4th axis drill and tap macro

[Born to machine]

Hi All,

Not sure if this is possible but i do alot of drilling and tapping on a 4th axis..

Instead of typing in my A values(rotation ) manually is there a way to just tell program to repeat drill at a certain A value and number of holes?

Kinda like a canned cycle but for rotation..

Thanks

 

[Colin Gilchrist]

6 minutes ago, Born to machine said:

Hi All,

Not sure if this is possible but i do alot of drilling and tapping on a 4th axis..

Instead of typing in my A values(rotation ) manually is there a way to just tell program to repeat drill at a certain A value and number of holes?

Kinda like a canned cycle but for rotation..

Thanks

 

Yes, by using an option called "Axis Substitution", you can do this.

If your points are "around the diameter", then you use the "unroll" option.

Enter the Rotary Diameter, and make sure you use the Top of the hole.

In the "Depths" page, use "Incremental" for all the depth options.

Axis Substitution will unwind the hole positions, and output the rotary axis value.

[jeff]

Why not just use the Transform/Rotate option?

[Jayson Kramer]

1 hour ago, jeff said:

Why not just use the Transform/Rotate option?

Jeff in most case more work then axis sub . now if all the holes are a lined in a row around the dia then Transform works great.

[Bill Craven]

If you have a solid model of the part and have the Mastercam multi-axis module, you could do it as a 5 axis drill path.  This works especially well if the holes aren't evenly spaced.

[Jayson Kramer]

Axis Sub-2019.zipHere is a file sample of some of these options. use the veiwsheets for different configurations.

[navsENG]

It almost seems like he wants to figure out how to do this outside of Mastercam? You could make  a very simple while/DO statement and just make it repeat the same code for the inital , how ever many times you want... Obviously this would only work if it is an equally spaced radial pattern. 

If not it would just require a little more code, still doable

[Born to machine]

Correct,

I actually do want to do this outside of mastercam..

Im not confident in writing these sort of programs but if anone has an example to share it would be a great starting point..

Thanks

 

[Colin Gilchrist]

You could do something like this, using Macro B:

 

 

#100=24. (Number of Holes)

#101=0. (Abs. Starting position, relative to G54)

#102=360./#100 (Get incremental A rotation Value)

#103=1. (hole counter)

#104=2. (Z DEPTH OF HOLE BOTTOM)

#105=2.6 (Z DEPTH OF HOLE START, .100 ABOVE STOCK)

#106=.05 (PECK AMOUNT)

#107=3.8  (FEED RATE)

#108=.1 (SAFE Z ABOVE R PLANE)

#109=3. (Z JUMP HEIGHT)

T01 M06

G00 G90 G54 X0. Y0.

G43 H01 Z#109

G00 G90 A#101 (MOVE TO START)

WHILE [#103 LE #100] DO1

G00 G90 Z[#105+#108] (R PLUS SAFE)

N1 G83 Z#104 R#105 Q#106 F#107

G80

G00 G90 Z#109

G00 G91 A#102 (MOVE A INCREMENT VALUE)

#103=#103+1 (INCREMENT COUNTER)

END1

[Colin Gilchrist]

Technically, the "N1" should be up one line, on the line that says (R PLUS SAFE).

[jlw™]

Can you post a picture of the rotary table on the machine?