contour formula

[JSomerville]

Good morning everyone. I had to go back to programming and I can't remember the formula to cut a pocket so the tool drops on center. It was something about the diameter of the tool and the lead in angle was 135 degrees. When I used this it dropped on center and cut returned to center and retracted. It's been a while so be kind. Thank you in advance....

[mayday]

just add a point in the chain geometry, tool will start at point

[JSomerville]

I understand that. This formula always dropped on the center piont and returned it was so simple. Made it nice when there was very little room for error.

[gcode]

Try

(width of pocket - Ø of tool)/4

I use that to define a 180° lead in/out that starts in the C/L of a slot

[jeff]

Is this what you are looking for?

 

[(Hole Diameter - Tool Diameter) / 2 ] X .4142

[JSomerville]

Yes I think that is it. Put that value in the length and the radius and use 135 for the sweep and it works every time. As long as the tool will go in the hole the tool will start at the center piont and return to the center piont after contouring the hole....

 

Thanks Jeff!!!!!!

[Dan@home]

Maydays suggestion sounded easier.

[jeff]

quote:

---

Maydays suggestion sounded easier.

---

For pockets yes, but not for interpolating a hole and having your endmill start and end at center.

[JSomerville]

exactly. This is a specific operation for bushing pockets, cavity insert pockets, guide pins ect.

 

It works great....

[shazam/TPP]

why not use circle mill? start at center

[Dave.L]

quote:

---

quote:

--------------------------------------------------------------------------------

Maydays suggestion sounded easier.

--------------------------------------------------------------------------------

 

For pockets yes, but not for interpolating a hole and having your endmill start and end at center.

---

 

I do exactly as Mayday says for holes and it works fine. I do check "use entry point" in lead in/lead out.

[Tyler Robertson]

quote:

---

why not use circle mill? start at center

---

+1

[Dave.L]

quote:

---

quote:

--------------------------------------------------------------------------------

why not use circle mill? start at center

--------------------------------------------------------------------------------

 

+1

---

Well, I have one reason, there is a bug with circle mill and it's been logged.

 

If you drill a hole then want to circle mill but rapid to the bottom, it won't, it will feed down.

 

There is a work around but CNC software has confirmed this is a bug.

[gcode]

quote:

---

If you drill a hole then want to circle mill but rapid to the bottom, it won't, it will feed down.

---

chain a circle at the bottom of the hole..

set incremental feed plane = 0

[Dave.L]

G, I will try that, but I think I found this issue when using 2D geo, so, no circle at bottom of hole.

[Dave.L]

Tom,

 

I just created a 2d circle. Entered feedplane = 0 incremental. set depth to -2.0

 

It does not work, it feeds down from Z0 to -2

 

(T | CIRMILL TEST.EIA | MAZAK_410A_640M | 02-23-10)

G20

G0 G17 G40 G49 G80 G90

G91 G28 Z0.

G90

N1

( 1/2" ENDMILL AMTPID 102919 | KENNAMETAL UCDE500J5BS KC643M | | TOOL 2 | DIA. OFF. 2 | LEN. 2 )

T2 T0 M6

G0 G90 G53 X0. Y0. S4500 M3

G43 H2 Z0. M8 T2

G1 Z-2. F10.

G41 D2 X.3394 Y.3394 F30.

G3 X0. Y.6788 I-.3394 J0.

I0. J-.6788

X-.3394 Y.3394 I0. J-.3394

G1 G40 X0. Y0.

G0 Z0.

G91 G28 Z0.

M01

N2

G91 G28 Z0.

T2 T0 M6

G0 G90 G53 X[#198] Y[#199]

M30

[gcode]

quote:

---

I just created a 2d circle.

---

draw the circle at z-2.

set Depth and top of stock and feed plane

to incrmental 0 .. leave retract off

set clearance to a safe absolute value.

[Dave.L]

Tom, same results: I will email my test file to you.

 

(T | CIRMILL TEST.EIA | MAZAK_410A_640M | 02-23-10)

G20

G0 G17 G40 G49 G80 G90

G91 G28 Z0.

G90

N1

( 1/2" ENDMILL AMTPID 102919 | KENNAMETAL UCDE500J5BS KC643M | | TOOL 2 | DIA. OFF. 2 | LEN. 2 )

T2 T0 M6

G0 G90 G53 X0. Y0. S4500 M3

G43 H2 Z.1 M8 T2

Z0.

G1 Z-2. F10.

G41 D2 X.3302 Y.3302 F30.

G3 X0. Y.6603 I-.3302 J0.

I0. J-.6603

X-.3302 Y.3302 I0. J-.3301

G1 G40 X0. Y0.

G0 Z.1

G91 G28 Z0.

M01

N2

G91 G28 Z0.

T2 T0 M6

G0 G90 G53 X[#198] Y[#199]

M30

[jeff]

quote:

---

why not use circle mill? start at center

---

Because the genius that I am, have a heavily edited Okuma Mill post and somewhere along the line I did something that messed up the circle mill with wear and multiple passes.

 

So, for my Okuma, I have to use contour for holes instead of circle mill if I want to use wear and multiple passes.

Otherwise it won't turn off comp

It's only for circle mill toolpath.

[Dave.L]

quote:

---

draw the circle at z-2.

set Depth and top of stock and feed plane

to incrmental 0 .. leave retract off

set clearance to a safe absolute value.

---

Tom got this to work, it looks like the trick is to ALSO set retract = 0 incremental.

 

PS, still a bug though.

[Mike S @ S4A]

[Rob @ Target Machine]

[shazam/TPP]

Dave,

if you don't want to draw extra geometry, why not just give it a high feedrate for plunge, that way all your retracts will remain in tact.

hth

[Dave.L]

quote:

---

Dave,

if you don't want to draw extra geometry, why not just give it a high feedrate for plunge, that way all your retracts will remain in tact.

---

I found this bug a while ago. Now I only use 3D geo.

 

However, still a bug and I am most concerned about setting parameters to make it work and then some day the bug maybe fixed and the parameters will act different and may be overlooked.

 

But, I doubt the bug will be fixed anytime soon.

[Cad-Camr]

I love the controls that have G13 capability. But I use the formula mentioned above with 135 Deg sweep all the time. Its awsome. 2c