[Fastest1]

Sharpie for a reference? Might be repeatable to what .1"?

[Potatohead908]

Sharpie for a reference? Might be repeatable to what .1"?

If your a Special kind of Special maybe. I'm a pessimist too so I know where your coming from though.

[Fastest1]

Pessimist? We have machines that can cut at tolerances well under .001 and you think you can eyeball a close proximity? Get your calipers out again and look at how small of an increment we are talking. If close is good enough.

[Potatohead908]

" If close is good enough." Yes, maybe....depends. Not arguing or trying to ruffle feathers. Real quick I wanted to point out I was talking about a reference point on a drill bit. I think if you marked it right you could get really close. Close enough I don't know. Would I recommend it? NO.

[Potatohead908]

I'm pulling my hair out. I haven't gotten to the ice pic in the eye yet. I am getting an error in Mach3 saying that my soft limits exceeded and I think it's in the Z axis. I don't know if it's because the tool table in my CAM are being posted in the G-code and Mach3 is adding it's tool table lengths to that.... Can someone send me a sample G-code that they know is good. I don't know if it's my CAM or POST or what.

The beginning of the G-code is:

; T2 D=0.375 CR=0 - ZMIN=0 - FLAT END MILL
: G90 G40 G94
G17
G70
M26
; 2D POCKET2
M9
M26
:T2 M6
; 2 FLUTE FLAT ENDMILL
M26
S1540 M3
H0
M8
G0 X2.0651 Y1.178
Z1.795
Z1.3969
G1 Z0.9325 F28
X2.0662 Y1.1775 Z0.923 F23
X2.0695 Y1.1761 Z0.9141
X2.0749 Y1.174 Z0.9064
X2.0819 Y1.1716 Z0.9004
X2.0903 Y1.1691 Z0.8966

[SCzEngrgGroup]

You should NOT have any M26s in your program. That is re-setting machine zero, which will lead to all kinds of nasty problems.

Regards,
Ray L.

[Potatohead908]

Thanks Ray. Any ideas how it is being inserted? I will ask on the HSM forum.

[Potatohead908]

I founded it. It was under the file save format. I had it set to mach2mill format. But when I went back to look I saw it had a .NC format. Changed it back to mach2mill and THEN changed my file save location. Came back and it was back in the .NC format. Yet another bug in Mach3 ver. .66. I am gong to find out what is the better version and reinstall that instead of .66

This is the new G-code using the .tap format.

(1)
(T2 D=0.375 CR=0. - ZMIN=0. - FLAT END MILL)
G90 G94 G17
G20
G28 G91 Z0.
G90

(2D POCKET2)
M5
M9
T2 M6
(2 FLUTE FLAT ENDMILL)
S1540 M3
G54
M8
G0 X2.0651 Y1.178
G43 Z1.795 H0
Z1.3969
G1 Z0.9325 F28.
G3 X2.0662 Y1.1775 Z0.923 I0.0718 J0.163 F23.
X2.0695 Y1.1761 Z0.9141 I0.0706 J0.1635
X2.0749 Y1.174 Z0.9064 I0.0673 J0.1649
X2.0819 Y1.1716 Z0.9004 I0.062 J0.167
X2.0903 Y1.1691 Z0.8966 I0.055 J0.1694
X2.0995 Y1.1669 Z0.895 I0.0466 J0.1719
X2.1743 Y1.5152 Z0.8755 I0.0374 J0.1742
X2.0995 Y1.1669 Z0.8559 I-0.0374 J-0.1742
X2.1743 Y1.5152 Z0.8364 I0.0374 J0.1742
X2.0995 Y1.1669 Z0.8168 I-0.0374 J-0.1742
X2.1743 Y1.5152 Z0.7973 I0.0374 J0.1742
X2.0995 Y1.1669 Z0.7778 I-0.0374 J-0.1742

[LeeWay]

Mach will open several types of files and remembers the last type it tried to open. Just hover over the options and select all to see all the files it will open or pick .tap or .txt.

Also in your code, the number behind the H in the middle is the way that Mach knows which offset to put with that tool. It should be H2 for tool number 2.
Go back into your tool definition in HSM and on the first screen, make sure the tool number and offset numbers(not actual offsets) match.
That should help.

[AVRnj]

I have my Gcode like this for tool changes:

T35 M06 G43 H35 T35 for tool 35, m06 for tool change, G43 for offset, H35 for offset value, as LeeWay mentioned, this should match your T value in HSM, and this tells Mach3 to use the offset value for this tool

This always works for me, have to make sure HSM is not putting any negating codes in there too, usually it should work, but test with air before you do anything.

[SCzEngrgGroup]

I have my Gcode like this for tool changes:

T35 M06 G43 H35 T35 for tool 35, m06 for tool change, G43 for offset, H35 for offset value, as LeeWay mentioned, this should match your T value in HSM, and this tells Mach3 to use the offset value for this tool

This always works for me, have to make sure HSM is not putting any negating codes in there too, usually it should work, but test with air before you do anything.

Keep in mind too that the order in which the "words" appear on the line makes no difference at all. All of the following will execute identically:

G43 H35 T35 M06
T35 H35 M06 G43
M06 G43 T35 H35
T35 M06 G43 H35
or any of the other possible permutations....

And the G43 Hn need not be on the same line as the M6 Tn. It may appear either on a line before or after the M6 Tn, and the code will execute the same, providing there are no Z axis moves between the two.

Regards,
Ray L.

[Potatohead908]

Mach will open several types of files and remembers the last type it tried to open. Just hover over the options and select all to see all the files it will open or pick .tap or .txt.

Also in your code, the number behind the H in the middle is the way that Mach knows which offset to put with that tool. It should be H2 for tool number 2.
Go back into your tool definition in HSM and on the first screen, make sure the tool number and offset numbers(not actual offsets) match.
That should help.

Perfect! I was wondering why I couldn't insert decimals in there. Thank you LeeWay!

[Potatohead908]

Thank you Ray and AVRnj. I will be cutting air and then wood at first. I will have more questions today I am sure.

[Potatohead908]

Success!! Thanks again for all the help! Now to build an enclosure and flood coolant system!

[LeeWay]

Enclosure first.

[Potatohead908]

I cant wait for an enclosure and a hose to flush it out with!