[widgitmaster]

Yesterday I made up 6x tool holders for the Monster, 4x 1/4" & 2x 1/8" & 1x setting gauge. The tool holders are long enough to hit bottom in the spindle's nose, giving me a solid datum to stop against. So the procedure is to measure the length of the setting gauge with a digital caliper, and set it's DRO to zero. Now I can measure the length of the tool holder with a cutter installed, the caliper will automatically deduct the length of the setting guage and give me the tool's cutter length.

Now I can enter all the tool lengths into Mach3, and use the z-tool setting block to set tool#0 to Z-zero. I have written a template G-Code with all the offsets & coordinates for manual tool changing, all I need to do is cut & paste the g-codes from VCarve-Pro into the template. This process works great, and speeds up production on many items I make, at least it does on my little machine in the back room!

For some reason, Mach3 is ignoring the T1 & H1 commands, and continuously uses tool #0


(Set Z=0 on top of part )
(G54 Set x,y,z zero at HOME position)
(G56 Center of and Z-Zero +0.750 above fixture top)

(Tool#1 .625 Dia x0.75 endmill)
(Tool#2 .250 Dia x0.50 endmill)
(Tool#3 .750 Dia 60-Deg V-Bit)
(Tool#4 .250 Dia x0.75 endmill)

G40 G17 G80 G50 G90 G56
G49 M5
G0 X0 Y-10.400 Z4.600 (tool change position)

M1

T1 H1 (Tool#1 .625 Dia x0.75 endmill)
S25000 M3 G04 P10
(-----------------------------------------------)
(insert code here)
(-----------------------------------------------)
G0 Z0.8000
G49 M5
G0 X0 Y-10.400 Z4.600 (tool change position)

M1

T2 H2 (Tool#2 .250 Dia x0.50 endmill)
S25000 M3 G04 P10
(-----------------------------------------------)
(insert code here)
(-----------------------------------------------)
G0 Z0.8000
G49 M5
G0 X0 Y-10.400 Z4.600 (tool change position)

M1

T3 H3 (Tool#3 .750 Dia 60-Deg V-Bit)
S25000 M3 G04 P10
(-----------------------------------------------)
(insert code here)
(-----------------------------------------------)
G0 Z0.8000
G49 M5
G0 X0 Y-10.400 Z4.600 (tool change position)

M1

T4 H4 (Tool#4 .250 Dia x0.75 endmill)
S25000 M3 G04 P10
(-----------------------------------------------)
(insert code here)
(-----------------------------------------------)
G0 Z0.8000
M5



Can anyone tell me why the tool lengths are being ignored by Mach3?
Widgit

[mactec54]

widgitmaster

You don't use the G54 for your machine home, that is only for your work offsets X 0.0 Y0.0 these will be set at a number that your work piece is from your machine home, You don't have to do anything with the machine Home number

You also have not done a call G43 Z.1H1 this is your tool comp number/call

N1G17G40G80
M5 (don't need this at the start of the program)
G0Z4.600
G90G0 X0 Y-10.400 (tool change position) ( don't do a Z move with a X Y move or some time down the road you will crash)
M1

T1
G54
S25000 M3 G04 P10
G90G0X-----------Y------------- (start to cut position)
G43Z.1H1
G1Z-????? ( Z depth of cut)

Don't use G49 this can get things messed up this cancels tool offsets which you don't need to do

[tauntdesigns]

Those tool holders look pretty sweet.

On your G-code( it's been a while since I programmed g-code with length comp )

I believe you need a line to pick up the tool offset.

T1 (Tool#1 .625 Dia x0.75 endmill)
S25000 M3 G04 P10
(-----------------------------------------------)
g0g43 h1 z1.
x0y0
g1z.2f10.
z-.05f5.
g03x-.25y0i-.125j0f5.
x-.25y0i.25j0
x-.5y0i-.125j0
x-.5y0i.5j0
x-.726y0i-.113j0
x-.726y0i.726j0
x-.736y0i-.005j0
x-.736y0i.736j0f8.0
x0y0i.368j0f20.
(-----------------------------------------------)
G0 Z0.8000
G49 M5
G0 X0 Y-10.400 Z4.600 (tool change position)

It worked on my control

Jack

(Keep a hand on the e-stop............ it's been a while for me)

[tauntdesigns]

Oops, I was typing and trying my input while you posted your answer....lol

[widgitmaster]

Thanks guys!

Did I get it right?

(Set Z=0 on top of part )
(G56 X0 Y0 fixture center)

(Tool#1 .625 Dia x0.75 endmill)
(Tool#2 .250 Dia x0.50 endmill)
(Tool#3 .750 Dia 60-Deg V-Bit)
(Tool#4 .250 Dia x0.75 endmill)

G40 G17 G80
G49 M5
G0 X0 Y-10.400 (tool change position)
G0 Z4.600

M1

T1 (Tool#1 .625 Dia x0.75 endmill)
G56
S25000 M3 G04 P10
G43 H1
G90
(-----------------------------------------------)
( insert code here)
(-----------------------------------------------)
G49 M5
G0 X0 Y-10.400 (tool change position)
G0 Z4.600

M1

T2 (Tool#2 .250 Dia x0.50 endmill)
G56
S25000 M3 G04 P10
G43 H2
G90
(-----------------------------------------------)
( insert code here)
(-----------------------------------------------)
G49 M5
G0 X0 Y-10.400 (tool change position)
G0 Z4.600

M1

T3 (Tool#3 .750 Dia 60-Deg V-Bit)
G56
S25000 M3 G04 P10
G43 H3
G90
(-----------------------------------------------)
( insert code here)
(-----------------------------------------------)
G49 M5
G0 X0 Y-10.400 (tool change position)
G0 Z4.600

M1

T4 (Tool#4 .250 Dia x0.75 endmill)
G56
S25000 M3 G04 P10
G43 H4
G90
(-----------------------------------------------)
( insert code here)
(-----------------------------------------------)
G0 Z0.8000
M5
G0 X0.0 Y18.2 Z6.0 (park away from fixture for part loading)
M30

[CarveOne]

Wigit,

If you select all vectors when creating a tool path it will jump around randomly. Most of the tool path types have a "Use vector selection order" option that might help. I haven't had the troubles you mention when using the offset mode though. I tend to use raster cuts when doing 3D finishing tool paths for Aspire projects that have models, but it depends on what I'm cutting. If significantly sized pieces of MDF are breaking off, that seems like a very soft type of MDF.with very little glue in the mix. The type I get at the local Lowes is a darker variety than some of it I see posted on the CNC Zone. When cutters are getting dull it will cause this more frequently.

[mactec54]

widgitmaster

No you still have some G49 in there, this will cancel the tool offset, & you don't want to do that

(Set Z=0 on top of part )
(G56 X0 Y0 fixture center)

(Tool#1 .625 Dia x0.75 endmill)
(Tool#2 .250 Dia x0.50 endmill)
(Tool#3 .750 Dia 60-Deg V-Bit)
(Tool#4 .250 Dia x0.75 endmill)

G40 G17 G80
G0 Z4.600 (Z move Before a X Y Move )
G0 X0 Y-10.400 (tool change position)

M1

T1 (Tool#1 .625 Dia x0.75 endmill)
G56
S25000 M3 G04 P10
G43 H1
G90
(-----------------------------------------------)
( insert code here)
(-----------------------------------------------)
M5
G0 Z4.600 (Z Move before a X Y Move )
G0 X0 Y-10.400 (tool change position)


M1

T2 (Tool#2 .250 Dia x0.50 endmill)
G56
S25000 M3 G04 P10
G43 H2
G90
(-----------------------------------------------)
( insert code here)
(-----------------------------------------------)
M5
G0 Z4.600
G0 X0 Y-10.400 (tool change position)


M1

T3 (Tool#3 .750 Dia 60-Deg V-Bit)
G56
S25000 M3 G04 P10
G43 H3
G90
(-----------------------------------------------)
( insert code here)
(-----------------------------------------------)
M5
G0 Z4.600
G0 X0 Y-10.400 (tool change position)


M1

T4 (Tool#4 .250 Dia x0.75 endmill)
G56
S25000 M3 G04 P10
G43 H4
G90
(-----------------------------------------------)
( insert code here)
(-----------------------------------------------)
G0 Z6.0 ( I changed this Z move to here )
M5
G0 X0.0 Y18.2 ( No Z move on this line Do your clearance Z move at the end of your program ) (park away from fixture for part loading)
M30

[tauntdesigns]

That code picks up the tool comp in my simulator.

Are you using positive or negative tool comp offsets?

On the tool change Z move, is that Z absolute machine coordinate?

[mactec54]

That code picks up the tool comp in my simulator.


On the tool change Z move, is that Z absolute machine coordinate?

If you are using G90 which widget is, all the Z moves will be absolute

[tauntdesigns]

If you are using G90 which widget is, all the Z moves will be absolute

My bad, I meant....... is the tool change Z position Machine or workpiece coordinates?
If Machine coordinates, I'd use a G53 calls:
G53 x0y-10.4
G53 z4.6

G49's can be dangerous if precautions are not taken
If you don't remove the tool offset the z4.6 could limit the z-axis in the plus direction(if the g53 is not used).

[mactec54]

My bad, I meant....... is the tool change Z position Machine or workpiece coordinates?
If Machine coordinates, I'd use a G53 calls:
G53 x0y-10.4
G53 z4.6

G49's can be dangerous if precautions are not taken
If you don't remove the tool offset the z4.6 could limit the z-axis in the plus direction(if the g53 is not used).

Keep it simple

G53 are not needed for any type of normal programing/machining operations

[tauntdesigns]

Keep it simple

G53 are not needed for any type of normal programing/machining operations

Cheers,

[widgitmaster]

Well, ALL I can say is THANK YOU!!

The template worked perfectly, as all I needed to do was tweak the feed rates!

Thanks again!
Widgit

[tauntdesigns]

Looks good Widget

[mactec54]

widgitmaster

Nice Job as usual Widgit,are you still using your small machine or do you like this one better

[widgitmaster]

widgitmaster

Nice Job as usual Widgit,are you still using your small machine or do you like this one better

Thanks Mac!
I'm using both of them, the one in the back room has been setup for a 6x9 plaques for over a month now! I run off 5 plaques every morning!
The monster just makes bigger stuff which take longer to run! But I love it

Hey, does anyone know how to Diamond-Drag a soft brass plate? Where do I get the drag tooling?
Widgit

[mactec54]

Thanks Mac!
I'm using both of them, the one in the back room has been setup for a 6x9 plaques for over a month now! I run off 5 plaques every morning!
The monster just makes bigger stuff which take longer to run! But I love it

Hey, does anyone know how to Diamond-Drag a soft brass plate? Where do I get the drag tooling?
Widgit

They have a lot on your favorite place Ebay, You could make your own body, & just buy the Diamond part

[aarggh]

That's a brilliant idea Widgit, do you mind putting a link up where you found that model blower? I'd be interested myself in one.

cheers, Ian

[zer0fighter]

Random question, is that Mach 4 beta? Looks a lot different than my Mach 3.

Sent from my SGH-I337M using Tapatalk

[widgitmaster]

Random question, is that Mach 4 beta? Looks a lot different than my Mach 3.

Sent from my SGH-I337M using Tapatalk

No it's Mach3 with the Big Tex Blue-Screen! I needed it to access the Z-Tool setting block !