>But for the home/light_industry CNC world where a program might
>use three different cutters, how is this set up if the G92
>command doesn't work? Is there a different command?
>
>

G92 DOES work, but using it for tool length offset is wrong, as far as
I can see. There is a function specifically designed for tool length
compensation, called G43. it interpolates in the offset on the first Z
move after it is invoked. It gets the length of the tool from the
tool table. I have converted over to end mill holders so i can get
repeatable tool locations every time I insert the tool.

>Say I had three end mills which I wanted to use for three
>different slots. (Yes, I know, use the smallest and make
>multiple passes). What would a program for the EMC application
>look like to cut three slots, 1" apart for two inches, X=3.000,
>Y=3.000 away from the home position. Let's make each of the
>slots 0.100" deep so they can all be cut in one pass. Oh yes,
>to make things a bit more difficult, two of the cutters have the
>same shank diameter and one is a bit smaller.
>
>My Drill/Mill has MT-3 tooling so I'd have to move the table out
>of the way, undo the drawbar, whack the drawbar with a mallet,
>unscrew the MT-3 the rest of the way and insert and tighten up
>the other MT-3 holder. Or would I keep 3 MT-3 holders in stock,
>each with their respective cutter and measure the end of the
>cutter relative to some 0 point for each cutter? Base of the
>Spindle perhaps?
>
>

Yes, that's the way to do it. I keep about 5 of the most commonly used
tools permanently in holders. I have a center drill, a 1/4" end mill, a
3/8" end mill and a 1/2" end mill as the most common tools. I can also
set up a drill bit in a Jacob's chuck (I have 2 small and one large one)
and preset the tool length of that, too. As long as I don't pull the
drill bit out
of the chuck, it will repeat the same length every time.

I made a replica of the R-8 spindle taper so I can put my tool holders in
it, and then read the height on a surface plate with a vernier height gauge.

>People have discussed moving the cutter down until it touches
>paper that is 0.005" thick so there I'm assuming that the cutter
>is changed in the holder and sits at a different height and then
>adjusting for the 0.005".
>
>

No, I leave the cutter tightly locked in the holder. When the paper is
pinched, I
stop jogging down and enter .005 on the Z axis. To do this, I place the
cursor over the Z axis coordinate display and right-click the mouse.
A dialog box appears. If the setting is totally non-critical, like for
drilling through a part, I just hit enter, and the Z axis is set to zero.
If it is critical, I type .005 and hit enter. Z is set to 0.005, which
is the
height of the cutting edge above the top of the part. I then jog up to get
more clearance.

>So what would the program look like? Seems it would be a simple
>G-Code application so could someone experienced post how they'd
>do this? How would it be done in Turbo-CNC. How about some
>commercial machine?
>
>

You might want to look at my programs that write the G-code for slotting
applications. (A slot is a kind of rectangular pocket.) I have 2 programs,
one that completely obliterates the interior of the pocket, called
rectpocket.
Another one just cuts the outer edge, allowing the blank to drop out. This
is called treprect, for trepan rectangle, and is for making a cutout in
a panel.
Both programs will rough the hole or pocket in depth steps, and then finish
to the final ID. See http://jelinux.pico-systems.com/gcode.html where you
can download c source or DOS executables of these and other programs.
(They are tested on EMC, but should work on most CNC programs, as they
use the lowest common denominator of G-codes.)

Jon