Threading on Lathe

I am trying to write a threading operation for my smithy lathe. Below is the code, but it will not load. Here are the errors I am getting.

line 9 cannot G01 with no feed rate (this probably just needs changed to G00)
line 11 k word missing with g33/g33.1
If some of you guys that know more about code than me could look this over, I would appreciate it.

G20
G64
(TOOL #3 60 DEG. 1/8 0.003 RADTHREADING)
T03M6
G18 G7
G00 X1.1 Z.0461 S200 M3
G94
N1 G00 X1.2 Z.0312
N2 G01 X.9828
N3 G33 Z-.3729 F.031
N4 G00 X1.2
N5 G00 Z.0201
N6 G01 X.9699
N7 G33 Z-.3729 F.031
N8 G00 X1.2
N9 G00 Z.0117
N10 G01 X.9603
N11 G33 Z-.3729 F.031
N12 G00 X1.2
N13 G00 Z.0055
N14 G01 X.9531
N15 G33 Z-.3729 F.031
N16 G00 X1.2
N17 G00 Z.0009
N18 G01 X.9478
N19 G33 Z-.3729 F.031
N20 G00 X1.2
N21 G00 Z-.0008
N22 G01 X.9459
N23 G33 Z-.3729 F.031
N24 G00 X1.2
N25 G00 Z-.0008
N26 G01 X.9459
N27 G33 Z-.3729 F.031
N28 G00 X1.2
N29 G00 Z-.0008
N30 G01 X.9459
N31 G33 Z-.3729 F.031
N32 G00 X1.2
G00 X2.
G00 Z1.
M5
M2
%

Two points:
EMC2 doesn't need line numbers, and ignores them.
Do you have a reason not to use G76?
www.linuxcnc.org/docview/html//gcode_mai...76:-Threading-Canned

To answer your actual question,

Line 9, you can either change it to a G0, or add an F (feed) to the G1 line.

iLine 11: EMC2 G33 uses a K parameter not an F parameter (it describes a slightly different concept, and you probably don't want G33 to alter your feed rate for other operations). Just swap the F to a K and it ought to work.

So G76 is what I need? Where do I need to put the G76.
The line #'s are just there because that is the way my software posted it out.

Thanks!

andypugh wrote:

To answer your actual question,

Line 9, you can either change it to a G0, or add an F (feed) to the G1 line.

iLine 11: EMC2 G33 uses a K parameter not an F parameter (it describes a slightly different concept, and you probably don't want G33 to alter your feed rate for other operations). Just swap the F to a K and it ought to work.

Thanks alot. I will give it a shot!

dp427tt wrote:

So G76 is what I need? Where do I need to put the G76.

G76 will replace just about all of your code.
(Do an air-cut first, I have a feeling that some numbers (I J and K) might need to be doubled/halved in G7 mode.)
I assume that you have a spindle encoder fitted?

G20
G64
(TOOL #3 60 DEG. 1/8 0.003 RADTHREADING)
T03M6
G18 G7
G00 X1.1 Z.0461 S200 M3
G94

G00 X1.2 Z.0312
G76 Z-.3729 P 0.031 I 0.2 J 0.02 K 0.0541 R1.5 Q29.5 H2
M2
%