2D Ramping Quirk

[Mic6]

So I was milling a 6.000 circle out of a 1" plate. I bolted the slug down, the ramp began at 0 deg. Went around 720 deg to depth. Now regardless if I have "additional pass at final depth" checked or not, when the tool came to 0 deg. at final depth it made a slight G03 move to a point @ about 300 deg on the prev. toolpath and continued on to 0 deg and retracted. It doesnt show in verify, but the extra move pops up when posted. Any ideas?

[88Matt]

run backplopt with show rapids turned on and see what it shows.

[88Matt]

run backplopt with show rapids turned on and see what it shows.

[Mic6]

So I'm still having prblems with contour ramping cutting an arc thru my part and then retracting. My explanantion in my previous post was kinda messy. When the tool reaches depth, it mills around to about 45deg to cleanout the entire ramp, then does a G03 move thru my part back to zero, and then retracts. It will do it regardless if "Make a pass at final depth" is checked or not. FTP doesnt seem to be working. I'llpost the file as soon as it's working.

[Mic6]

Here's the part.

Mastercam_forum/MCX2_Files/2.375 SIDE HOLES.MCX

[Guest]

You're problem is related to using Wear comp and no lead in/lead out

 

Change it to computer and it works perfectly.

 

If you NEED wear add small lead in/lead out moves

 

The ONLY difference between the 2 paths is wear and computer

 

 

[Tony35]

I just backplotted your file in x3 and cant see any problems when it gets to 45 deg at final pass it retracts. Am i missing something?

[Mic6]

O1111( 2 )

( T2 | 3/8 VARIMILL | H2 )

G20

G0 G17 G40 G49 G80 G90

( MILL 2.375 HOLE THRU 8X )

T2 M6 ( 3/8 VARIMILL | T: 2 | D: 2 | H: 2 | DIA: .375 )

G0 G90 G54 X.9617 Y-.1738 C0. S2850 M3

G43 H2 Z.25

/M8

Z-1.25

G1 X.9877 Y-.026 F18.5

G3 X.99 Y0. R.15

Z-1.31 I-.99 J0.

Z-1.37 I-.99 J0.

Z-1.43 I-.99 J0.

Z-1.49 I-.99 J0.

X.495 Y.8574 Z-1.5 I-.99 J0.

 

X.99 Y0. R.99 <-------This is the move cutting back thru my part

 

X.495 Y.8574 R.99

X.4713 Y.8684 R.15

G1 X.3303 Y.9197

G0 Z.25

M5

G91 G28 Z0. M9

G0 G90 G154 P99 X0. Y0.

T2 M6

M30

%

 

 

I tried using computer comp as suggested. I also added small lead-in/out moves. As well as added moves to Wear. This problem isnt visible in backplot or verify. Only when it posts.

[Guest]

Then you have a post issue.

 

The screen shots above are verfied gcode from a generic HAAS post

[Mic6]

It verifies and backplots perfectly for me as well. I've been manually deleting the extra move. What would I even be looking for in the post? Thanks Again

[Guest]

The backplot I used is the actual posted gcode. It is outside of Mastsrecam.

 

Mastercam does NOT show the move.

 

What to look for.

 

I can not say off the top. Have you made any modifications to your post?

 

You should turn on debugging and see what section of the post is outputting that line. That should give you a starting point for troubleshooting.

[gcode]

You have both I's J's and R's in those arc statements..

Go to your Arc page in the Control Def and

make sure you have all three planes

set to Delta Start to Center..

 

It looks like you've got at least one of them set to output R's (which are bad news)

[Mic6]

I'll check that first thing on Monday

[Thad]

gcode teh eagle eye.

 

Thad

[Mic6]

code:

---

%

O1111( 2 )

( T2 | 3/8 VARIMILL | H2 | D2 | DIA: .375 )

G20

G0 G17 G40 G49 G80 G90

( MILL 2.375 HOLE THRU 8X )

T2 M6 ( 3/8 VARIMILL | T: 2 | D: 2 | H: 2 | DIA: .375 )

G0 G90 G54 X.99 Y0. C0. S2850 M3

G43 H2 Z.25

/M8

Z-1.25

G3 G41 D2 Z-1.31 I-.99 J0. F18.5

Z-1.37 I-.99 J0.

Z-1.43 I-.99 J0.

Z-1.49 I-.99 J0.

X.495 Y.8574 Z-1.5 I-.99 J0.

X.99 Y0. I-.495 J-.8574

G40 X.495 Y.8574 I-.99 J0.

G0 Z.25

M5

G91 G28 Z0. M9

G0 G90 G154 P99 X0. Y0.

T2 M6

M30

%

---

Thanks, that did it.

[gcode]

Mic6,

Make sure you do the fix from

Settings/Machine Defintion..

that permanently changes you machine/control def..

 

If you make the fix from the Edit button in the OPS Manager.. you are only changing the local copy for that MCX file.... and you'll have the same problem on your next project..

 

also...

 

will your machine accept a G40 in an arc statment.

most won't

[Mic6]

Yup, changed the CD/MD

 

It's a Haas. I just ran it, and it liked it. Suprised me too. Thanks

[gcode]

quote:

---

It's a Haas. I just ran it, and it liked it. Suprised me too.

---

Do you have a value in the D register or did you run D = 0.

 

If you ran D=0 try running D=-.03 and D= .03

UP IN THE AIR... Turning Cutter comp off

and on with arcs is dangerous business.

[Mic6]

Yea, it was D0. Maybe I celebrated to early huh? All kinds of red lights on that G03. Did'nt even get to G40. Bummer. What's next?

[htm01]

you need a straight line lead-in/lead-out

[Mic6]

Here's the code WITH Lead-in/Lead-Out. I stayed tangent with a 5deg. sweep. I want to preserve as much of the slug as I can.

 

code:

---

%

O1111( 2 )

( T2 | 3/8 VARIMILL | H2 | D2 | DIA: .375 )

G20

G0 G17 G40 G49 G80 G90

( MILL 2.375 HOLE THRU 8X )

T2 M6 ( 3/8 VARIMILL | T: 2 | D: 2 | H: 2 | DIA: .375 )

G0 G90 G54 X.9764 Y-.1625 C0. S2850 M3

G43 H2 Z.25

/M8

Z-1.25

G1 G41 D2 X.9894 Y-.0131 F18.5

G3 X.99 Y0. I-.1494 J.0131

Z-1.31 I-.99 J0.

Z-1.37 I-.99 J0.

Z-1.43 I-.99 J0.

Z-1.49 I-.99 J0.

X.495 Y.8574 Z-1.5 I-.99 J0.

X.99 Y0. I-.495 J-.8574

X.495 Y.8574 I-.99 J0.

X.4834 Y.8634 I-.075 J-.1299

G1 G40 X.3474 Y.9268

G0 Z.25

M5

G91 G28 Z0. M9

G0 G90 G154 P99 X0. Y0.

T2 M6

M30

%

---

It ran fine with D.025