Gear Cutting Wizard

[Peterb33]

I have been trying to use the gear cutting wizard for a while and it does all of the right things for number of teeth, cut depth etc., but I cannot make sense of the start position, I must be missing something!

Where should the cutter be placed relative to the workpiece when the axis are zero'd? When I click start cycle the Y axis moves a large amount, from one side of the work piece to the other and then the movements for the cutting cycle start?

Peter

[Hood]

Is that the spline and gear cutting wizard? If yes then ot would seem the Y zero should be centre of shaft.
Hood

[Overloaded]

Y zero is the centerline of the tool on the centerline of the rotary spindle / blank.
The wizard the uses the entries for the mat. and tool dia. to program the Y positions for the cuts in X.
Set the X start and feed dist. to suit.
Dont go to Y0 or you will likely crash to the centerline of the A axis ! unless you are well clear in X.

[Peterb33]

Yes, it is the gear and spline cutting wizard. Tried setting the Y axis 0 as centre of shaft but still moves one side of the blank to the other so not sure what happening really

While I was waiting for reply I decided to have a go try and write something.

Based on the G code the gear wizard generates, I managed to write what is below to cut a 108 tooth gear. Never written any G code before and chuffed it works even though it's simple!
Ideally I would like to have 5 passes of cut depth 0.05mm, and rather than put each one in as separate lines in the code, can a sub program be entered to do these passes then move the A axis and repeat and how would I do it?

Thanks

M04 S4000
G00 G64 A0
M98 P0001 Q108
M5
M30

O0001
G01 Y1.5
G01 X-25 F50
G00 Y-3
G00 X0
G00 Y0
G01 Y2.54
G01 X-25 F50
G00 Y-3
G00 X0
G91 A3.3333
Y0
G90
M99

[rcaffin]

Based on the G code the gear wizard generates, I managed to write what is below to cut a 108 tooth gear. Never written any G code before and chuffed it works even though it's simple!

Ah, a slippery slope into g-code addiction. :-)
Next stop, parametric.  :-)

Ideally I would like to have 5 passes of cut depth 0.05mm, and rather than put each one in as separate lines in the code, can a sub program be entered to do these passes then move the A axis and repeat and how would I do it?

Yes. You can do it using incremental mode, but that can be tricky to debug. Alternately, go parametric, which is easy.

ASSUME X=0 is on the gear axis (This is different from your code)
ASSUME radius of blank is R  (you need to substitute real values of course)
ASSUME cut depth is C (=0.05 in your case)
ASSUME number of cuts is N (=5 in your case)
ASSUME gear blank left side is Y=-1
ASSUME gear blank right side is Y=+1
Note: Mach uses defined parameters as set up in the first few line below.

Program:
#1=R           % you have to insert real values here!
#2=C
#3=N
#4=[0-#1]    % This starts at the surface of the blank, south of X=0
m3
f50 S4000
G64
G00 x[#4-5] A0       % clearance of 5 units south of gear
M98 P0001 Q108     % number of teeth
M5
M30

% cut one tooth
O0001
#5=#4               % reset X start position - crucial!
m98 p0002 Q#3  % make N passes for this tooth
g0 x[#1-5]
G91 A3.3333       % next tooth
m99

% do single cut
o0002
G0 X[#5-5]    % clearance
G0 Y-1.5        % start 0.5 to the left of the blank
G0 X#5         % move to face of gear blank (but offset to left)
#5=[#5-#2]    % move in one cut depth - key to whole idea
G1 Y1.5         % cut to right of gear blank
G0 X[#5-5]     % get clear again
G0 Y-1.5        % go back to left side
m99

CAUTION: you will need to set the gear blank up and do all the prelim stuff yourself. Correctness of code NOT garranteed!

Cheers