Response to Cliff's lathe programming ideas.


Feeling somewhat masochistic this afternoon, I will add to the TNR/tool
setting/axis designation free-for-all.

First, axis designation.
As BB has described so well, most 2 axis lathes define Z+ away from the
chuck and Z- as toward the chuck, and X+ away from centerline of rotation
and X- as toward centerline of rotation.

On my Monarch Metalist, the Z axis ways are vertical to the floor, in
that the "back" way is directly above the "front" way with the tool
turret mounted on the cross slide (X axis) directly over the work piece.
In other words, a 90 degree slant bed lathe.

By parameter, the GE 1050HL control on the monarch can change the Z and X
axi and change the +/- designation any way you would like. Example: Z+
away from chuck, X+ toward centerline. Actually, the variuos
configurations are illustrated by arrows that point up/down and
left/right. 8 parameter settings availible.

Second, CAD/CAM axis on the monitor.
Unless I go thru a lot of gyrations with Edgecam, which is a full CAD and
CAM package, the 2 axis turning module screen is Z+ from left to right,
X+ from bottom to top. You CAN NOT enter a Y axis value.

Third, determining the X an Z tool(tip) location.
The procedure in the Monarch, Anilam and Fanuc operator manuals all
agree. Touch the tool to the end of the stock sticking out of the chuck
and give this some Z value. Then assign a value in the tool data/offset
tables. Monarch recommended setting the tool value to zero for the first
tool and setting the subsequent tools to a plus or minus value in
relation to the first tool.

To set X, touch off or turn a short bit of the stock to create a
concentric diameter. Measure this diameter and go thru the appropriate
hoops to establish the tool data for the first tool. The GE1050HL
requires that you do the math and enter the data. The Anilam and Fanuc
do the math and make the entry after you tell the control what the
measured diameter is.

During this procedure, none of the manuals ask for the radius of the tool
tip.

Fourth. Toolpath and TNR compensation.
But first, a definition: Theoretical or Imaginary tool tip. The point
where X and Z axis cross one another and are tangent to the tool radius
in each axis. Edgecam calls this point "orthogonal."

The GE 1050HL control does calculate a tool path using the center of the
TNR. However, if the TNR is set to zero the calculated path will be the
same as the measured or drawn dimension. The Anilam calculates a path
along the edge of the tool until a radius is encountered, then it
calculates a radial move using arc that is based on the imaginary
tooltip, but only in a canned cycle or with G41/G42 compensation active.
I'm not sure what the Fanuc does because I have never tried to figure it
out.

Following are 3 programs for the same profile using three different
methods in edgecam, one of which simulates the GE 1050 calculations. The
profile begins at (from left to right) Z0 and X4., goes to Z1.5, then
goes to Z2. X3.(45 degrees), then to Z3.0.

The tool uses a DNMG 432 insert. .031 TNR, for those who may not know.

1. Using "orthogonal" tool tip. No tool nose compensation.

N30 T0200
N40 G92 X18.4 Z10
N50 M51
N60 G97 S400 M03
N70 G00 X3.2 Z3.1 T0202 M08
N80 X3.1 Z3.05
N90 G01 X3 Z3 F.01
N100 Z2
N110 X4 Z1.5
N120 Z.5
N130 G00 X18.4 Z10 T0200 M09
N140 M30

2. Using center of TNR with radius value entered in tool table.
These numbers were verified on the Monarch by single blocking the above
program and reading the values in the machine display.

N30 T0200
N40 G92 X18.4 Z10
N50 M51
N60 G97 S400 M03
N70 G00 X3.2 Z3.1 T0202 M08
N80 X3.1423 Z3.0582
N90 G01 X3.062 Z3 F.01
N100 Z2.0128
N110 X4.0438 Z1.5219
N120 G03 X4.062 Z1.5 I.0219 K.0219
N130 G01 Z.5
N140 G00 X18.4 Z10 T0200 M09
N150 M30

3. Using "orthogonal" tip and Edgecam "pathcomp", a utility that
calculates the tool path using the imaginary tool tip as the center of
the arc in the calculations. The same as the Anilam control(Also
verified by single blocking the program).

N30 T0200
N40 G92 X18.4 Z10
N50 M51
N60 G97 S400 M03
N70 G00 X3.2 Z3.1 T0202 M08
N80 X3.0858 Z3.0252
N90 G01 X3 Z2.969 F.01
N100 Z1.9818
N110 X3.9818 Z1.4909
N120 G03 X4 Z1.469 I.0219 K.0219
N130 G01 Z.469
N140 G00 X18.4 Z10 T0200 M09
N150 M30

The second and third programs introduce an arc move as the tool
transitions from the 45 degree move to the Z move after X 4. is reached.
As you can see, there are slightly different positioning and acrc moves
in the two programs. It has been my experience (only 20 years) that the
use of "Pathcomp" is better at making a smooth transition (no burr or
roughness) than the centerline programming.

I just don't mess with G41/ G42 or centerline programming at all. Just
let "Pathcomp" handle it. Except when using canned cycles on the Anilam
control; then I have to cancel the "pathcomp" and let the control
calculate the toolpath.

So, Cliff was right, to some extent, when he said the control uses
centerline to calculate the tool path..... on the GE 1050HL, but not the
Anilam or Fanuc controls. And from those who seem to know about the
Yasnac on the Mori SL1 that Mr. Clark has been asking about, the Yasnac
doesn't do centerline calculations either.
--
Remove "nospam" to get to me.
.

Relevant Pages

  • Re: AVR Butterfly (was Re: Beginner needs help...)
    ... My first motion control project, and first real microcontroller project was ... a 2 axis system. ... It can't hurt to plunge in as deep as you care to. ... A big scary 16 bit micro may look bigger and scarier than a Pic ...
    (comp.robotics.misc)
  • Re: Obsolete Memory
    ... We're a 2 man job shop, wanting to expand into doing some production work. ... 2 1/2 axis CNC knee type mill doing some simple work. ... Control wise, we don't really know as we haven't been able to get it up an running. ... There is no reason this machine if in good mechanical shape wont run ...
    (alt.machines.cnc)
  • Re: What sort of joystick/controller to use to remotely control/pilot walking robot?
    ... about switching over to something like a 3 axis joystick, ... Also - I can't decide about which control should do what. ... that the harder you twist the joystick the tighter of a circle it ...
    (comp.robotics.misc)
  • Re: Newbie question of the day
    ... >axis designators in ordinary G-code syntax. ... By the time you have that many axes it's not really an "ordinary" ... >probably work depending on the control vendor. ... With a gantry it would probably be a twin spindle 5 axes ...
    (alt.machines.cnc)
  • Re: Polar Coordinate Programing
    ... It was an old fanuc 6T control ... with a C axis and I wrote a Qbasic program that trigged the X position ...
    (alt.machines.cnc)