I was making a mold for wax yesterday. The shape is a cone, the size
of a hockey puck (2.3 inches on top, about 1.9 inches on bottom, 1
inch deep), with some features on the bottom.


\ /
\ /
-_-------_-

The material was 6061 aluminum. I did it with my own G code that I
generated to smooth the side of the cone, the bottom etc.

2400 RPM, 3/8" ball endmill.

The only really bad thing about this is that it took 50 minutes to
complete. This really sucked for two reasons, one is that it wounded
my pride and took a long time to watch, and two, the machine would
wear itself unnecessarily while running sub-optimal code. I was
cleaning the shop at the same time, so this time was not fully wasted,
but still it was ridiculous.

So, let's say that instead of me, with 3 hours of CNC experience, an
expert CNC machinist was programming my Bridgeport Interact mill and
had to use the same speed (no crazy 50k RPM machines!). That expert
could use any common solid endmill, such as ball or square ended,
proper coolant, select feed speeds up to 60 IPM as appropriate, RPM up
to 2,400 etc.

He could be limited by what my machine can do.

So, if that expert could do a better job programming, how long would
this CNC job take? 2.5 by 1 inch deep cone profile. I used a 0.04"
vertical step to finish the sides of the cone.

I know that I should have used a square ended endmill for roughing out
and for smoothing the bottom.

i

On 8/3/2010 8:18 AM, Ignoramus30076 wrote:
I was making a mold for wax yesterday. The shape is a cone, the size
of a hockey puck (2.3 inches on top, about 1.9 inches on bottom, 1
inch deep), with some features on the bottom.


\ /
\ /
-_-------_-

The material was 6061 aluminum. I did it with my own G code that I
generated to smooth the side of the cone, the bottom etc.

2400 RPM, 3/8" ball endmill.

The only really bad thing about this is that it took 50 minutes to
complete. This really sucked for two reasons, one is that it wounded
my pride and took a long time to watch, and two, the machine would
wear itself unnecessarily while running sub-optimal code. I was
cleaning the shop at the same time, so this time was not fully wasted,
but still it was ridiculous.

So, let's say that instead of me, with 3 hours of CNC experience, an
expert CNC machinist was programming my Bridgeport Interact mill and
had to use the same speed (no crazy 50k RPM machines!). That expert
could use any common solid endmill, such as ball or square ended,
proper coolant, select feed speeds up to 60 IPM as appropriate, RPM up
to 2,400 etc.

He could be limited by what my machine can do.

So, if that expert could do a better job programming, how long would
this CNC job take? 2.5 by 1 inch deep cone profile. I used a 0.04"
vertical step to finish the sides of the cone.

I know that I should have used a square ended endmill for roughing out
and for smoothing the bottom.

i

There's alot you could do.. You could plunge out a center hole with a
drill, then go in with a 1/2" cutter to get the meat out, then come in
with your ballmill to finish..

Your really limited with your 2400 max RPM.. I could see doing 60ipm @
2400 rpm at .04 DOC (equates to ~ .025 total chipload) if you had most
of the meat taken out already.

The ballmill is going to take long regardless. But if you use it just
for finishing it should run alot faster.

Ignoramus30076 wrote:

I was making a mold for wax yesterday. The shape is a cone, the size
of a hockey puck (2.3 inches on top, about 1.9 inches on bottom, 1
inch deep), with some features on the bottom.

\ /
\ /
-_-------_-

The material was 6061 aluminum. I did it with my own G code that I
generated to smooth the side of the cone, the bottom etc.

2400 RPM, 3/8" ball endmill.

The only really bad thing about this is that it took 50 minutes to
complete. This really sucked for two reasons, one is that it wounded
my pride and took a long time to watch, and two, the machine would
wear itself unnecessarily while running sub-optimal code. I was
cleaning the shop at the same time, so this time was not fully wasted,
but still it was ridiculous.

So, let's say that instead of me, with 3 hours of CNC experience, an
expert CNC machinist was programming my Bridgeport Interact mill and
had to use the same speed (no crazy 50k RPM machines!). That expert
could use any common solid endmill, such as ball or square ended,
proper coolant, select feed speeds up to 60 IPM as appropriate, RPM up
to 2,400 etc.

He could be limited by what my machine can do.

So, if that expert could do a better job programming, how long would
this CNC job take? 2.5 by 1 inch deep cone profile. I used a 0.04"
vertical step to finish the sides of the cone.

I know that I should have used a square ended endmill for roughing out
and for smoothing the bottom.

i

10 minutes, not counting the tool change.

Roughing with a square end end mill, 4 minutes since the regular end
mill can take pretty heavy cuts on AL and your pattern doesn't have any
corners to slow the process based on max decel and accel rates, just one
big spiral down taking advantage of your 3 HP spindle and coolant to
flush the chips away.

Change tools to the ball end mill.

Finish pass with the ball end mill 6 minutes since you have very little
material left to remove, cutting with the angled side of the ball end
mill (adjust your chip load calculations for the diameter at the point
you're cutting with) and can run a higher than normal feed rate since
you're removing a little triangle step, not a full cut, so your chip
load can be higher and your feed rate very high even though your spindle
tops out at 3,000 RPM.

On 2010-08-03, tnik wrote:
On 8/3/2010 8:18 AM, Ignoramus30076 wrote:
I was making a mold for wax yesterday. The shape is a cone, the size
of a hockey puck (2.3 inches on top, about 1.9 inches on bottom, 1
inch deep), with some features on the bottom.


\ /
\ /
-_-------_-

The material was 6061 aluminum. I did it with my own G code that I
generated to smooth the side of the cone, the bottom etc.

2400 RPM, 3/8" ball endmill.

The only really bad thing about this is that it took 50 minutes to
complete. This really sucked for two reasons, one is that it wounded
my pride and took a long time to watch, and two, the machine would
wear itself unnecessarily while running sub-optimal code. I was
cleaning the shop at the same time, so this time was not fully wasted,
but still it was ridiculous.

So, let's say that instead of me, with 3 hours of CNC experience, an
expert CNC machinist was programming my Bridgeport Interact mill and
had to use the same speed (no crazy 50k RPM machines!). That expert
could use any common solid endmill, such as ball or square ended,
proper coolant, select feed speeds up to 60 IPM as appropriate, RPM up
to 2,400 etc.

He could be limited by what my machine can do.

So, if that expert could do a better job programming, how long would
this CNC job take? 2.5 by 1 inch deep cone profile. I used a 0.04"
vertical step to finish the sides of the cone.

I know that I should have used a square ended endmill for roughing out
and for smoothing the bottom.

i

There's alot you could do.. You could plunge out a center hole with a
drill, then go in with a 1/2" cutter to get the meat out, then come in
with your ballmill to finish..

Your really limited with your 2400 max RPM.. I could see doing 60ipm @
2400 rpm at .04 DOC (equates to ~ .025 total chipload) if you had most
of the meat taken out already.

Yes. The mill could go higher (to 4,200 RPM) but I would not want to
do it for an extended period.

The ballmill is going to take long regardless. But if you use it just
for finishing it should run alot faster.

I agree. I think that I should use this case to perfect my skills.

i

On 2010-08-03, Pete C. wrote:

Ignoramus30076 wrote:

I was making a mold for wax yesterday. The shape is a cone, the size
of a hockey puck (2.3 inches on top, about 1.9 inches on bottom, 1
inch deep), with some features on the bottom.

\ /
\ /
-_-------_-

The material was 6061 aluminum. I did it with my own G code that I
generated to smooth the side of the cone, the bottom etc.

2400 RPM, 3/8" ball endmill.

The only really bad thing about this is that it took 50 minutes to
complete. This really sucked for two reasons, one is that it wounded
my pride and took a long time to watch, and two, the machine would
wear itself unnecessarily while running sub-optimal code. I was
cleaning the shop at the same time, so this time was not fully wasted,
but still it was ridiculous.

So, let's say that instead of me, with 3 hours of CNC experience, an
expert CNC machinist was programming my Bridgeport Interact mill and
had to use the same speed (no crazy 50k RPM machines!). That expert
could use any common solid endmill, such as ball or square ended,
proper coolant, select feed speeds up to 60 IPM as appropriate, RPM up
to 2,400 etc.

He could be limited by what my machine can do.

So, if that expert could do a better job programming, how long would
this CNC job take? 2.5 by 1 inch deep cone profile. I used a 0.04"
vertical step to finish the sides of the cone.

I know that I should have used a square ended endmill for roughing out
and for smoothing the bottom.

i

10 minutes, not counting the tool change.

Roughing with a square end end mill, 4 minutes since the regular end
mill can take pretty heavy cuts on AL and your pattern doesn't have any
corners to slow the process based on max decel and accel rates, just one
big spiral down taking advantage of your 3 HP spindle and coolant to
flush the chips away.

Change tools to the ball end mill.

Finish pass with the ball end mill 6 minutes since you have very little
material left to remove, cutting with the angled side of the ball end
mill (adjust your chip load calculations for the diameter at the point
you're cutting with) and can run a higher than normal feed rate since
you're removing a little triangle step, not a full cut, so your chip
load can be higher and your feed rate very high even though your spindle
tops out at 3,000 RPM.

Sounds pretty good. I will try to do it this way (on smaller size to
save material). I bought about 120-150 lbs of Aluminum a few months
ago, I should have gotten more then, which I could.

i

Ignoramus30076 wrote:

Yes. The mill could go higher (to 4,200 RPM) but I would not want to
do it for an extended period.

Do a search on the McMaster site for "temperature labels" and add a pack
of them to your next order. Stick a couple on key spindle areas. ~$1 ea
in 10 packs is pretty cheap.

On 2010-08-03, Pete C. wrote:

Ignoramus30076 wrote:

Yes. The mill could go higher (to 4,200 RPM) but I would not want to
do it for an extended period.

Do a search on the McMaster site for "temperature labels" and add a pack
of them to your next order. Stick a couple on key spindle areas. ~$1 ea
in 10 packs is pretty cheap.

Interesting. I added one sheet. My spindle is covered with oil, but
maybe a label would stay long enough to be useful,

i

Ignoramus30076 wrote:

On 2010-08-03, Pete C. wrote:

Ignoramus30076 wrote:

Yes. The mill could go higher (to 4,200 RPM) but I would not want to
do it for an extended period.

Do a search on the McMaster site for "temperature labels" and add a pack
of them to your next order. Stick a couple on key spindle areas. ~$1 ea
in 10 packs is pretty cheap.

Interesting. I added one sheet. My spindle is covered with oil, but
maybe a label would stay long enough to be useful,

i

There are all kinds of solvents for removing that oil before applying
the label. Since the labels are intended for industrial use, I expect
they have pretty good adhesive.

Ignoramus30076 wrote:

I was making a mold for wax yesterday. The shape is a cone, the size
of a hockey puck (2.3 inches on top, about 1.9 inches on bottom, 1
inch deep), with some features on the bottom.

\ /
\ /
-_-------_-

The material was 6061 aluminum. I did it with my own G code that I
generated to smooth the side of the cone, the bottom etc.

2400 RPM, 3/8" ball endmill.

The only really bad thing about this is that it took 50 minutes to
complete. This really sucked for two reasons, one is that it wounded
my pride and took a long time to watch, and two, the machine would
wear itself unnecessarily while running sub-optimal code. I was
cleaning the shop at the same time, so this time was not fully wasted,
but still it was ridiculous.

So, let's say that instead of me, with 3 hours of CNC experience, an
expert CNC machinist was programming my Bridgeport Interact mill and
had to use the same speed (no crazy 50k RPM machines!). That expert
could use any common solid endmill, such as ball or square ended,
proper coolant, select feed speeds up to 60 IPM as appropriate, RPM up
to 2,400 etc.

He could be limited by what my machine can do.

So, if that expert could do a better job programming, how long would
this CNC job take? 2.5 by 1 inch deep cone profile. I used a 0.04"
vertical step to finish the sides of the cone.

I know that I should have used a square ended endmill for roughing out
and for smoothing the bottom.

i

BTW, when you're producing your G-code, you should be simulating it /
estimating run time (I presume EMC2 has these functions for offline use)
so you can see where you need to optimize the code. In my setup, I do my
CAD/CAM in my office and run a copy of Mach3 there as well for
simulation and estimation independent of my actual CNC machine(s) in my
detached shop.

On 2010-08-03, Pete C. wrote:

Ignoramus30076 wrote:

I was making a mold for wax yesterday. The shape is a cone, the size
of a hockey puck (2.3 inches on top, about 1.9 inches on bottom, 1
inch deep), with some features on the bottom.

\ /
\ /
-_-------_-

The material was 6061 aluminum. I did it with my own G code that I
generated to smooth the side of the cone, the bottom etc.

2400 RPM, 3/8" ball endmill.

The only really bad thing about this is that it took 50 minutes to
complete. This really sucked for two reasons, one is that it wounded
my pride and took a long time to watch, and two, the machine would
wear itself unnecessarily while running sub-optimal code. I was
cleaning the shop at the same time, so this time was not fully wasted,
but still it was ridiculous.

So, let's say that instead of me, with 3 hours of CNC experience, an
expert CNC machinist was programming my Bridgeport Interact mill and
had to use the same speed (no crazy 50k RPM machines!). That expert
could use any common solid endmill, such as ball or square ended,
proper coolant, select feed speeds up to 60 IPM as appropriate, RPM up
to 2,400 etc.

He could be limited by what my machine can do.

So, if that expert could do a better job programming, how long would
this CNC job take? 2.5 by 1 inch deep cone profile. I used a 0.04"
vertical step to finish the sides of the cone.

I know that I should have used a square ended endmill for roughing out
and for smoothing the bottom.

i

BTW, when you're producing your G-code, you should be simulating it /
estimating run time (I presume EMC2 has these functions for offline use)
so you can see where you need to optimize the code. In my setup, I do my
CAD/CAM in my office and run a copy of Mach3 there as well for
simulation and estimation independent of my actual CNC machine(s) in my
detached shop.

I have not done that yet, but I should look into it.

What do you personally use for CAD/CAM?

I have an example job: the aluminum cover for the servo motor on the
rotary table, is too shallow to for the encoder to hide udner it. So,
I will try to make a new aluminum cap.

So I need to design a machining job to reduce a square aluminum plate
to become a round cap-shaped object with four holes drilled (to be
tapped).

This seems like a good case to try out some CAD/CAM things out there.

i
i

Ignoramus30076 wrote:

On 2010-08-03, Pete C. wrote:

Ignoramus30076 wrote:

I was making a mold for wax yesterday. The shape is a cone, the size
of a hockey puck (2.3 inches on top, about 1.9 inches on bottom, 1
inch deep), with some features on the bottom.

\ /
\ /
-_-------_-

The material was 6061 aluminum. I did it with my own G code that I
generated to smooth the side of the cone, the bottom etc.

2400 RPM, 3/8" ball endmill.

The only really bad thing about this is that it took 50 minutes to
complete. This really sucked for two reasons, one is that it wounded
my pride and took a long time to watch, and two, the machine would
wear itself unnecessarily while running sub-optimal code. I was
cleaning the shop at the same time, so this time was not fully wasted,
but still it was ridiculous.

So, let's say that instead of me, with 3 hours of CNC experience, an
expert CNC machinist was programming my Bridgeport Interact mill and
had to use the same speed (no crazy 50k RPM machines!). That expert
could use any common solid endmill, such as ball or square ended,
proper coolant, select feed speeds up to 60 IPM as appropriate, RPM up
to 2,400 etc.

He could be limited by what my machine can do.

So, if that expert could do a better job programming, how long would
this CNC job take? 2.5 by 1 inch deep cone profile. I used a 0.04"
vertical step to finish the sides of the cone.

I know that I should have used a square ended endmill for roughing out
and for smoothing the bottom.

i

BTW, when you're producing your G-code, you should be simulating it /
estimating run time (I presume EMC2 has these functions for offline use)
so you can see where you need to optimize the code. In my setup, I do my
CAD/CAM in my office and run a copy of Mach3 there as well for
simulation and estimation independent of my actual CNC machine(s) in my
detached shop.

I have not done that yet, but I should look into it.

What do you personally use for CAD/CAM?

TurboCAD and SheetCAM.


I have an example job: the aluminum cover for the servo motor on the
rotary table, is too shallow to for the encoder to hide udner it. So,
I will try to make a new aluminum cap.

So I need to design a machining job to reduce a square aluminum plate
to become a round cap-shaped object with four holes drilled (to be
tapped).

This seems like a good case to try out some CAD/CAM things out there.

Yep, and it sounds like a pretty simple job as well. If you'd like, you
could email me the specs, dimensions, end mill you want to use, etc. and
I could produce a CAD DXF and G-code for you to play with.

On 2010-08-03, Pete C. wrote:

Ignoramus30076 wrote:

On 2010-08-03, Pete C. wrote:

Ignoramus30076 wrote:

I was making a mold for wax yesterday. The shape is a cone, the size
of a hockey puck (2.3 inches on top, about 1.9 inches on bottom, 1
inch deep), with some features on the bottom.

\ /
\ /
-_-------_-

The material was 6061 aluminum. I did it with my own G code that I
generated to smooth the side of the cone, the bottom etc.

2400 RPM, 3/8" ball endmill.

The only really bad thing about this is that it took 50 minutes to
complete. This really sucked for two reasons, one is that it wounded
my pride and took a long time to watch, and two, the machine would
wear itself unnecessarily while running sub-optimal code. I was
cleaning the shop at the same time, so this time was not fully wasted,
but still it was ridiculous.

So, let's say that instead of me, with 3 hours of CNC experience, an
expert CNC machinist was programming my Bridgeport Interact mill and
had to use the same speed (no crazy 50k RPM machines!). That expert
could use any common solid endmill, such as ball or square ended,
proper coolant, select feed speeds up to 60 IPM as appropriate, RPM up
to 2,400 etc.

He could be limited by what my machine can do.

So, if that expert could do a better job programming, how long would
this CNC job take? 2.5 by 1 inch deep cone profile. I used a 0.04"
vertical step to finish the sides of the cone.

I know that I should have used a square ended endmill for roughing out
and for smoothing the bottom.

i

BTW, when you're producing your G-code, you should be simulating it /
estimating run time (I presume EMC2 has these functions for offline use)
so you can see where you need to optimize the code. In my setup, I do my
CAD/CAM in my office and run a copy of Mach3 there as well for
simulation and estimation independent of my actual CNC machine(s) in my
detached shop.

I have not done that yet, but I should look into it.

What do you personally use for CAD/CAM?

TurboCAD and SheetCAM.


I have an example job: the aluminum cover for the servo motor on the
rotary table, is too shallow to for the encoder to hide udner it. So,
I will try to make a new aluminum cap.

So I need to design a machining job to reduce a square aluminum plate
to become a round cap-shaped object with four holes drilled (to be
tapped).

This seems like a good case to try out some CAD/CAM things out there.

Yep, and it sounds like a pretty simple job as well. If you'd like, you
could email me the specs, dimensions, end mill you want to use, etc. and
I could produce a CAD DXF and G-code for you to play with.

There is SheetCAM for Linux. I will try it and I will buy it if I like
it. So you make your design in TurboCAD, export a DXF, and then give
it to SheetCAM?

Do you have any simple DXF drawings that you could email me? I want to
evaluate this SheetCAM.

i

Ignoramus30076 wrote:

On 2010-08-03, Pete C. wrote:

Ignoramus30076 wrote:

On 2010-08-03, Pete C. wrote:

Ignoramus30076 wrote:

I was making a mold for wax yesterday. The shape is a cone, the size
of a hockey puck (2.3 inches on top, about 1.9 inches on bottom, 1
inch deep), with some features on the bottom.

\ /
\ /
-_-------_-

The material was 6061 aluminum. I did it with my own G code that I
generated to smooth the side of the cone, the bottom etc.

2400 RPM, 3/8" ball endmill.

The only really bad thing about this is that it took 50 minutes to
complete. This really sucked for two reasons, one is that it wounded
my pride and took a long time to watch, and two, the machine would
wear itself unnecessarily while running sub-optimal code. I was
cleaning the shop at the same time, so this time was not fully wasted,
but still it was ridiculous.

So, let's say that instead of me, with 3 hours of CNC experience, an
expert CNC machinist was programming my Bridgeport Interact mill and
had to use the same speed (no crazy 50k RPM machines!). That expert
could use any common solid endmill, such as ball or square ended,
proper coolant, select feed speeds up to 60 IPM as appropriate, RPM up
to 2,400 etc.

He could be limited by what my machine can do.

So, if that expert could do a better job programming, how long would
this CNC job take? 2.5 by 1 inch deep cone profile. I used a 0.04"
vertical step to finish the sides of the cone.

I know that I should have used a square ended endmill for roughing out
and for smoothing the bottom.

i

BTW, when you're producing your G-code, you should be simulating it /
estimating run time (I presume EMC2 has these functions for offline use)
so you can see where you need to optimize the code. In my setup, I do my
CAD/CAM in my office and run a copy of Mach3 there as well for
simulation and estimation independent of my actual CNC machine(s) in my
detached shop.

I have not done that yet, but I should look into it.

What do you personally use for CAD/CAM?

TurboCAD and SheetCAM.


I have an example job: the aluminum cover for the servo motor on the
rotary table, is too shallow to for the encoder to hide udner it. So,
I will try to make a new aluminum cap.

So I need to design a machining job to reduce a square aluminum plate
to become a round cap-shaped object with four holes drilled (to be
tapped).

This seems like a good case to try out some CAD/CAM things out there.

Yep, and it sounds like a pretty simple job as well. If you'd like, you
could email me the specs, dimensions, end mill you want to use, etc. and
I could produce a CAD DXF and G-code for you to play with.

There is SheetCAM for Linux. I will try it and I will buy it if I like
it. So you make your design in TurboCAD, export a DXF, and then give
it to SheetCAM?

Do you have any simple DXF drawings that you could email me? I want to
evaluate this SheetCAM.

i

It's a bit more complicated that exporting a DXF to SheetCAM and telling
it to have at it. In SheetCAM you need to select the various layers from
your CAD print, and apply processes to them, specifying the various
parameters for each process such as end mill diameter, spindle speed,
feed rate, etc. You do this for each layer in your CAD print, and
different layers can specify different tools and processes, like mill on
one layer, drill holes on another layer, etc. I'll email you a DXF with
some simple shapes on different layers to play with.

On 2010-08-03, Pete C. wrote:
It's a bit more complicated that exporting a DXF to SheetCAM and telling
it to have at it. In SheetCAM you need to select the various layers from
your CAD print, and apply processes to them, specifying the various
parameters for each process such as end mill diameter, spindle speed,
feed rate, etc. You do this for each layer in your CAD print, and
different layers can specify different tools and processes, like mill on
one layer, drill holes on another layer, etc. I'll email you a DXF with
some simple shapes on different layers to play with.

Thanks a lot. I had some progress. I loaded your DXF, and specified
twp operations: spiral pocket of the square and spiral pocket of the
hexagon.

Then I ran a post processor.

It created a file PeteC.tap:

(Filename: PeteC.tap)
(Post processor: EMC.scpost)
(Date: 03/08/10)
G20 (Units: Inches)
G40 G90
F1
(Part: Shapes)
(Operation: Spiral pocket, Square, T1: Mill/router, 0.375 inch
diameter, 0.6 inch Deep)
M6 T1 (Mill/router, 0.375 inch diameter)
G43 H1
G00 Z0.1575
M03 S2000
(Operation: Spiral pocket, Hexagon, T1: Mill/router, 0.375 inch
diameter, 0.3 inch Deep)
M05
M05 M30

I have a feeling that I did not specify material. I will keep looking.

i

Ignoramus30076 wrote:

On 2010-08-03, Pete C. wrote:
It's a bit more complicated that exporting a DXF to SheetCAM and telling
it to have at it. In SheetCAM you need to select the various layers from
your CAD print, and apply processes to them, specifying the various
parameters for each process such as end mill diameter, spindle speed,
feed rate, etc. You do this for each layer in your CAD print, and
different layers can specify different tools and processes, like mill on
one layer, drill holes on another layer, etc. I'll email you a DXF with
some simple shapes on different layers to play with.

Thanks a lot. I had some progress. I loaded your DXF, and specified
twp operations: spiral pocket of the square and spiral pocket of the
hexagon.

Then I ran a post processor.

It created a file PeteC.tap:

(Filename: PeteC.tap)
(Post processor: EMC.scpost)
(Date: 03/08/10)
G20 (Units: Inches)
G40 G90
F1
(Part: Shapes)
(Operation: Spiral pocket, Square, T1: Mill/router, 0.375 inch
diameter, 0.6 inch Deep)
M6 T1 (Mill/router, 0.375 inch diameter)
G43 H1
G00 Z0.1575
M03 S2000
(Operation: Spiral pocket, Hexagon, T1: Mill/router, 0.375 inch
diameter, 0.3 inch Deep)
M05
M05 M30

I have a feeling that I did not specify material. I will keep looking.

i

Yep, it takes some experimenting to get an understanding of how the
process works. I've mostly done CNC plasma, so that process is a bit
different than milling. When I finish re-retrofitting my little CNC mini
mill I'll be using the milling functions more.

Don't forget to run simulations to watch the toolpath plot and see what
the code is actually doing, and eventually test the code on your
machinable wax.

On 2010-08-03, Pete C. wrote:

Ignoramus30076 wrote:

On 2010-08-03, Pete C. wrote:
It's a bit more complicated that exporting a DXF to SheetCAM and telling
it to have at it. In SheetCAM you need to select the various layers from
your CAD print, and apply processes to them, specifying the various
parameters for each process such as end mill diameter, spindle speed,
feed rate, etc. You do this for each layer in your CAD print, and
different layers can specify different tools and processes, like mill on
one layer, drill holes on another layer, etc. I'll email you a DXF with
some simple shapes on different layers to play with.

Thanks a lot. I had some progress. I loaded your DXF, and specified
twp operations: spiral pocket of the square and spiral pocket of the
hexagon.

Then I ran a post processor.

It created a file PeteC.tap:

(Filename: PeteC.tap)
(Post processor: EMC.scpost)
(Date: 03/08/10)
G20 (Units: Inches)
G40 G90
F1
(Part: Shapes)
(Operation: Spiral pocket, Square, T1: Mill/router, 0.375 inch
diameter, 0.6 inch Deep)
M6 T1 (Mill/router, 0.375 inch diameter)
G43 H1
G00 Z0.1575
M03 S2000
(Operation: Spiral pocket, Hexagon, T1: Mill/router, 0.375 inch
diameter, 0.3 inch Deep)
M05
M05 M30

I have a feeling that I did not specify material. I will keep looking.

i

Yep, it takes some experimenting to get an understanding of how the
process works. I've mostly done CNC plasma, so that process is a bit
different than milling. When I finish re-retrofitting my little CNC mini
mill I'll be using the milling functions more.

Don't forget to run simulations to watch the toolpath plot and see what
the code is actually doing, and eventually test the code on your
machinable wax.

Yes, for sure, thanks

i

Ignoramus30076 wrote:

So, let's say that instead of me, with 3 hours of CNC experience, an
expert CNC machinist was programming my Bridgeport Interact mill and
had to use the same speed (no crazy 50k RPM machines!). That expert
could use any common solid endmill, such as ball or square ended,
proper coolant, select feed speeds up to 60 IPM as appropriate, RPM up
to 2,400 etc.

Us a tapered end mill to match the sidewall draft angle. Mill out with
a large end mill, then change to the tapered mill for the finish cut.

Very fast.

Jon

"Ignoramus30076" wrote in message
...
On 2010-08-03, Pete C. wrote:

Ignoramus30076 wrote:

I was making a mold for wax yesterday. The shape is a cone, the size
of a hockey puck (2.3 inches on top, about 1.9 inches on bottom, 1
inch deep), with some features on the bottom.

\ /
\ /
-_-------_-

The material was 6061 aluminum. I did it with my own G code that I
generated to smooth the side of the cone, the bottom etc.

2400 RPM, 3/8" ball endmill.

The only really bad thing about this is that it took 50 minutes to
complete. This really sucked for two reasons, one is that it wounded
my pride and took a long time to watch, and two, the machine would
wear itself unnecessarily while running sub-optimal code. I was
cleaning the shop at the same time, so this time was not fully wasted,
but still it was ridiculous.

So, let's say that instead of me, with 3 hours of CNC experience, an
expert CNC machinist was programming my Bridgeport Interact mill and
had to use the same speed (no crazy 50k RPM machines!). That expert
could use any common solid endmill, such as ball or square ended,
proper coolant, select feed speeds up to 60 IPM as appropriate, RPM up
to 2,400 etc.

He could be limited by what my machine can do.

So, if that expert could do a better job programming, how long would
this CNC job take? 2.5 by 1 inch deep cone profile. I used a 0.04"
vertical step to finish the sides of the cone.

I know that I should have used a square ended endmill for roughing out
and for smoothing the bottom.

i

BTW, when you're producing your G-code, you should be simulating it /
estimating run time (I presume EMC2 has these functions for offline use)
so you can see where you need to optimize the code. In my setup, I do my
CAD/CAM in my office and run a copy of Mach3 there as well for
simulation and estimation independent of my actual CNC machine(s) in my
detached shop.

I have not done that yet, but I should look into it.

What do you personally use for CAD/CAM?

I have an example job: the aluminum cover for the servo motor on the
rotary table, is too shallow to for the encoder to hide udner it. So,
I will try to make a new aluminum cap.

So I need to design a machining job to reduce a square aluminum plate
to become a round cap-shaped object with four holes drilled (to be
tapped).

This seems like a good case to try out some CAD/CAM things out there.

i
i

For parametric 3D CAD, check out Alibre. There is a 30-day trial version
that used to turn into a free, limited feature version, but I think that
they've stopped marketing the free version. The most basic version is only
$100 though and that should do most of what you want. It's a Windows only
program though. I'm not sure but the $100 version might come with some
basic CAM functionality.

On 2010-08-04, Mike Henry wrote:

"Ignoramus30076" wrote in message
...
On 2010-08-03, Pete C. wrote:

Ignoramus30076 wrote:

I was making a mold for wax yesterday. The shape is a cone, the size
of a hockey puck (2.3 inches on top, about 1.9 inches on bottom, 1
inch deep), with some features on the bottom.

\ /
\ /
-_-------_-

The material was 6061 aluminum. I did it with my own G code that I
generated to smooth the side of the cone, the bottom etc.

2400 RPM, 3/8" ball endmill.

The only really bad thing about this is that it took 50 minutes to
complete. This really sucked for two reasons, one is that it wounded
my pride and took a long time to watch, and two, the machine would
wear itself unnecessarily while running sub-optimal code. I was
cleaning the shop at the same time, so this time was not fully wasted,
but still it was ridiculous.

So, let's say that instead of me, with 3 hours of CNC experience, an
expert CNC machinist was programming my Bridgeport Interact mill and
had to use the same speed (no crazy 50k RPM machines!). That expert
could use any common solid endmill, such as ball or square ended,
proper coolant, select feed speeds up to 60 IPM as appropriate, RPM up
to 2,400 etc.

He could be limited by what my machine can do.

So, if that expert could do a better job programming, how long would
this CNC job take? 2.5 by 1 inch deep cone profile. I used a 0.04"
vertical step to finish the sides of the cone.

I know that I should have used a square ended endmill for roughing out
and for smoothing the bottom.

i

BTW, when you're producing your G-code, you should be simulating it /
estimating run time (I presume EMC2 has these functions for offline use)
so you can see where you need to optimize the code. In my setup, I do my
CAD/CAM in my office and run a copy of Mach3 there as well for
simulation and estimation independent of my actual CNC machine(s) in my
detached shop.

I have not done that yet, but I should look into it.

What do you personally use for CAD/CAM?

I have an example job: the aluminum cover for the servo motor on the
rotary table, is too shallow to for the encoder to hide udner it. So,
I will try to make a new aluminum cap.

So I need to design a machining job to reduce a square aluminum plate
to become a round cap-shaped object with four holes drilled (to be
tapped).

This seems like a good case to try out some CAD/CAM things out there.

i
i

For parametric 3D CAD, check out Alibre. There is a 30-day trial version
that used to turn into a free, limited feature version, but I think that
they've stopped marketing the free version. The most basic version is only
$100 though and that should do most of what you want. It's a Windows only
program though. I'm not sure but the $100 version might come with some
basic CAM functionality.


Mike, I am looking at this Alibre. I do not really mind paying some
money.

The question that I currently have, is is there some kind of a 4D
software that could do 4D CAM.

i

Ignoramus30382 wrote:

On 2010-08-04, Mike Henry wrote:

"Ignoramus30076" wrote in message
...
On 2010-08-03, Pete C. wrote:

Ignoramus30076 wrote:

I was making a mold for wax yesterday. The shape is a cone, the size
of a hockey puck (2.3 inches on top, about 1.9 inches on bottom, 1
inch deep), with some features on the bottom.

\ /
\ /
-_-------_-

The material was 6061 aluminum. I did it with my own G code that I
generated to smooth the side of the cone, the bottom etc.

2400 RPM, 3/8" ball endmill.

The only really bad thing about this is that it took 50 minutes to
complete. This really sucked for two reasons, one is that it wounded
my pride and took a long time to watch, and two, the machine would
wear itself unnecessarily while running sub-optimal code. I was
cleaning the shop at the same time, so this time was not fully wasted,
but still it was ridiculous.

So, let's say that instead of me, with 3 hours of CNC experience, an
expert CNC machinist was programming my Bridgeport Interact mill and
had to use the same speed (no crazy 50k RPM machines!). That expert
could use any common solid endmill, such as ball or square ended,
proper coolant, select feed speeds up to 60 IPM as appropriate, RPM up
to 2,400 etc.

He could be limited by what my machine can do.

So, if that expert could do a better job programming, how long would
this CNC job take? 2.5 by 1 inch deep cone profile. I used a 0.04"
vertical step to finish the sides of the cone.

I know that I should have used a square ended endmill for roughing out
and for smoothing the bottom.

i

BTW, when you're producing your G-code, you should be simulating it /
estimating run time (I presume EMC2 has these functions for offline use)
so you can see where you need to optimize the code. In my setup, I do my
CAD/CAM in my office and run a copy of Mach3 there as well for
simulation and estimation independent of my actual CNC machine(s) in my
detached shop.

I have not done that yet, but I should look into it.

What do you personally use for CAD/CAM?

I have an example job: the aluminum cover for the servo motor on the
rotary table, is too shallow to for the encoder to hide udner it. So,
I will try to make a new aluminum cap.

So I need to design a machining job to reduce a square aluminum plate
to become a round cap-shaped object with four holes drilled (to be
tapped).

This seems like a good case to try out some CAD/CAM things out there.

i
i

For parametric 3D CAD, check out Alibre. There is a 30-day trial version
that used to turn into a free, limited feature version, but I think that
they've stopped marketing the free version. The most basic version is only
$100 though and that should do most of what you want. It's a Windows only
program though. I'm not sure but the $100 version might come with some
basic CAM functionality.


Mike, I am looking at this Alibre. I do not really mind paying some
money.

The question that I currently have, is is there some kind of a 4D
software that could do 4D CAM.

i

Remember that the CAM part is a separate piece. CAD does the design, CAM
figures out how to make it. The standard version of TurboCAD runs about
$100 as well, and there is a TurboCAM available as well (forget the
price). I haven't tried the TurboCAM yet since SheetCAM works well for
the mostly CNC plasma cutting I've been doing.

On that 4D thing, you can get creative on that depending on what you're
doing. If you looked at my pano bracket project, you saw the CNC
engraving of the round degree scales with an improvised 4th axis setup.
For the G-code for that I simply generated the code as a flat strip,
with the length matching the circumference of the part and treated the
rotary axis as a linear one.

On Aug 5, 8:28*am, "Pete C." wrote:

On that 4D thing, you can get creative on that depending on what you're
doing. If you looked at my pano bracket project, you saw the CNC
engraving of the round degree scales with an improvised 4th axis setup.
For the G-code for that I simply generated the code as a flat strip,
with the length matching the circumference of the part and treated the
rotary axis as a linear one

I seem to have missed that one, but it sounds interesting. Could you
post a link?

Thanks

Pete, my first thought on this 4D is kind of a simple one -- I could
use it to machine both sides of a part in one setup. Say, machine both
sides, add rounded corners etc, and then cut off in the last step.

i

"Ignoramus16841" wrote in message
...
Pete, my first thought on this 4D is kind of a simple one -- I could
use it to machine both sides of a part in one setup. Say, machine both
sides, add rounded corners etc, and then cut off in the last step.

i

I must have missed something. What do you mean by "4D"? Are you talking
about simultaneous 4-axis machining?

--
Ed Huntress

"Ignoramus30382" wrote in message
...
On 2010-08-04, Mike Henry wrote:

"Ignoramus30076" wrote in message
...
On 2010-08-03, Pete C. wrote:

Ignoramus30076 wrote:

I was making a mold for wax yesterday. The shape is a cone, the size
of a hockey puck (2.3 inches on top, about 1.9 inches on bottom, 1
inch deep), with some features on the bottom.

\ /
\ /
-_-------_-

The material was 6061 aluminum. I did it with my own G code that I
generated to smooth the side of the cone, the bottom etc.

2400 RPM, 3/8" ball endmill.

The only really bad thing about this is that it took 50 minutes to
complete. This really sucked for two reasons, one is that it wounded
my pride and took a long time to watch, and two, the machine would
wear itself unnecessarily while running sub-optimal code. I was
cleaning the shop at the same time, so this time was not fully wasted,
but still it was ridiculous.

So, let's say that instead of me, with 3 hours of CNC experience, an
expert CNC machinist was programming my Bridgeport Interact mill and
had to use the same speed (no crazy 50k RPM machines!). That expert
could use any common solid endmill, such as ball or square ended,
proper coolant, select feed speeds up to 60 IPM as appropriate, RPM up
to 2,400 etc.

He could be limited by what my machine can do.

So, if that expert could do a better job programming, how long would
this CNC job take? 2.5 by 1 inch deep cone profile. I used a 0.04"
vertical step to finish the sides of the cone.

I know that I should have used a square ended endmill for roughing out
and for smoothing the bottom.

i

BTW, when you're producing your G-code, you should be simulating it /
estimating run time (I presume EMC2 has these functions for offline
use)
so you can see where you need to optimize the code. In my setup, I do
my
CAD/CAM in my office and run a copy of Mach3 there as well for
simulation and estimation independent of my actual CNC machine(s) in my
detached shop.

I have not done that yet, but I should look into it.

What do you personally use for CAD/CAM?

I have an example job: the aluminum cover for the servo motor on the
rotary table, is too shallow to for the encoder to hide udner it. So,
I will try to make a new aluminum cap.

So I need to design a machining job to reduce a square aluminum plate
to become a round cap-shaped object with four holes drilled (to be
tapped).

This seems like a good case to try out some CAD/CAM things out there.

i
i

For parametric 3D CAD, check out Alibre. There is a 30-day trial version
that used to turn into a free, limited feature version, but I think that
they've stopped marketing the free version. The most basic version is
only
$100 though and that should do most of what you want. It's a Windows
only
program though. I'm not sure but the $100 version might come with some
basic CAM functionality.


Mike, I am looking at this Alibre. I do not really mind paying some
money.

The question that I currently have, is is there some kind of a 4D
software that could do 4D CAM.

i

If you want to do 3D or 4th axis CAM you will probably need to spend some
serious money. I use SprutCAM (written in Russia) and the 4th-axis capable
version of that runs around $4k. That's one of the cheaper programs out
there, I think.

There's nothing to prevent writing your own code for flipping a part on a
rotary table though and that would may require only a couple of lines of
G-code.

On 2010-08-05, Ed Huntress wrote:

"Ignoramus16841" wrote in message
...
Pete, my first thought on this 4D is kind of a simple one -- I could
use it to machine both sides of a part in one setup. Say, machine both
sides, add rounded corners etc, and then cut off in the last step.

i

I must have missed something. What do you mean by "4D"? Are you talking
about simultaneous 4-axis machining?


I am not sure about simultaneous, but I am working towards using 4
axes for machining.

On 2010-08-05, Mike Henry wrote:

"Ignoramus30382" wrote in message
...
On 2010-08-04, Mike Henry wrote:

"Ignoramus30076" wrote in message
...
On 2010-08-03, Pete C. wrote:

Ignoramus30076 wrote:

I was making a mold for wax yesterday. The shape is a cone, the size
of a hockey puck (2.3 inches on top, about 1.9 inches on bottom, 1
inch deep), with some features on the bottom.

\ /
\ /
-_-------_-

The material was 6061 aluminum. I did it with my own G code that I
generated to smooth the side of the cone, the bottom etc.

2400 RPM, 3/8" ball endmill.

The only really bad thing about this is that it took 50 minutes to
complete. This really sucked for two reasons, one is that it wounded
my pride and took a long time to watch, and two, the machine would
wear itself unnecessarily while running sub-optimal code. I was
cleaning the shop at the same time, so this time was not fully wasted,
but still it was ridiculous.

So, let's say that instead of me, with 3 hours of CNC experience, an
expert CNC machinist was programming my Bridgeport Interact mill and
had to use the same speed (no crazy 50k RPM machines!). That expert
could use any common solid endmill, such as ball or square ended,
proper coolant, select feed speeds up to 60 IPM as appropriate, RPM up
to 2,400 etc.

He could be limited by what my machine can do.

So, if that expert could do a better job programming, how long would
this CNC job take? 2.5 by 1 inch deep cone profile. I used a 0.04"
vertical step to finish the sides of the cone.

I know that I should have used a square ended endmill for roughing out
and for smoothing the bottom.

i

BTW, when you're producing your G-code, you should be simulating it /
estimating run time (I presume EMC2 has these functions for offline
use)
so you can see where you need to optimize the code. In my setup, I do
my
CAD/CAM in my office and run a copy of Mach3 there as well for
simulation and estimation independent of my actual CNC machine(s) in my
detached shop.

I have not done that yet, but I should look into it.

What do you personally use for CAD/CAM?

I have an example job: the aluminum cover for the servo motor on the
rotary table, is too shallow to for the encoder to hide udner it. So,
I will try to make a new aluminum cap.

So I need to design a machining job to reduce a square aluminum plate
to become a round cap-shaped object with four holes drilled (to be
tapped).

This seems like a good case to try out some CAD/CAM things out there.

i
i

For parametric 3D CAD, check out Alibre. There is a 30-day trial version
that used to turn into a free, limited feature version, but I think that
they've stopped marketing the free version. The most basic version is
only
$100 though and that should do most of what you want. It's a Windows
only
program though. I'm not sure but the $100 version might come with some
basic CAM functionality.


Mike, I am looking at this Alibre. I do not really mind paying some
money.

The question that I currently have, is is there some kind of a 4D
software that could do 4D CAM.

i

If you want to do 3D or 4th axis CAM you will probably need to spend some
serious money. I use SprutCAM (written in Russia) and the 4th-axis capable
version of that runs around $4k. That's one of the cheaper programs out
there, I think.

There's nothing to prevent writing your own code for flipping a part on a
rotary table though and that would may require only a couple of lines of
G-code.


May even be one line, like G0 A180 or something. Just making it up.

Even machining a screw type of surface could be a few lines, like say
if I want to cut a 1/4" deep helical groove in 1 inch stock

(move to starting point)
G0 x0 Y1

(plunge)
G1 Y0.75 F5

(cut helical screw)
G1 X2 R1800

(entirely made up example, may not even be correct).

The more general example of simultaneous could be trickier.

i

"Ignoramus16841" wrote in message
news
On 2010-08-05, Ed Huntress wrote:

"Ignoramus16841" wrote in message
...
Pete, my first thought on this 4D is kind of a simple one -- I could
use it to machine both sides of a part in one setup. Say, machine both
sides, add rounded corners etc, and then cut off in the last step.

i

I must have missed something. What do you mean by "4D"? Are you talking
about simultaneous 4-axis machining?


I am not sure about simultaneous, but I am working towards using 4
axes for machining.

If it's two, 2- or 3-axis machining steps in sequence (as in machining two
sides of a part in separate, sequential operations), that's just two simpler
programs with some kind of indexing step in between. If your part is mounted
on a horizontal or vertical indexing table, you just put a 180-degree
rotation in the middle of the program. You might call that 3-1/2 axis
machining.

If you're talking about machining with four axes simultaneously --
programming moves in your indexing table while you're machining with the
other axes, for example -- that gets really interesting. Five axes are even
more interesting. d8-)

Duplex milling, machining with two spindles on opposite sides of a
workpiece, is another issue. You may be interested to see that but of course
it's not relevant to your situation:

http://www.mmsonline.com/videos/vide...duplex-milling

It seems unlikely you'll be ready for more than three axes until you get
more experience. Most five-axis work is for machining undercuts and really
difficult geometry in moldmaking, skelatonizing aerospace parts, etc., with
pivoting-spindle machines.

Your ambition is laudable but you're trying to run before you walk.

--
Ed Huntress

On 2010-08-05, Ed Huntress wrote:

"Ignoramus16841" wrote in message
news
On 2010-08-05, Ed Huntress wrote:

"Ignoramus16841" wrote in message
...
Pete, my first thought on this 4D is kind of a simple one -- I could
use it to machine both sides of a part in one setup. Say, machine both
sides, add rounded corners etc, and then cut off in the last step.

i

I must have missed something. What do you mean by "4D"? Are you talking
about simultaneous 4-axis machining?


I am not sure about simultaneous, but I am working towards using 4
axes for machining.

If it's two, 2- or 3-axis machining steps in sequence (as in machining two
sides of a part in separate, sequential operations), that's just two simpler
programs with some kind of indexing step in between. If your part is mounted
on a horizontal or vertical indexing table, you just put a 180-degree
rotation in the middle of the program. You might call that 3-1/2 axis
machining.

If you're talking about machining with four axes simultaneously --
programming moves in your indexing table while you're machining with the
other axes, for example -- that gets really interesting. Five axes are even
more interesting. d8-)

Duplex milling, machining with two spindles on opposite sides of a
workpiece, is another issue. You may be interested to see that but of course
it's not relevant to your situation:

http://www.mmsonline.com/videos/vide...duplex-milling

It seems unlikely you'll be ready for more than three axes until you get
more experience. Most five-axis work is for machining undercuts and really
difficult geometry in moldmaking, skelatonizing aerospace parts, etc., with
pivoting-spindle machines.

Your ambition is laudable but you're trying to run before you walk.


Yes. I agree.

i