broaching a keyway

The guys at www.Razorformtools.com have come out with a new insert and holder for broaching keyways in a CNC machine. We cut a lot of gears on our Integrex using an involute cutter. Some day in my lifetime maybe I'll be able to hobb with ours, but I'm losing hope... at any rate, we typically end up cutting the keyway for the pinion gears with a broach cutter manually. I'd like to automate the process and broach the keyway on our Integrex.

I've figured out how to get the toolpath I want pretty easilly in MazaCam by automatically creating a toolpath with the .001 depth of cut do depth than retract out of the bore and repeat and then use the toolpath as geometry. What I can't figure out is how to clamp the C axis so it won't rotate, AND clamp the spindle so I can use it as a fixed turret like any old lathe tool.

Can both spinbdles be stopped and clamped but still allow motion in a line center or bar in Mazatrol process, or is there a better way to do it in a manual process.

thanks,

Stu

Hey Stuart, have you ever got broaching to work yet? I'm looking at doing some on our 200IVS and looking for advice. Let me know.

You are better to build a eia macro for this...

I had to broach some sharp corners in a part a while back.

Here is the Manual Unit I used on the 640 MTPro control.

http://integrexmachinist.com/PicWeek/Integrexman/Brouch.gif

Here is a broaching program I made on the Vortex. It uses macros to increment each pass (37 in this case).

%
O0
G00 G20 G40 G49 G80 G90
G91 G00 G28 Z0.
T29
M06
G05 P0
M161
M19
#101=58.88
G00 G54 G17 G94 G90 X#101 Y-.23
G43.4 H#1034 Z2.0
G00 B-30.25
(====Slot1====)
#100=58.888
#101=58.88
#102=0
G00 Z.1
N1
#100=#100+.005
G00 X#100
G01 Z-2.249F60.
X#101
G00 Z.1
#102=#102+1
IF [#102 LT 37] GOTO1
(====Slot2====)
#100=58.888
#101=58.88
#102=0
G00 X#101 Y-.77
N2
#100=#100+.005
G00 X#100
G01 Z-2.249F60.
X#101
G00 Z.1
#102=#102+1
IF [#102 LT 37] GOTO2
(====Slot3====)
#100=47.143
#101=47.135
#102=0
G00 X#101 Y-.77
G00 Z-1.65
N3
#100=#100+.005
G00 X#100
G01 Z-2.749F60.
X#101
G00 Z-1.65
#102=#102+1
IF [#102 LT 37] GOTO3
(====Slot4====)
#100=47.143
#101=47.135
#102=0
G00 X#101 Y-.23
G00 Z-1.65
N4
#100=#100+.005
G00 X#100
G01 Z-2.749F60.
X#101
G00 Z-1.65
#102=#102+1
IF [#102 LT 37] GOTO4
(====Slot5====)
#100=13.607
#101=13.612
#102=0
G00 Z.1
G00 X#101 Y-.23 B30.25
G00 Z-1.65
N5
#100=#100-.005
G00 X#100
G01 Z-2.749F60.
X#101
G00 Z-1.65
#102=#102+1
IF [#102 LT 37] GOTO5
(====Slot6====)
#100=13.607
#101=13.612
#102=0
G00 X#101 Y-.77
G00 Z-1.65
N6
#100=#100-.005
G00 X#100
G01 Z-2.749F60.
X#101
G00 Z-1.65
#102=#102+1
IF [#102 LT 37] GOTO6
(====Slot7====)
#100=1.862
#101=1.867
#102=0
G00 Z.1
G00 X#101 Y-.77
N7
#100=#100-.005
G00 X#100
G01 Z-2.249F60.
X#101
G00 Z.1
#102=#102+1
IF [#102 LT 37] GOTO7
(====Slot8====)
#100=1.862
#101=1.867
#102=0
G00 Z.1
G00 X#101 Y-.23
N8
#100=#100-.005
G00 X#100
G01 Z-2.249F60.
X#101
G00 Z.1
#102=#102+1
IF [#102 LT 37] GOTO8
G00 Z2.0
G49
G91 G00 G28 Z0. M9
G28 Y0. A0. B0.
M30
%

Yeah I'll be writing the code in .eia. I've never broached anything before so I was just looking for any info out there.

Integrexman - Thanks for the info.

The only problem I see running into (like Stu was asking about) is how to Clamp the milling spindle and the C-Axis. Not sure if I describe the broach as a turning tool and use milling mode. Not sure if the control will let me do that. Guess it'll take some playing around with.

On our E series Integrex werun broaching in an ISO macro.We use Mazatrol tool data. The tool is described as an e-mill. If you measure (shadow graph) from C/L to the tip of tool and double it this would be the Ø of the tool. Length set in normal manor (tool eye ect).
This will get your tool tip to the correct programed position.

The spindle is orintated and clamped by M code in the macro and the chuck (C axis ) clamps when in correct position.
Our inserts are from ''pHorn'' they are expensive but last a long time

Stuart
I do some broaching on a plastic part. Works really slick. I have the "C" axis and the mill spindle clamped. I'll dig up the program on Monday. I could email it to you if you would like.
Steve

Love the macro idea.

I actually use MazaCam to create the toolpath for me. Mazcam allows you to call a tool and use say a .001" depth of cut to go from your start point to the desired depth. When it creates the toolpath, you then use that toolpath as geometry to drive the broach and everything is handled automatically.

Here's a little macro program I use on a few jobs.

I call this up from a Mazatrol prog.
Set your start position in X.
Define the number of passes.
In the O2001 sub it controls the X and Z depth of cuts.
I also run a similar program for broaching on the sub spindle.


<BROACH-FRONT>(BROACH-FRONT.EIA)
(BROACH FRONT OF PART)
G109L1
M901(HD1 SELECTION)
M200(C1-AXIS SELECTION)
G53.5(MAZATROL COORDINATE SYS SELECTION)
G98 M8
G00 C0.0
G17UH
G12.1
G122.1
G00 Z3.
G00 X3.5(APPROACH)
G00 X.62(START POSITION OF BROACH CUT)
G65 P2001 L134(NUMBER OF PASSES)
( 1PASS=.001 )
G00 Z1.
G13.1
G28 U0. M205 M9 M154
M99


O2001(BROACH-FRONT-SUB)
(BROACH FRONT OF PART)
G90 G01 Z0. F50.
G90 G01 U0.001 F100.(DEPTH OF CUT IN X)
G90 G01 Z-2.05(DEPTH OF CUT IN Z)
G00 Z0.1
M99

Rogue33

that's a pretty simple way to accomplish the task. Can youi give me an idea how you call this from a Mazatrol program, and go back to it?

Do you call up the broach tool in a manual process before calling this subprogram, and how do you define the tool.

Your approach is WAY simpler than the MazaCam method I've been using to accomplish the same task.

Curiously,

Stu

Rogue33

I don't seem to have any problems running in EIA, or Mazatrol as long as I stick to one format.

I'm trying to machine a shape (pulley actually) that is stupid simple in Mazatrol, except it's a bastard sized bore to fit a weird torque converter assembly. the shape is easy, and I can get your broaching program to work, but it seems the X and Z locations don't want to go where I want them. I'm guessing it's because I'm missing a step somewhere, or losing something between co-ordinate systems. The broach is trying to broach the keyway several inches into my spindle and up an inch or so higher than the bore is. Thankfully I'm trying this in the air 8" in front of the chuck.

I've set up the program in Mazatrol and defined the tool as a special. Both the origin and tool definitions are in Mazatrol co-ordinates. After I'm done with the pulley I call your Broach front program as an EIA sub that repeats once. It calls the 2001 sub program to make the individual passes.

Am I supposed to shift co-ordinate systems somewhere, or do I need to redefine the setup origin for the EIA programs? Does it use my original Mazatrol origin? Does X somehow get confused because of the radial command interpretation?

In your sub, can I add something like

G90 U-0.002 F100. (move in .002" before retracting)
G00 Z.1 (retract to clearance point for next pass)
G90 U0.002 (move out to original point)

So the tool won't scuff on the way out?

With a bit of luck I'll get this working and I won't need to make an arbor just to broach a single keyway. Besides, I'll learn soemthing in the process.

Many Thanks,

Stu

Rogue 33

you can use a manual prog. Special to call the tool,
then you can use a sub pro unit to input the variable data
and call the eia program. This is how i have do it every time
cut a key way.

Rogue 33

O/K I got this to work! Thanks Dude, it works sweet and is super simple. Simple enough I figured out a way to not only broach the keyway I needed and save the effort to build an oddball arbor, buit I was able to grind a custom tool and broach a neat square inside a part that slides freely yet doesn't rotate by indexing the broach and C axis. It takes a bit of time, but saved the cost of a custom broach and netted me a cool functioning prototype tool.

Many Thanks!!!!!!!!!!!!!!!

Stu

This is a program I use for broaching that works well for me. Just call it up as an EIA sub in Mazatrol. This one was setup for broaching a keyway that was blind until the part was cutoff. I had issues with chips compacting in the bottom so I just started deeper than normal and let it back up per pass.

Nick

O101(BROACHING)

G109L1
G28 U0 V0
G30 W0
G122.1 (RADIUS MODE)
M901 (HEAD 1)
M200 (MILL MODE)

T20 T25 M06
M253 (MILL SPINDLE CLAMP)

G00 B0 C90.
G53.5
M210 (C-AXIS CLAMP)
M08

#1=.0025 (X DEPTH OF CUT)
#2=2.23 (Z STARTING DEPTH)

G00 X.144+#1 Y0 Z.1 (START POINT \ X IS RADIUS MODE)
M98 Q1 L52 (Q=SEQUENCE LINE CALL \ L=REPEAT TIMES)
G00 Z.1
M09
G28 U0 V0
G30 W0
M99


(SUB PROGRAM)
N1
G01 G98 Z-#2 F300.
U-#1
G00 Z.1
U#1*2
#2=#2-.0019
M99

(******************************************)