slotting programme

[davedoubleu]

Just taken delivery of new haas tm 3, been on the course and dont have any problem drilling etc . We could do with an example programme for a slot between two centres say at start position x10 and end position x100 and 12mm deep using 1mm cuts . I think we need to call a sub programme up but we have no idea how to do this , once we get the right format we can use this for numerous applications . Any help greatly appreciated.

[Geof]

The M97 Pn calls a subroutine which is tacked on after the M30 in the program and starts with line number n:

O00000
Stuff
M97 P1000
Stuff
M30
N1000 Subroutine
Stuff
M99

The M99 returns the machine back to the line below the M97 line...Except if you have this:

O00000
Stuff
M97 P1000 Ln
Stuff
M30
N1000 Subroutine
Stuff
M99

Now it returns to the M97 line until the L is counted down to zero so you call the subroutines n times.

You can also have a motion command on the M97 line like this:

G91 G01 X90. Z-1.0 Fwhatever M97 P1000

For slotting I place the tool just above the surface at one end and offset negative by half the difference between the tool width and the slot width.

Then I use a line like the one above, the tool increments the length of the slot going down the Z distance and then enters the subroutine.

In the subroutine the tool increments positive the difference between tool and slot width, then increments negative the X distance and then negative the slot/tool width difference so it is back where it started for the M99.

This sequence repeats n times at which point the tool has reached the final slot depth but part of the slot still has the final Z increment. On the last return the machine goes to the line below the M97 with the L count and this is also a M97 command so the subroutine is run through one more time without any Z motion; This takes out the ramp from the final Z increment. It is also possible to have an L2 so that there is a springpass to remove tool deflection.

After the second M97 there is a G90 G00 Z1.0 to go back to absolute and lift the Z clear.

Using Tool Compensation requires a few extra commands and sometimes it is necessary to start at the center of the slot to avoid overshooting the end on the final motion command before the Z retract and the G40 move. If you write a few sample programs and look at them in graphics you will se what I mean.

[JWK42]

Did you get Macros and Scaling & Rotation? I have a few Macro slot programs that I can share.
Good lucK with your new machine.

[davedoubleu]

thanks for the very useful information , we seem to have got the hang of it now