[Jake@SRM]

Hi guys. I wish to use the M19 orient spindle function with a single point custom ground tool to cut a 56 tooth spline into an aluminium hub. I have done a couple of test and in principle the theroy works fine, however programming is a pain in the ass. I have OneCNC mill, however this broaching facility is not in there (no surprises).
I would love to know a quick way of writing a program which will:

Orient Spindle for tooth 1 (0 degrees)
Perform reciprocating motion whilst increasing radial depth of cut (say 8 cuts)
Orient Spindle for tooth 2 (6.4285 degrees)
Perform reciprocating motion whilst increasing radial depth of cut (say 8 cuts)
Orient Spindle for tooth 3 (12.871 degrees)
and so on.

Any ideas how to write a quick program which will perform this? :wave:

[Machineit]

Hi guys. I wish to use the M19 orient spindle function with a single point custom ground tool to cut a 56 tooth spline into an aluminium hub. I have done a couple of test and in principle the theroy works fine, however programming is a pain in the ass. I have OneCNC mill, however this broaching facility is not in there (no surprises).
I would love to know a quick way of writing a program which will:

Orient Spindle for tooth 1 (0 degrees)
Perform reciprocating motion whilst increasing radial depth of cut (say 8 cuts)
Orient Spindle for tooth 2 (6.4285 degrees)
Perform reciprocating motion whilst increasing radial depth of cut (say 8 cuts)
Orient Spindle for tooth 3 (12.871 degrees)
and so on.

Any ideas how to write a quick program which will perform this? :wave:

Just use a sub-routine or a sub-program. Rotate to your location then call sub. In the main call for L55 6.4285, which will repeat the process 55 more times to complete 56 splines. The whole program could be about 30 lines of code.

The use of subs and "L" - loop commands is very neat!

Not sure how this would be done on a spindle orient, but may be very similar to and A axis program.

Mike

[KenFoulks]

You will have to use R instead of P, because of the decimal value. Try using a sub like this:


G103 P1 (Limit block look ahead)
#100= 0 (Set to Zero for 1st run)
M97 P1 L56 (Run sub #1 56 times)
M30

N1 M19 R#100 (Orient to variable #100 value)
M97 P2
#100= #100+ 6.4285 (Increment degree variable)
M99

N2 G91 (sub to broach)
(20 lines or so here)
M99

[WallyL7]

Did something really similar to this...but was able to cheat and use a rotary table. Super simple sub program with -Y- moves for nibbling out the material, then a quick -A- move of the rotary and run the sub again...etc.

Not sure if you have that option.

[Jake@SRM]

Cheers for the replies guys, much appreciated!

I don't have a rotary table that'd be too easy anyways ;-)

Ken & Mike, your way looks cool, very versatile to cut different splines, I have had a quick try and it works (with Macro's trial on - never played with these before) cheers, I will play some more til it does what its told!

[Jake@SRM]

Ok so this is the first time I've used macros, but it works! (Haas TM-1)
I had a problem that the M19 would orient the wrong direction, so I set up #104 which counts down from 360. Also I had to use M19 Pxx instead of M19 Rxx so I'm not sure if its using the decimals? Gratuitous use of macros but you can cange the number of teeth, etc. quite easily. Thanks for your help guys :-)

%
O14001 (SPLINE CUT)

G90 G54 G40 G49
G103 P1
#100= 0 (START POSITION)
#101= 56 (No. OF TEETH)
#102= 360 / #101 (SETS TOOTH ANGLE)
#103= 25. (MINOR DIAMETER)
#104= 360

M06 T10 (BROACH TOOL)
M97 P1 L#101
G53 Z0.
M30

N1 M19 P#104
G90 G54
G68 X0. Y0. R#100
G00 X0. Y#103 (MINOR DIAMETER)
G43 H10 G00 Z1.
M97 P2 L8 (L=No OF CUTS)
#100= #100 + #102
#104= #104 - #102
M99

N2 G91
G00 Y0.2 (D.O.C.)
G01 Z-16. F1000. (CUT LENGTH)
G01 Y-0.1 (RETRACT)
G90 G00 Z1.
G91 Y0.1
M99
%

[omy005]

Here is my program I've used many times.

%
O01000 (SPLINE)
#100= 208 (tool start angle m19)
#101= 4.5 (orient inc angle)
#102= 360 / #101 (calculate number of steps)
#105= #100
G91 G28 Z0
G40 G49 G94 G69
G55
G90 G00 X0 Y0 A0 B0

#103= -18. (Y START) (INSIDE OR OUT SIDE SPLINE Y START POSITION )
M97 P10 L1 (NUM OF CUTS)
G91 G28 Z0.
G28 Y0.
M30

N10
T9 M06 G90
M97 P1 L#102
G69
#105= #100
#103= #103 + 0.2 (Y INCREMENT)
M01
M99

N1 G00 G90 Y#103 X0
M19 P#105
G43 H09 Z5.
G01 Z-12. F6000. (DEPTH OF CUT )
G91 Y-1.
G00 G90 Z5.
G91 G68 X0 Y0 R - #101
G90
#105= #105 + #101
M99
%


Andrew

[Jake@SRM]

Does anyone have any suggestions for tooling for this job (single point gear broadching)?
I ground a tool out of HSS Cobalt which lasted about 2 minutes in Aluminium Alloy before being totally destroyed.
Thanks

[omy005]

HSS should be fine in Aluminum. I use either HSS or a piece of tungsten carbide brazed onto a HSS shank. It sounds like you didn't have any chip clearance at the bottom the the slot if it is a blind hole and that is why the tool broke? Also ensure your coolant is flushing the chips away.

Andrew