Broaching on Caxis lathe

[JPensack Acker Drill]

I'm hoping to broach out 4 .501-.502 keys 90 deg. apart. They are .254 deep and 1.375 long. They have a radius groove for relief but then there is a shoulder behind it. The bore is around 4 11/16. Does anyone know of any good tooling for this job? Also is this feasible. We have a keyseater but with it not being a through key it will be tuff, also there are bolt circles but they can't be put in untill its keyed. So if I key it on the lathe then I can put the holes in.

[J Coulston]

PH Horn

 

They have a video of running.

 

HTH

[ATG]

I use Ph horn all the time. And i program the parts in mastercam....

[Philcott]

Nice looking tool.

 

I have made my own tools using grooving inserts in the past that have worked well for us.

 

Broaching up to a shoulder can give you troubles with the chips. I suggest a small depth of cut so the chip is not too big.

 

I programmed it using the canned groove cycle G74.

[chris m]

That is a nice looking tool; I will keep that in mind for the future. I like the video; having 1/2 the part missing certainly helps chip evacuation

 

I'd suggest leaving .005 or so on the shoulder and finishing it after broaching in case the broaching chips ding the face up a little.

 

C

[JPensack Acker Drill]

Thanks for the replies. I found some cutters but I'm still looking into finding one for the .501-.502 width. Now in MC what is the best way to program it? I could just use manual entry because my post isn't set up for any canned cycles. What is the best way to attack this?

[Ron Branch @ Verisurf]

Use a finish lathe cycle. Define the tool with a Zero radius and no RPM. Then use the multipass and it will make the code for you with no problem. Might do .002 to .004 steps and use cutting oil not coolant it will be easy.

 

HTH

[JerryBenoit]

Ron,

 

You might also want to mention that the feed should be set in in/min. the lathe will not feed unless the machine spindle is on in in/rev.

[JPensack Acker Drill]

I need there to be 4 keyways 90 degrees apart. I got the lathe finish pass to look good, but I can't get it to do more than one keyway. I'm thinking about using a caxis toolpath such as face contour. Any ideas?

[ATG]

Thats what I use. C Axis Cross Contour. Just use negative values to get the right cutter motion and rapid direction.

[Greg Williams]

I would use a simple macro, something like

 

OBRCH

IDIA=25 (MINOR DIAMETER)

ODIA=32 (MAJOR DIAMETER)

LEGH=-15 (Z FINAL LENGHT)

INC=0.1 (INCREMENTAL VALUE FOR BROACHING SHIFT)

CANG=0 (C-AXIS ANGLE)

 

 

T0101

M110

G0 C=CANG

M147

V1=INC

NLOOP X=IDIA+V1 Z3

G94 G1 Z=LEGH F250

IF [V1 EQ [ODIA-IDIA][NEND

X=IDIA

G0 Z3

V1=V1+INC

GOTO NLOOP

NEND X=IDIA

G0 Z3

X500 Z500

M146

M109

RTS

[Bruce Caulley]

I also have a macro for this. Leave it saved in the control and call the parameters in your "main" programme. Can have a few different programmes calling it then to do different keyways.

 

Bruce