I had a little light bulb go off in my head.

I think that I know what to do.

I will have functions that could combine different machining notions
together.

For example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Okay so far.

This really involves two separate concepts:

1) Generating the shape of the cut (circular, in this example)
and
2) Implementing a cut along an arbitrary shape, with several passes if
necessary

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.

Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.

This kind of approach, has potential for some very fun results.

i

On Jul 22, 2:35*pm, Ignoramus24043 ignoramus24...@NOSPAM.
24043.invalid wrote:
I had a little light bulb go off in my head.

I think that I know what to do.

I will have functions that could combine different machining notions
together.

For example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Okay so far.

This really involves two separate concepts:

1) Generating the shape of the cut (circular, in this example)
and
2) Implementing a cut along an arbitrary shape, with several passes if
necessary

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.

Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.

This kind of approach, has potential for some very fun results.

i

If I'm getting this right, you're putting X and Y moves in an inner
loop with minor Z movements outside them and major Z movements outside
of that, Correct? No reason at all why something like that shouldn't
work.

Ignoramus24043 wrote:

I had a little light bulb go off in my head.

I think that I know what to do.

I will have functions that could combine different machining notions
together.

For example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Okay so far.

This really involves two separate concepts:

1) Generating the shape of the cut (circular, in this example)
and
2) Implementing a cut along an arbitrary shape, with several passes if
necessary

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.

Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.

This kind of approach, has potential for some very fun results.

i

You're picking up on what CAM software does. CAD provides the design of
the part, CAM figures out how to make the part essentially.

Ignoramus24043 wrote:

2) Implementing a cut along an arbitrary shape, with several passes if
necessary

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.

The generally suggested method is to ramp down while performing the cut,
rather than plunging in Z and then moving in XY. I have already
converted my "treprect" program that plunged first, then cut around the
rectangular shape, then made a finish pass at full depth. The new
version, which I haven't gotten up on my web page yet ramps down on the
first side of each level.
Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.
If it is not a simple circle, oval or rectangle, then it may be better
to plan the whole thing on a CAD system. Bobcad/CAM, one of the
lower-level packages, will do this pretty much automatically. You give
the pocket outline, the depth, and set some parameters such as the
step-over and plunge increment, and have it draw an offset line to
compensate for the tool radius, and it will carve out the interior of
the pattern automatically. Pretty much any CAM system ought to be able
to do the same.

Jon

On 2010-07-22, Jon Elson wrote:
Ignoramus24043 wrote:

2) Implementing a cut along an arbitrary shape, with several passes if
necessary

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.

The generally suggested method is to ramp down while performing the cut,
rather than plunging in Z and then moving in XY. I have already
converted my "treprect" program that plunged first, then cut around the
rectangular shape, then made a finish pass at full depth. The new
version, which I haven't gotten up on my web page yet ramps down on the
first side of each level.

That actually makes perfect sense. Thanks for bringing this up.

Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.

If it is not a simple circle, oval or rectangle, then it may be better
to plan the whole thing on a CAD system. Bobcad/CAM, one of the
lower-level packages, will do this pretty much automatically. You give
the pocket outline, the depth, and set some parameters such as the
step-over and plunge increment, and have it draw an offset line to
compensate for the tool radius, and it will carve out the interior of
the pattern automatically. Pretty much any CAM system ought to be able
to do the same.

Sure. I will look into all of it.

i

"Jon Elson" wrote in message
...
Ignoramus24043 wrote:

2) Implementing a cut along an arbitrary shape, with several passes if
necessary

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.
The generally suggested method is to ramp down while performing the cut,
rather than plunging in Z and then moving in XY. I have already converted
my "treprect" program that plunged first, then cut around the rectangular
shape, then made a finish pass at full depth. The new version, which I
haven't gotten up on my web page yet ramps down on the first side of each
level.
Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.
If it is not a simple circle, oval or rectangle, then it may be better to
plan the whole thing on a CAD system. Bobcad/CAM, one of the lower-level
packages, will do this pretty much automatically. You give the pocket
outline, the depth, and set some parameters such as the step-over and
plunge increment, and have it draw an offset line to compensate for the
tool radius, and it will carve out the interior of the pattern
automatically. Pretty much any CAM system ought to be able to do the
same.

Dudn't dat Mach controller program do all this?
These are all standard routines in any Haas/fadal, etc.

If doing a curve with an underlying analytic function, that function can be
straightforwardly done in a macro, without the need for cad or cam.
Fadal supplies such a macro for an ellipse. I think it has to be done
quadrant by quadrant, but no biggie.
I've done such a macro for fishmouth chamfering.
--
EA

Jon

Existential Angst wrote:

"Jon Elson" wrote in message
...
Ignoramus24043 wrote:

2) Implementing a cut along an arbitrary shape, with several passes if
necessary

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.
The generally suggested method is to ramp down while performing the cut,
rather than plunging in Z and then moving in XY. I have already converted
my "treprect" program that plunged first, then cut around the rectangular
shape, then made a finish pass at full depth. The new version, which I
haven't gotten up on my web page yet ramps down on the first side of each
level.
Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.
If it is not a simple circle, oval or rectangle, then it may be better to
plan the whole thing on a CAD system. Bobcad/CAM, one of the lower-level
packages, will do this pretty much automatically. You give the pocket
outline, the depth, and set some parameters such as the step-over and
plunge increment, and have it draw an offset line to compensate for the
tool radius, and it will carve out the interior of the pattern
automatically. Pretty much any CAM system ought to be able to do the
same.

Dudn't dat Mach controller program do all this?
These are all standard routines in any Haas/fadal, etc.

Iggy is using EMC2, but yes, Mach3 has "wizards" for these type of
functions and I'm pretty sure EMC2 has something comparable as well.

Ignoramus24043 wrote:

or example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Okay so far.

See G12,G13 with plane select keyword(G17,18,19). My quick google shows that g2 g3 now
take a ramping value on some controls.

In the case of G12, G13 on older controls, it was basically a G2/3 move with an infeed or
ramping down/up per revolution. That is if I remember this correctly.


Wes

http://www.new.manufacturinget.com/?p=620

--
"Additionally as a security officer, I carry a gun to protect
government officials but my life isn't worth protecting at home
in their eyes." Dick Anthony Heller

On 2010-07-22, Ignoramus24043 wrote:
I had a little light bulb go off in my head.

I think that I know what to do.

I will have functions that could combine different machining notions
together.

For example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Even better is to ramp down as you circle. Plunging requires a
center-cutting mill. The ramp does not as you get slightly deeper as
you progress.

Okay so far.

This really involves two separate concepts:

1) Generating the shape of the cut (circular, in this example)
and
2) Implementing a cut along an arbitrary shape, with several passes if
necessary

Also consider cutter compensation -- telling the CNC machine
what diameter cutter you are using, and which side of the cutter you are
using, and it generates a tool path to produce the shape you want -- or
complains if the drawing calls for a tighter radius in the pocket than
your mill can actually produce. Of course, you don't hit this
particular problem when cutting the outside of a rectangle.

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.

But if you don't separate (in time) the tasks, you can do the
ramp down instead.

Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.

This kind of approach, has potential for some very fun results.

Indeed so.

Enjoy,
DoN.

--
Remove oil spill source from e-mail
Email: | Voice (all times): (703) 938-4564
(too) near Washington D.C. | http://www.d-and-d.com/dnichols/DoN.html
--- Black Holes are where God is dividing by zero ---

Ignoramus24043 on Thu, 22 Jul
2010 14:03:10 -0500 typed in rec.crafts.metalworking the following:
On 2010-07-22, Pete C. wrote:

Ignoramus24043 wrote:

I had a little light bulb go off in my head.

I think that I know what to do.

I will have functions that could combine different machining notions
together.

For example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Okay so far.

This really involves two separate concepts:

1) Generating the shape of the cut (circular, in this example)
and
2) Implementing a cut along an arbitrary shape, with several passes if
necessary

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.

Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.

This kind of approach, has potential for some very fun results.

i

You're picking up on what CAM software does. CAD provides the design of
the part, CAM figures out how to make the part essentially.

I think that what I am trying to do, is build a library of functions
to provide CAM functionality.

And is a good thing to understand in and of itself. That is,
when I was taking a class on CNC, we started out having to write the
code to move the end mill from point A to point B. All the code, all
the way. From "turn on spindle" to descend, to enter metal, to move
to starting point, make pass, exit, etc, etc, etc. Once we knew what
we wanted, and how it was done, then we moved on to the "neat" CAD/CAM
which let us draw the part, then let the program figure out how to
mill it. Even then, it required us to understand the process.

pyotr
--
pyotr filipivich
We will drink no whiskey before its nine.
It's eight fifty eight. Close enough!

On 2010-07-23, pyotr filipivich wrote:
Ignoramus24043 on Thu, 22 Jul
2010 14:03:10 -0500 typed in rec.crafts.metalworking the following:
On 2010-07-22, Pete C. wrote:

Ignoramus24043 wrote:

I had a little light bulb go off in my head.

I think that I know what to do.

I will have functions that could combine different machining notions
together.

For example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Okay so far.

This really involves two separate concepts:

1) Generating the shape of the cut (circular, in this example)
and
2) Implementing a cut along an arbitrary shape, with several passes if
necessary

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.

Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.

This kind of approach, has potential for some very fun results.

i

You're picking up on what CAM software does. CAD provides the design of
the part, CAM figures out how to make the part essentially.

I think that what I am trying to do, is build a library of functions
to provide CAM functionality.

And is a good thing to understand in and of itself. That is,
when I was taking a class on CNC, we started out having to write the
code to move the end mill from point A to point B. All the code, all
the way. From "turn on spindle" to descend, to enter metal, to move
to starting point, make pass, exit, etc, etc, etc. Once we knew what
we wanted, and how it was done, then we moved on to the "neat" CAD/CAM
which let us draw the part, then let the program figure out how to
mill it. Even then, it required us to understand the process.

Great approach. Cover the basics first. Since I have a mill, I have to
write all codes etc. (and if I cut its table in half accidentally, it
will be my loss to eat!)

i

On Jul 22, 6:21*pm, Ignoramus24043 ignoramus24...@NOSPAM.
24043.invalid wrote:
On 2010-07-23, pyotr filipivich wrote:



Ignoramus24043 on Thu, 22 Jul
2010 14:03:10 -0500 typed in rec.crafts.metalworking *the following:
On 2010-07-22, Pete C. wrote:

Ignoramus24043 wrote:

I had a little light bulb go off in my head.

I think that I know what to do.

I will have functions that could combine different machining notions
together.

For example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Okay so far.

This really involves two separate concepts:

1) Generating the shape of the cut (circular, in this example)
and
2) Implementing a cut along an arbitrary shape, with several passes if
necessary

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.

Same applies to "milling out a deep pocket along an arbitrary shape"..
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.

This kind of approach, has potential for some very fun results.

i

You're picking up on what CAM software does. CAD provides the design of
the part, CAM figures out how to make the part essentially.

I think that what I am trying to do, is build a library of functions
to provide CAM functionality.

* *And is a good thing to understand in and of itself. * That is,
when I was taking a class on CNC, we started out having to write the
code to move the end mill from point A to point B. *All the code, all
the way. *From "turn on spindle" to descend, to enter metal, to move
to starting point, make pass, exit, etc, etc, etc. *Once we knew what
we wanted, and how it was done, then we moved on to the "neat" CAD/CAM
which let us draw the part, then let the program figure out how to
mill it. *Even then, it required us to understand the process.

Great approach. Cover the basics first. Since I have a mill, I have to
write all codes etc. (and if I cut its table in half accidentally, it
will be my loss to eat!)

i

If, when using one of your programs, you suddenly hit an emergency
stop button, does your program stop, also? Then are you able to go
back to the operation that stopped and continue on? Something to
consider.

Paul

On 2010-07-23, wrote:
On Jul 22, 6:21*pm, Ignoramus24043 ignoramus24...@NOSPAM.
24043.invalid wrote:

[ ... ]

Great approach. Cover the basics first. Since I have a mill, I have to
write all codes etc. (and if I cut its table in half accidentally, it
will be my loss to eat!)

i

If, when using one of your programs, you suddenly hit an emergency
stop button, does your program stop, also? Then are you able to go
back to the operation that stopped and continue on? Something to
consider.

I consider it to be very likely using EMC.

However -- using my Compact-5/CNC lathe (Emco-Maier 5" swing,
stepper driven, 6502 CPU) not only can I not restart from the step which
I stopped on -- but I lose the entire program (unless I saved it on tape
first), because it drops power from the CPU and spindle motor as well as
the stepper motors.

And if you have the encoder counters powered by an alternative
power source (e.g. the Servo-To-Go board has provisions for a battery to
back up the counters and continue power to the encoders) you can even
have the machine record how far it was moved by manually manipulating
the powered-down servo motors or the leadscrews (if they rotate -- the
Bridgeport BOSS-3 X-axis does not -- the nut rotates in precision
bearings instead, so you avoid whip in the leadscrew at high speeds --
as though you could accomplish high speeds with the original stepper
motors in the BOSS-3.)

Enjoy,
DoN.

--
Remove oil spill source from e-mail
Email: | Voice (all times): (703) 938-4564
(too) near Washington D.C. | http://www.d-and-d.com/dnichols/DoN.html
--- Black Holes are where God is dividing by zero ---

On 23 Jul 2010 05:03:26 GMT, "DoN. Nichols"
wrote:

On 2010-07-23, wrote:
On Jul 22, 6:21*pm, Ignoramus24043 ignoramus24...@NOSPAM.
24043.invalid wrote:

[ ... ]

Great approach. Cover the basics first. Since I have a mill, I have to
write all codes etc. (and if I cut its table in half accidentally, it
will be my loss to eat!)

i

If, when using one of your programs, you suddenly hit an emergency
stop button, does your program stop, also? Then are you able to go
back to the operation that stopped and continue on? Something to
consider.

I consider it to be very likely using EMC.

However -- using my Compact-5/CNC lathe (Emco-Maier 5" swing,
stepper driven, 6502 CPU) not only can I not restart from the step which
I stopped on -- but I lose the entire program (unless I saved it on tape
first), because it drops power from the CPU and spindle motor as well as
the stepper motors.

You really need to have the program written to tape (uggg!!) a floppy,
or even a flash device and simply reload from the files.


There is no way to go to Toolx and start from there?



And if you have the encoder counters powered by an alternative
power source (e.g. the Servo-To-Go board has provisions for a battery to
back up the counters and continue power to the encoders) you can even
have the machine record how far it was moved by manually manipulating
the powered-down servo motors or the leadscrews (if they rotate -- the
Bridgeport BOSS-3 X-axis does not -- the nut rotates in precision
bearings instead, so you avoid whip in the leadscrew at high speeds --
as though you could accomplish high speeds with the original stepper
motors in the BOSS-3.)

Enjoy,
DoN.

One could not be a successful Leftwinger without realizing that,
in contrast to the popular conception supported by newspapers
and mothers of Leftwingers, a goodly number of Leftwingers are
not only narrow-minded and dull, but also just stupid.
Gunner Asch

On 2010-07-22, Wes wrote:
Ignoramus24043 wrote:

or example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Okay so far.

See G12,G13 with plane select keyword(G17,18,19). My quick google shows that g2 g3 now
take a ramping value on some controls.

Yes, but for circles only. EMC takes arguments to make the cut helical.

I want to make a lifting eye with a egg shaped hole.

In the case of G12, G13 on older controls, it was basically a G2/3 move with an infeed or
ramping down/up per revolution. That is if I remember this correctly.

You do.

i


Wes

http://www.new.manufacturinget.com/?p=620


EMC is almost all software, so,

On 2010-07-22, DoN. Nichols wrote:
On 2010-07-22, Ignoramus24043 wrote:
I had a little light bulb go off in my head.

I think that I know what to do.

I will have functions that could combine different machining notions
together.

For example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Even better is to ramp down as you circle. Plunging requires a
center-cutting mill. The ramp does not as you get slightly deeper as
you progress.

Great point.

Okay so far.

This really involves two separate concepts:

1) Generating the shape of the cut (circular, in this example)
and
2) Implementing a cut along an arbitrary shape, with several passes if
necessary

Also consider cutter compensation -- telling the CNC machine
what diameter cutter you are using, and which side of the cutter you are
using, and it generates a tool path to produce the shape you want -- or
complains if the drawing calls for a tighter radius in the pocket than
your mill can actually produce. Of course, you don't hit this
particular problem when cutting the outside of a rectangle.

you mean inside rectangle?

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.

But if you don't separate (in time) the tasks, you can do the
ramp down instead.

Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.

This kind of approach, has potential for some very fun results.

Indeed so.

I will first try to just learn G codes, I think, but I started
experimenting with better way of writing those scripts. Basically a
CAM library in perl.

But I think that before running, I need to learn to walk, so, I will
practice using G-Codes in a non-idiosyncratic manner.

i


i

On 2010-07-23, wrote:
On Jul 22, 6:21?pm, Ignoramus24043 ignoramus24...@NOSPAM.
24043.invalid wrote:
On 2010-07-23, pyotr filipivich wrote:



Ignoramus24043 on Thu, 22 Jul
2010 14:03:10 -0500 typed in rec.crafts.metalworking ?the following:
On 2010-07-22, Pete C. wrote:

Ignoramus24043 wrote:

I had a little light bulb go off in my head.

I think that I know what to do.

I will have functions that could combine different machining notions
together.

For example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Okay so far.

This really involves two separate concepts:

1) Generating the shape of the cut (circular, in this example)
and
2) Implementing a cut along an arbitrary shape, with several passes if
necessary

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.

Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.

This kind of approach, has potential for some very fun results.

i

You're picking up on what CAM software does. CAD provides the design of
the part, CAM figures out how to make the part essentially.

I think that what I am trying to do, is build a library of functions
to provide CAM functionality.

? ?And is a good thing to understand in and of itself. ? That is,
when I was taking a class on CNC, we started out having to write the
code to move the end mill from point A to point B. ?All the code, all
the way. ?From "turn on spindle" to descend, to enter metal, to move
to starting point, make pass, exit, etc, etc, etc. ?Once we knew what
we wanted, and how it was done, then we moved on to the "neat" CAD/CAM
which let us draw the part, then let the program figure out how to
mill it. ?Even then, it required us to understand the process.

Great approach. Cover the basics first. Since I have a mill, I have to
write all codes etc. (and if I cut its table in half accidentally, it
will be my loss to eat!)

i

If, when using one of your programs, you suddenly hit an emergency
stop button, does your program stop, also? Then are you able to go
back to the operation that stopped and continue on? Something to
consider.

I am not sure, I will check it out.

"Ignoramus24043" wrote in message
...
I had a little light bulb go off in my head.

I think that I know what to do.

I will have functions that could combine different machining notions
together.

For example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Okay so far.

This really involves two separate concepts:

1) Generating the shape of the cut (circular, in this example)
and
2) Implementing a cut along an arbitrary shape, with several passes if
necessary

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.

Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.

This kind of approach, has potential for some very fun results.


Have you looked at Mach 3? It has wizards included that do many of these
functions already. It has a number of lines of code limit, and I think you
need to register to use the wizards, but its worth a look see.

Have you looked at Cam Bam? They claim it's a beta, but I have done some
real serious detail work with this CAM software, and it even has some
limited CAD capability. The executions limited demo is 100% non crippled,
and the price to register is very reasonable.

If you enjoy writing programs soldier on, but otherwise I think you are
reinventing the wheel.

Yes, I still do some hand coding of G-code, but as I learn to use the tools
I have I do less and less of it.

"rangerssuck" wrote in message
...
On Jul 22, 2:35 pm, Ignoramus24043 ignoramus24...@NOSPAM.
24043.invalid wrote:
I had a little light bulb go off in my head.

I think that I know what to do.

I will have functions that could combine different machining notions
together.

For example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Okay so far.

This really involves two separate concepts:

1) Generating the shape of the cut (circular, in this example)
and
2) Implementing a cut along an arbitrary shape, with several passes if
necessary

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.

Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.

This kind of approach, has potential for some very fun results.

i

If I'm getting this right, you're putting X and Y moves in an inner
loop with minor Z movements outside them and major Z movements outside
of that, Correct? No reason at all why something like that shouldn't
work.

Yeah, NFS Wizards in Mach 3 have functions to do that built in. You just
tell it to ramp to depth. It drills a helical pattern to depth and then
finishes the pocket. If the pocket is multi pass it will do it for each
pass.

Ignoramus7608 wrote:

See G12,G13 with plane select keyword(G17,18,19). My quick google shows that g2 g3 now
take a ramping value on some controls.

Yes, but for circles only. EMC takes arguments to make the cut helical.

I want to make a lifting eye with a egg shaped hole.

Might as well have fun. Pictures are expected

Wes
--
"Additionally as a security officer, I carry a gun to protect
government officials but my life isn't worth protecting at home
in their eyes." Dick Anthony Heller

On Fri, 23 Jul 2010 11:58:20 -0700, "Bob La Londe"
wrote:

"Ignoramus24043" wrote in message
m...
I had a little light bulb go off in my head.

I think that I know what to do.

I will have functions that could combine different machining notions
together.

For example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Okay so far.

This really involves two separate concepts:

1) Generating the shape of the cut (circular, in this example)
and
2) Implementing a cut along an arbitrary shape, with several passes if
necessary

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.

Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.

This kind of approach, has potential for some very fun results.


Have you looked at Mach 3? It has wizards included that do many of these
functions already. It has a number of lines of code limit, and I think you
need to register to use the wizards, but its worth a look see.

Have you looked at Cam Bam? They claim it's a beta, but I have done some
real serious detail work with this CAM software, and it even has some
limited CAD capability. The executions limited demo is 100% non crippled,
and the price to register is very reasonable.

If you enjoy writing programs soldier on, but otherwise I think you are
reinventing the wheel.

Yes, I still do some hand coding of G-code, but as I learn to use the tools
I have I do less and less of it.


I do have a spare registered dongle for one of the older versions of
MasterCam btw...I was wanting $1000 for it..but ..I might Swap for it.

Gunner

One could not be a successful Leftwinger without realizing that,
in contrast to the popular conception supported by newspapers
and mothers of Leftwingers, a goodly number of Leftwingers are
not only narrow-minded and dull, but also just stupid.
Gunner Asch

On 2010-07-23, Gunner Asch wrote:
On 23 Jul 2010 05:03:26 GMT, "DoN. Nichols"
wrote:

On 2010-07-23, wrote:

[ ... ]

If, when using one of your programs, you suddenly hit an emergency
stop button, does your program stop, also? Then are you able to go
back to the operation that stopped and continue on? Something to
consider.

I consider it to be very likely using EMC.

However -- using my Compact-5/CNC lathe (Emco-Maier 5" swing,
stepper driven, 6502 CPU) not only can I not restart from the step which
I stopped on -- but I lose the entire program (unless I saved it on tape
first), because it drops power from the CPU and spindle motor as well as
the stepper motors.

You really need to have the program written to tape (uggg!!) a floppy,
or even a flash device and simply reload from the files.

The provisions on this machine are saving to tape (a weird
miniaturized cassette which is not quite compatible with the tiny
answering machine tapes) or to punched tape via a RS-232 interface
(which is what I use to save to a computer instead -- though it is
awkward in any case.

I do have a (totally undocumented) 3-1/2" floppy drive with a
controller card on it from the Emco-Maier people which can replace the
tape drive (and which probably acts *just* like the tape drive from the
front panel controls) which I have not yet bothered to make up the
mounting hardware for. But I'm not at all sure that it is any better
than the tapes, other than floppies are easier to find. :-)


There is no way to go to Toolx and start from there?

Note that this has no home positions. You move to somewhere
and then select absolute mode, and it works from there. If the program
stops and power is lost (e.g. the e-Stop) it also loses track of where
it was.

You can't define the tool offsets at the beginning of the
program -- *each* time you call up a tool, you have to enter the offsets
with it. And the tool turret does not have a home position either. You
tell it to move forward N stations (so you have to keep track of where
it is -- and have to end the program with a return to the starting
station or everything will be a disaster when you start again. :-)

Remember -- this is not EMC -- or anything else serious. It
lives entirely in the address space of a 6502 (the CPU used in the
Apple-II or the Commodore PET).

I believe that it was sold to be used as a training tool, not a
working one. :-)

Enjoy,
DoN.

--
Remove oil spill source from e-mail
Email: | Voice (all times): (703) 938-4564
(too) near Washington D.C. | http://www.d-and-d.com/dnichols/DoN.html
--- Black Holes are where God is dividing by zero ---

On 2010-07-23, Ignoramus7608 wrote:
On 2010-07-22, Wes wrote:
Ignoramus24043 wrote:

or example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Okay so far.

See G12,G13 with plane select keyword(G17,18,19). My quick google shows that g2 g3 now
take a ramping value on some controls.

Yes, but for circles only. EMC takes arguments to make the cut helical.

Hmm ... what about arguments to make a circle elliptical?

I want to make a lifting eye with a egg shaped hole.

With *that* -- you will need a much more complex program,
blending various curves to make the total desired shape -- and you might
as well find a section which is the largest segment of a circle and ramp
down during that, then complete the shape from there.

Enjoy,
DoN.

--
Remove oil spill source from e-mail
Email: | Voice (all times): (703) 938-4564
(too) near Washington D.C. | http://www.d-and-d.com/dnichols/DoN.html
--- Black Holes are where God is dividing by zero ---

"Gunner Asch" wrote in message
...
On Fri, 23 Jul 2010 11:58:20 -0700, "Bob La Londe"
wrote:

"Ignoramus24043" wrote in message
om...
I had a little light bulb go off in my head.

I think that I know what to do.

I will have functions that could combine different machining notions
together.

For example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Okay so far.

This really involves two separate concepts:

1) Generating the shape of the cut (circular, in this example)
and
2) Implementing a cut along an arbitrary shape, with several passes if
necessary

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.

Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.

This kind of approach, has potential for some very fun results.


Have you looked at Mach 3? It has wizards included that do many of these
functions already. It has a number of lines of code limit, and I think
you
need to register to use the wizards, but its worth a look see.

Have you looked at Cam Bam? They claim it's a beta, but I have done some
real serious detail work with this CAM software, and it even has some
limited CAD capability. The executions limited demo is 100% non crippled,
and the price to register is very reasonable.

If you enjoy writing programs soldier on, but otherwise I think you are
reinventing the wheel.

Yes, I still do some hand coding of G-code, but as I learn to use the
tools
I have I do less and less of it.


I do have a spare registered dongle for one of the older versions of
MasterCam btw...I was wanting $1000 for it..but ..I might Swap for it.

A weekend of fishing the river and a huge bag of hand injected plastic
baits?

On 2010-07-23, Ignoramus7608 wrote:
On 2010-07-22, DoN. Nichols wrote:
On 2010-07-22, Ignoramus24043 wrote:

[ ... ]

For example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Even better is to ramp down as you circle. Plunging requires a
center-cutting mill. The ramp does not as you get slightly deeper as
you progress.

Great point.

Okay so far.

This really involves two separate concepts:

1) Generating the shape of the cut (circular, in this example)
and
2) Implementing a cut along an arbitrary shape, with several passes if
necessary

Also consider cutter compensation -- telling the CNC machine
what diameter cutter you are using, and which side of the cutter you are
using, and it generates a tool path to produce the shape you want -- or
complains if the drawing calls for a tighter radius in the pocket than
your mill can actually produce. Of course, you don't hit this
particular problem when cutting the outside of a rectangle.

you mean inside rectangle?

No -- I mean *outside* the rectangle. If you are making a
rectangular plateau -- or cutting the outside dimensions of a plate, you
can produce totally square corners -- or round them to whatever degree
you want, with no consideration of the size of the cutter -- as long as
it will fit between the feature you are making and all surrounding ones.

But when doing the *inside* of a rectangle, you *can't* produce
a square corner unless you have a special tool which holds mills at a 45
degree angle and the mills come to a sharp point at just the right
angle. *That* can be fed vertically to make the inside of the corners
sharp. But it will have to be re-oriented for each corner, unless the
workpiece is on a rotary table.

Otherwise, your inside corners are limited to the radius of the
mill being used.

Picture what would happen if you had a 1/2" diameter (1/4"
radius) end mill, and asked it to produce a 1/8" radius in the corners.
If the software is good -- it will simply error out. If not, it will
attempt it, gouging out around the corners. :-)

BTW A trick for roughing vs finish cutting. When you first run the
program -- *lie* to it about the size of the cutter, telling it
that the cutter is N thousandths larger than it really is, so it
will leave "N thousandths"/2 of material on each surface. Then
re-run the program with the true size of the mill entered, and
you will get a finish cut. (You will also waste some machine
time as it re-cuts air in the pocket forming and such, but you
can slightly re-write the program to only do the finish passes
if time is more important to you.

[ ... ]

Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.

This kind of approach, has potential for some very fun results.

Indeed so.

I will first try to just learn G codes, I think, but I started
experimenting with better way of writing those scripts. Basically a
CAM library in perl.

O.K.

But I think that before running, I need to learn to walk, so, I will
practice using G-Codes in a non-idiosyncratic manner.

Yes -- that makes sense. Some things (like blending curves to
straight cuts) may benefit from a CAD program generating the desired
shape, and a CAM one generating the g-Codes as a starting point -- which
could still be hand optimized.

Enjoy,
DoN.

--
Remove oil spill source from e-mail
Email: | Voice (all times): (703) 938-4564
(too) near Washington D.C. | http://www.d-and-d.com/dnichols/DoN.html
--- Black Holes are where God is dividing by zero ---

On Fri, 23 Jul 2010 18:19:07 -0700, "Bob La Londe"
wrote:

"Gunner Asch" wrote in message
.. .
On Fri, 23 Jul 2010 11:58:20 -0700, "Bob La Londe"
wrote:

"Ignoramus24043" wrote in message
news:4f6dne8h2534EtXRnZ2dnUVZ_smdnZ2d@giganews. com...
I had a little light bulb go off in my head.

I think that I know what to do.

I will have functions that could combine different machining notions
together.

For example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Okay so far.

This really involves two separate concepts:

1) Generating the shape of the cut (circular, in this example)
and
2) Implementing a cut along an arbitrary shape, with several passes if
necessary

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.

Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.

This kind of approach, has potential for some very fun results.


Have you looked at Mach 3? It has wizards included that do many of these
functions already. It has a number of lines of code limit, and I think
you
need to register to use the wizards, but its worth a look see.

Have you looked at Cam Bam? They claim it's a beta, but I have done some
real serious detail work with this CAM software, and it even has some
limited CAD capability. The executions limited demo is 100% non crippled,
and the price to register is very reasonable.

If you enjoy writing programs soldier on, but otherwise I think you are
reinventing the wheel.

Yes, I still do some hand coding of G-code, but as I learn to use the
tools
I have I do less and less of it.


I do have a spare registered dongle for one of the older versions of
MasterCam btw...I was wanting $1000 for it..but ..I might Swap for it.

A weekend of fishing the river and a huge bag of hand injected plastic
baits?




You actually interested in it? It has hummm...5 Mastercam versions on it
IRRC..master mill, the lathe thingy and 3 others.

Ill have to go dig it up and refresh my memory as to which version its
good for.

Lots of downloads out there..with the dongle..they are legal. Or mostly
G

Gunner

One could not be a successful Leftwinger without realizing that,
in contrast to the popular conception supported by newspapers
and mothers of Leftwingers, a goodly number of Leftwingers are
not only narrow-minded and dull, but also just stupid.
Gunner Asch

"Gunner Asch" wrote in message
...
On Fri, 23 Jul 2010 18:19:07 -0700, "Bob La Londe"
wrote:

"Gunner Asch" wrote in message
. ..
On Fri, 23 Jul 2010 11:58:20 -0700, "Bob La Londe"
wrote:

"Ignoramus24043" wrote in message
news:4f6dne8h2534EtXRnZ2dnUVZ_smdnZ2d@giganews .com...
I had a little light bulb go off in my head.

I think that I know what to do.

I will have functions that could combine different machining notions
together.

For example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Okay so far.

This really involves two separate concepts:

1) Generating the shape of the cut (circular, in this example)
and
2) Implementing a cut along an arbitrary shape, with several passes if
necessary

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.

Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.

This kind of approach, has potential for some very fun results.


Have you looked at Mach 3? It has wizards included that do many of
these
functions already. It has a number of lines of code limit, and I think
you
need to register to use the wizards, but its worth a look see.

Have you looked at Cam Bam? They claim it's a beta, but I have done
some
real serious detail work with this CAM software, and it even has some
limited CAD capability. The executions limited demo is 100% non
crippled,
and the price to register is very reasonable.

If you enjoy writing programs soldier on, but otherwise I think you are
reinventing the wheel.

Yes, I still do some hand coding of G-code, but as I learn to use the
tools
I have I do less and less of it.


I do have a spare registered dongle for one of the older versions of
MasterCam btw...I was wanting $1000 for it..but ..I might Swap for it.

A weekend of fishing the river and a huge bag of hand injected plastic
baits?




You actually interested in it? It has hummm...5 Mastercam versions on it
IRRC..master mill, the lathe thingy and 3 others.

Ill have to go dig it up and refresh my memory as to which version its
good for.

Lots of downloads out there..with the dongle..they are legal. Or mostly
G

I haven't a clue if I would like Master Cam or not. I have not played with
it at all. For 2D an 2.5D I like Cam Bam a lot. It took me a few weeks to
get a handle on how it works, and if I had time to just sit and play I could
probably have done it in a day or two. Supposedly it does 3D pretty well,
but I have not gotten a 3D CAD program yet that I can use effectively to try
it. I am fighting right now with some shapes that I just can't seem to
backdoor without hand writing the code and using my Excel macro to do the
reiterative work. It's a big pain. However, if I could get the dongle in
exchange for taking you fishing for a couple days (something I would do
anyway)... I would atleast give MasterCam a try. LOL

Ignoramus24043 wrote:
On 2010-07-22, Jon Elson wrote:


The generally suggested method is to ramp down while performing the cut,
rather than plunging in Z and then moving in XY. I have already
converted my "treprect" program that plunged first, then cut around the
rectangular shape, then made a finish pass at full depth. The new
version, which I haven't gotten up on my web page yet ramps down on the
first side of each level.


That actually makes perfect sense. Thanks for bringing this up.

I've posted my treprectramp.c program, which generates G-code to ramp
down while milling along the interior outline of a rectangular cutout,
then makes a finish pass at full depth. See

http://pico-systems.com/treprectramp.c

Jon

On 2010-07-25, Jon Elson wrote:
Ignoramus24043 wrote:
On 2010-07-22, Jon Elson wrote:


The generally suggested method is to ramp down while performing the cut,
rather than plunging in Z and then moving in XY. I have already
converted my "treprect" program that plunged first, then cut around the
rectangular shape, then made a finish pass at full depth. The new
version, which I haven't gotten up on my web page yet ramps down on the
first side of each level.


That actually makes perfect sense. Thanks for bringing this up.

I've posted my treprectramp.c program, which generates G-code to ramp
down while milling along the interior outline of a rectangular cutout,
then makes a finish pass at full depth. See

http://pico-systems.com/treprectramp.c

Jon

Jon, I am writing a function (in perl), to do what you did, but
possibly in multiple passes for many pockets. I will reuse that idea.

After maybe half a year, I will provide it as a module on CPAN.

It would be essentially a library with building blocks for CAM. Could
be useful for someone willing to write a GUI for it or for some
websites.

i

Ignoramus7608 wrote:

If, when using one of your programs, you suddenly hit an emergency
stop button, does your program stop, also? Then are you able to go
back to the operation that stopped and continue on? Something to
consider.


I am not sure, I will check it out.

If his E-stop chain breaks the PPMC estop circuit, then EMC will be
notified of the condition, and it stops, showing the current block of
G-code. EMC continues reading the encoder position all the time, so you
don't have to re-home or reset the part coordinates. Unfortunately,
EMC doesn't handle restarts perfectly seamlessly. You have to click on
the line (or a different program line that is a better/safer start
place) and then select the "start from line" menu. This causes EMC2 to
scan through the program and find the coordinates at the beginning of
the selected move and go there first before resuming. Most of this
works pretty well. One problem is it won't start the spindle and
coolant, etc. So, you have to manually set that first before clicking
the start from line. (There's an option that disables the ability to
start the spindle and go to manual, but this seems to work by default.)
You have to leave the machine in such a position that the restart move
is clear of crashes.

Jon

In article ,
Ignoramus7608 wrote:

On 2010-07-23, wrote:
On Jul 22, 6:21?pm, Ignoramus24043 ignoramus24...@NOSPAM.
24043.invalid wrote:
On 2010-07-23, pyotr filipivich wrote:



Ignoramus24043 on Thu, 22 Jul
2010 14:03:10 -0500 typed in rec.crafts.metalworking ?the following:
On 2010-07-22, Pete C. wrote:

Ignoramus24043 wrote:

I had a little light bulb go off in my head.

I think that I know what to do.

I will have functions that could combine different machining notions
together.

For example, say, I have a steel plate. I could make a circular cut
through it. If the plate is thick or hard, I may need to do it in
several passes, with plunging.

Okay so far.

This really involves two separate concepts:

1) Generating the shape of the cut (circular, in this example)
and
2) Implementing a cut along an arbitrary shape, with several passes if
necessary

If I can do these two tasks separately, then I have a lot of
flexibility, as I could easily cut a square shaped hole in plate, egg
shaped, etc.

Same applies to "milling out a deep pocket along an arbitrary shape".
Generating a shape is one thing, and removing material inside it (in
possibly several layers) is another.

This kind of approach, has potential for some very fun results.

i

You're picking up on what CAM software does. CAD provides the design of
the part, CAM figures out how to make the part essentially.

I think that what I am trying to do, is build a library of functions
to provide CAM functionality.

? ?And is a good thing to understand in and of itself. ? That is,
when I was taking a class on CNC, we started out having to write the
code to move the end mill from point A to point B. ?All the code, all
the way. ?From "turn on spindle" to descend, to enter metal, to move
to starting point, make pass, exit, etc, etc, etc. ?Once we knew what
we wanted, and how it was done, then we moved on to the "neat" CAD/CAM
which let us draw the part, then let the program figure out how to
mill it. ?Even then, it required us to understand the process.

Great approach. Cover the basics first. Since I have a mill, I have to
write all codes etc. (and if I cut its table in half accidentally, it
will be my loss to eat!)

i

If, when using one of your programs, you suddenly hit an emergency
stop button, does your program stop, also? Then are you able to go
back to the operation that stopped and continue on? Something to
consider.

I am not sure, I will check it out.

At the very least, it is very useful to record in non-volatile storage the line
number of the G-code step that was started just before the eStop, as that step
may be the problem.

More generally, I would build a "flight recorder" in, recording say the last 100
codes and their line numbers, the exact time of execution, and an eStop flag to
mark where the airplane crashed.


Joe Gwinn

On Sat, 24 Jul 2010 01:38:30 +0000, DoN. Nichols wrote:
On 2010-07-23, Bob La Londe wrote:
....
Have you looked at Mach 3? It has wizards included that do many of
these functions already. It has a number of lines of code limit, and I
think you need to register to use the wizards, but its worth a look
see.

However -- Mach 3 requires Windows under it, which Iggy does not
care for -- and neither do I -- especially with servos instead of
steppers. If you got a BSOD just after issuing a fast move -- the axis
or axes would keep going until they hit the overrun stops -- even if it
meant moving the cutter (or what was left of it) through the workpiece
which happened to be in the way beyond the planned stop point.
....

[Following is OT in R.C.M so I adjusted Subject]

Some safety systems aboard the Deepwater Horizon were based on
Microsoft Windows NT and got frequent BSOD's. Here's an article
that suggests that use of Microsoft Windows is partly to blame for
sensors and alarms being inhibited aboard the drilling platform:
http://www.examiner.com/x-39728-Tech-Buzz-Examiner~y2010m7d24-Did-BSODs-on-the-Deepwater-Horizon-contribute-to-the-Gulf-oil-disaster

http://techrights.org/2010/07/23/blue-screen-of-death-and-bp/ is
an over-the-top article on the same topic.

--
jiw

On 2010-07-26, James Waldby wrote:
On Sat, 24 Jul 2010 01:38:30 +0000, DoN. Nichols wrote:
On 2010-07-23, Bob La Londe wrote:
...
Have you looked at Mach 3? It has wizards included that do many of
these functions already. It has a number of lines of code limit, and I
think you need to register to use the wizards, but its worth a look
see.

However -- Mach 3 requires Windows under it, which Iggy does not
care for -- and neither do I -- especially with servos instead of
steppers. If you got a BSOD just after issuing a fast move -- the axis
or axes would keep going until they hit the overrun stops -- even if it
meant moving the cutter (or what was left of it) through the workpiece
which happened to be in the way beyond the planned stop point.
...

[Following is OT in R.C.M so I adjusted Subject]

Some safety systems aboard the Deepwater Horizon were based on
Microsoft Windows NT and got frequent BSOD's. Here's an article
that suggests that use of Microsoft Windows is partly to blame for
sensors and alarms being inhibited aboard the drilling platform:
http://www.examiner.com/x-39728-Tech-Buzz-Examiner~y2010m7d24-Did-BSODs-on-the-Deepwater-Horizon-contribute-to-the-Gulf-oil-disaster

http://techrights.org/2010/07/23/blue-screen-of-death-and-bp/ is
an over-the-top article on the same topic.


I really do not care for Windows.There is one thing that I need to do
in Windows -- update maps on my GPS -- and I have been postponing
that.

i

"Ignoramus1880" wrote in message
...
On 2010-07-26, James Waldby wrote:
On Sat, 24 Jul 2010 01:38:30 +0000, DoN. Nichols wrote:
On 2010-07-23, Bob La Londe wrote:
...
Have you looked at Mach 3? It has wizards included that do many of
these functions already. It has a number of lines of code limit, and I
think you need to register to use the wizards, but its worth a look
see.

However -- Mach 3 requires Windows under it, which Iggy does not
care for -- and neither do I -- especially with servos instead of
steppers. If you got a BSOD just after issuing a fast move -- the axis
or axes would keep going until they hit the overrun stops -- even if it
meant moving the cutter (or what was left of it) through the workpiece
which happened to be in the way beyond the planned stop point.
...

[Following is OT in R.C.M so I adjusted Subject]

Some safety systems aboard the Deepwater Horizon were based on
Microsoft Windows NT and got frequent BSOD's. Here's an article
that suggests that use of Microsoft Windows is partly to blame for
sensors and alarms being inhibited aboard the drilling platform:
http://www.examiner.com/x-39728-Tech-Buzz-Examiner~y2010m7d24-Did-BSODs-on-the-Deepwater-Horizon-contribute-to-the-Gulf-oil-disaster

http://techrights.org/2010/07/23/blue-screen-of-death-and-bp/ is
an over-the-top article on the same topic.


I really do not care for Windows.There is one thing that I need to do
in Windows -- update maps on my GPS -- and I have been postponing
that.

Reboot, reboot, reboot. LOL. One thing I like about the version of Ubuntu
distributed with EMC2 is that you can set install it over top of Windows and
set it up for dual boot so you can go to Windows or Linux as needed.

James Waldby wrote:

On Sat, 24 Jul 2010 01:38:30 +0000, DoN. Nichols wrote:
On 2010-07-23, Bob La Londe wrote:
...
Have you looked at Mach 3? It has wizards included that do many of
these functions already. It has a number of lines of code limit, and I
think you need to register to use the wizards, but its worth a look
see.

However -- Mach 3 requires Windows under it, which Iggy does not
care for -- and neither do I -- especially with servos instead of
steppers. If you got a BSOD just after issuing a fast move -- the axis
or axes would keep going until they hit the overrun stops -- even if it
meant moving the cutter (or what was left of it) through the workpiece
which happened to be in the way beyond the planned stop point.
...

[Following is OT in R.C.M so I adjusted Subject]

Some safety systems aboard the Deepwater Horizon were based on
Microsoft Windows NT and got frequent BSOD's. Here's an article
that suggests that use of Microsoft Windows is partly to blame for
sensors and alarms being inhibited aboard the drilling platform:
http://www.examiner.com/x-39728-Tech-Buzz-Examiner~y2010m7d24-Did-BSODs-on-the-Deepwater-Horizon-contribute-to-the-Gulf-oil-disaster

http://techrights.org/2010/07/23/blue-screen-of-death-and-bp/ is
an over-the-top article on the same topic.

We have Mazak Qt-250's and multiplex's using w95 for the hmi, thankfully the backend (NC)
is a mitsubishi processor. That seems to work. W95 didn't try to do to much.

I've had the joy of dealing with a windows based assembly cell. IFix, Kepware,
FactoryTalk, yada. What a steaming pile of chit. Oh yes, to stay on theme, our SCHMIDT®
Servo Presses are running NT4.

Meanwhile back on another line, mostly plc and panelview based, things work fairly well.

Another line also plc based with one win hmi app, I think is factory talk, works fine
software wise, has issues mechanically but we will figure that out eventually.

Windows is fine for desktop apps. It isn't a mission critical OS.



Wes
--
"Additionally as a security officer, I carry a gun to protect
government officials but my life isn't worth protecting at home
in their eyes." Dick Anthony Heller

Wes wrote:

Windows is fine for desktop apps. It isn't a mission critical OS.


NASA uses 'Embedded NT' in some of their telemetry equipment. I
would think that the Space Shttle and the ISS were mission critical.


--
Anyone wanting to run for any political office in the US should have to
have a DD214, and a honorable discharge.