Looking to write a canned cycle for VMC broaching

[MBX5]

I have a Fadal 4020VMC CNC88HS - 1995 vintage... I am using HSMWorks in Solidworks for my CAM.

Looking to accomplish this:
http://www.youtube.com/watch?v=iO81YZsUc_4]Broaching a keyway Haas VF-7 - YouTube

Using one of these tools in a collet holder:
Broach Tool Specifications for Razorform Tools

Obviously there isn't a canned cycle for this in the s/w....so could anyone help me with coding this? I am really kind of green with G-code, but probably could accomplish this with some guidance.

Thanks!!

[txcncman]

Why do you need a canned cycle?

[MBX5]

Not sure I do.

Really just need to accomplish what's in the video.

Thanks.

[dcoupar]

It looks like it could be done with a G81 cycle and repeat - not sure how to do this on a Fadal, but here's one idea for a Fanuc.

G00 X0 Y0 M19 (POSITION TO CENTER & ORIENT SPINDLE)
G43 Z0.5 H01
G81 G91 X-0.01 Z-1.5 F50. K20 (20 PASSES @ 0.01 PER PASS)
G00 G28 Z0

[txcncman]

Unless you have a lot of part sizes to handle, a G91 loop/subprogram will probably be easiest.

Repeat number of times needed for final X.

G91 X(Stepover)
Z-(Depth)
Z+(Depth)
M99

[underthetire]

Not sure on your machine, but you do show a hs spec. Make sure it does not have ceramic spindle bearings, and go light on the cuts. Spindle bearings really hate shock load on them when they aren't rotating,

[angelw]

It looks like it could be done with a G81 cycle and repeat - not sure how to do this on a Fadal, but here's one idea for a Fanuc.

G00 X0 Y0 M19 (POSITION TO CENTER & ORIENT SPINDLE)
G43 Z0.5 H01
G81 G91 X-0.01 Z-1.5 F50. K20 (20 PASSES @ 0.01 PER PASS)
G00 G28 Z0

Dave's solution would be clean. The code for the Fadal control is as follows:
G81 Z-1.5 F50
G91 X-0.01 L20 (20 PASSES @ 0.01 PER PASS)
G80

An R argument can be used in the G81 cycle to set an R Plane from which feed will commence. In G90 mode the R value is relative to the Workpiece Z Zero, in G91 mode the R value is relative to the Initial Z Plane. The Initial Level is the last Z level before executing the canned cycle.

Absolute and Incremental can be mixed in the cycle. For example the Z move can be in absolute and the X move in Incremental.

Regards,

Bill

[MBX5]

Thanks for the help - I am going to try it out this week!!

Thanks again!

[tfisher]

Carefull on your depth of cut. I do this on a horizontal boring bar quite a bit and only take .002" each stroke, it can be very hard on the thrust bearing on the back of the spindle. Also it's a good idea to have the machine move away from the cut on the return stroke rather than drag it across the part, otherwise it can chip out the face of your tool pretty easily.

[sinha_nsit]

If I recall correctly:
In incremental mode, X, Y, Z and R, all are incremental values. However, R is measured relative to the Z level of the tool just before calling the canned cycle, whereas Z is measured from the R level defined in the cycle.

Simplest way is to make the first hole in the absolute mode and the remaining holes (two in this example) in the incremental mode:
G90 G73 G99 X50 Y25 Z-25 Q3 R2 F50
G91 X20 K2
Note that, in the incremental mode as well as in the absolute mode, if a particular word is not specified, its value remains unchanged (Y, Z and R, in this case).

[FuddMcDee]

what about using a WHILE command in there? turn it into a somewhat universal program?
WHILE[#500LT10.]DO1

[sinha_nsit]

what about using a WHILE command in there? turn it into a somewhat universal program?
WHILE[#500LT10.]DO1

That is right.
In fact, nested WHILE can be used for xy array of holes.
See the attachment for more details.