Helial interpolation

[wevz]

I have to do move that is new to me. It is a helical interpolation. I'm not positive on how to do this.

Tool diameter: 4.0mm
Finished hole diameter:5.01mm
LOC: 19.0mm

I need to do a full circle arc and go down 19.0mm total. Any help would be appreciated. Thanks.

[dcoupar]

This is one way...

(NORMAL START UP STUFF - PROGRAM IN MM)
...
...
N40 G00 G54 G90 X0. Y0. S6000 M03 (POSITION TO CENTER)
N50G43 Z2.0 H01 (RAPID Z TO CLEAR)
(ENTER TOOL RADIUS IN D01)
N60 G01 G41 G91 X2.505 Z0 D01 F100.0 M08 (FEED TO START)
N70 M98 P102001 (CALL SUB 2001 10 TIMES)
N80 I-2.505 (ONCE AROUND AT BOTTOM)
N90 G01 G40 X-2.505 (CANCEL COMP)
N100 G00 G90 Z2.0 M05 (RETRACT Z TO CLEAR)
(ADDITIONAL HOLES)
N110 G91 G28 Y0 Z0 (Y AND Z TO HOME)
N120 G90 M30

O2001 (HELICAL SUB)
G03 I-2.505 Z-1.9 (ONCE AROUND AND DOWN)
M99

For additional holes, position X & Y, & copy N60 to N100 for each hole. If you do a lot of this, it might be worthwhile to write a macro, but that's another subject.

[wevz]

After reading your post i'm wondering if this is what i need? I am using a 4.0mm endmill w/.3 radius. I will be going in a predrilled hole and bore it out to a finished size of 5.008mm. I would like to make one continuous feed motion, circular and in z axis. After reaching bottom, i would like to go back to x0 y0 and rapid up. I have to do 16 of these holes in each part. Do you think i'm using the correct interpolation or should i try cylindrical, which i've never done either.

[dcoupar]

Helical Interpolation? Hmmm... that's exactly what I posted. Cylindrical interpolation wraps toolpath around a cylinder (engrave text on the OD of a shaft, for example).

Try the example I posted; if it doesn't do what you want, let me know.

Your original post said 5.01MM dia., this one is 5.008... you'll have to add to the value in D01 to adjust.

[billystein]

i have used this procedure for milling threads. I have found that it works good to go to the bottom of the helix and feed up. use cutter comp so you can adjust your finish size.

[wevz]

dcouper
I have a Daewoo DVC320 mill with fanuc oi 21 controls. In your post you stated to put the tool radius in D01. I have never seen a D code nor can I find any reference to one in the book. Am I overlooking something?

[dcoupar]

wevz,

G41 (and G42) offset the programmed tool path left (or right) of the path. To do so they need an offset value, which is stored in the control's offset memory. Most newer Fanuc's allow you to enter both a length offset and a diameter offset, but some don't.

Look at your offset display:

You may see OFFSET, SETING, and WORK. If you press OFFSET, you may see several columns:

NO. GEOM(H) WEAR(H) GEOM(D) WEAR(D)
001 10.000 0.000 0.000 0.000
002 –1.000 0.000 0.000 0.000
003 0.000 0.000 0.000 0.000
004 20.000 0.000 0.000 0.000
005 0.000 0.000 0.000 0.000
006 0.000 0.000 0.000 0.000
007 0.000 0.000 0.000 0.000
008 0.000 0.000 0.000 0.000

For the example I gave earlier, your tool length offset goes in GEOM(H) #01, enter the radius of your cutter in GEOM(D) #001

Hope this helps.

Dave

[wevz]

dcouper
Now it's starting to click in my head. We've never used the diameter geometry on the controller. Makes much more sence now. Thanks!