Appealing to All Professional CNC Programmers

[Chelo]

I am in desperate need for a CNC program for broaching on a VF4 Vertical Milling Machine.  Can someone please help me.

[crazy^millman]

Point toolpath will be a quick and dirty way to get it done. Can be done with 3D contour if you draw the lines. Can use Transform to step over the broaching amount once the seed operation is done.

 

Pretty straight forward to broach on a CNC Mill. Don't forget to M19 your Spindle before starting. Not S0, but M19 to orient the Spindle.

 

HTH(Hope that Helps)

 

Welcome to the forum.

[Chelo]

I feel there is gotta be a better way ( no pun Intended)...

I found this on the almighty internet but it doesn't work, I am sure is a good start ...

 

N9 G20
N11 G00 G17 G90 G54 X0. Y0.
N13 T7 M6
N15 M19
N17 G43 H7 Z1.
N19 M8
N21 Z.1
N23 G1 Z-1. F10.
N25 G19 G02 Y-.1 J-.002 K0.
N27 G00 Z3.
N29 G91 G28 Z0. M9
N31 G28 Y0.
N33 M30

 

Thanks

[crazy^millman]

Better way in how. Pretty simple thing to broach. You need a Position move to put the broach where you want it. Cannot cut all the material in one pass with broaching. You need to step it over and a lot of factors come into play here. Material you are cutting, the material you are using for the broach, the type of shape you are cutting, is it a blind or is it a thru, and etc.....

 

I deal with a lot of people who keep trying to reinvent the wheel. Guess what the wheel is still the best thing to move something from point A to point B. What they are still used on cars.

[Chelo]

Thanks Ron for your comment .

 

I am looking for some codes that would point me in the right direction.

My keyway is pretty straight forward and right thru a 2" plate

 

 

I get the concept  and I know what needs to be  done I just don't know how.

I was hoping somebody would have a template of a working program that I can modify.

 

Thanks

[The Cathedral]

I do broaching by drawing a line for the toolpath with a line for retract off the bottom. Then I chain it and do multi-passes. Works every time. Easy as pie. A whopping two pieces of geometry.

[Del.]

Wire edm in 15 minutes.

[Chelo]

Hey Trogdor, the Burninator, thanks.

I think you are up to something...(Trolls aside)... Care to share some code lines?.

it would be greatly appreciated.

 

[crazy^millman]

N9 G20
N11 G00 G17 G90 G54 X0. Y.74
N13 T7 M6
N15 M19
N17 G43 H7 Z1.
N19 M8
N21 Z.1
N23 G1 Z-1. F10.
N25 G0 Y.64
Z.1
Y.745
G1Z-1.
G0Y.64
Z.1
Y.750
G1Z-1.
G0Y.64
Z.1
Y.755
G1Z-1.
G0Y.64
Z.1
Y.760
G1Z-1.
G0Y.64
Z.1
Y.765
G1Z-1.
G0Y.64
Z.1
Y.770
G0Y.64
Z.1
G91 G28 Z0. M9
G28 Y0.
M30

That is taking what you put up and less than 5 minutes worth of editing to get you out to .770. Machinist Handbook has the correct place you need to be for clearance. I was writing this by hand back in the late 80's. You need to take some basic programming classes.

 

Use at your own risk. 5th Axis Consulting takes no responsibility for errors or problems from this example.

[The Cathedral]

Ron's example is good; I usually write mine as macros or using WHILE/DO

 

 

N22 (BROACH)
G0 G40 G90 G57 X-.187 Y0 M19
G43 H22 Z.1 M8 T23
M84
#100=0
WHILE [#100LT115] DO1
G91 G1 Z-2.36 F200.
G0 X.3
Z2.36
X-.302
#100=#100+1
END1
G90 G0 Z1.
M9
G0 G91 G28 Z0
G30 Y0
M6

 

[htm01]

here you go

[Mic6]

I never broached on a Haas, but I've read elsewhere that with spindle off it's a lot of force on the ceramic bearings or something.  Somebody want to clarify?

[Rstewart]

I never broached on a Haas, but I've read elsewhere that with spindle off it's a lot of force on the ceramic bearings or something.  Somebody want to clarify?

 

 

Yeah, If you turn your VMC into a broaching machine the spindle is gonna be shot soon...  Once every now and then in aluminum or soft steel ain't no problem.

 

To answer your question, spindle bearings are meant to be used while in motion.  You can put flat spots on the balls, or dent the races.

 

Haas Doesn't use ceramic

[Chelo]

Thank you Guys for the code and the tips. Now off to the machine for testing

 

[Brad St.]

Rstewart, the VFOE I ran in the early 2000's had ceramic bearings. it was the neatest thing to see the static charge build and jump from the cutter to the graphite trodes because the head wasn't grounded as well due to the ceramic bearings.

 

Opps, I should say the cutting tool to the head wasn't grounded.

[crazy^millman]

Ron's example is good; I usually write mine as macros or using WHILE/DO

 

I was trying to keep it basic and not get into Macros, but good way to go about it as well.

[Guest]

The macros are especially nice with NCplot because you can convert them to long hand G-Code for use on controls without macro capability.

[Redfire427]

^{M19 is important, however, equally important is how the tool is positioned in the spindle. You need to know the correct position of the tool so you can program the proper vector for machining.}

 

^Carmen

[Newbeeee™]

Thanks Ron for your comment .

 

I am looking for some codes that would point me in the right direction.

My keyway is pretty straight forward and right thru a 2" plate

 

keyway.PNG

 

I get the concept  and I know what needs to be  done I just don't know how.

I was hoping somebody would have a template of a working program that I can modify.

 

Thanks

What I would say is don't do it.

Yes you can drill first to get most of the mtl out, but 2" plate!!!

That is a heck of a length of mtl to push through. 

We've done it on small flanges and it works well, but 2" is a lot of force loaded right on your bearings, even at a couple of thou stepover/cut.