Live tool, Lathe Help

[alloutmx]

Cutting splines on a Mazak, with C axis and live tooling

In Mastercam it looks Okay, but it doesnt seem to be posting out correctly.

Do I have machine def. incorrect or is it my planes or.....?

 

Thank you for your help. Im a mill guy, but that isnt stopping the owner from sh!ting on me today, because I cant figure this out fast enough.

HT6185-4 375-LEVER-REVC.MCX-7

[crazy^millman]

Well the way you have that defined it will cut along the Z axis of the machine. Do you want it to cut along the Diameter? IF so turn the spline 90 degree so it parrelle to the face. Turn 90 again so the back plane will be about center and should be good to go., If it is like you want then change the machine to the correct machine definition. You have default lathe. I would try Lathe C-Axis Slant Bed and see if that helps. Have you reached out to your dealer?

[alloutmx]

I do want to cut along the Z axis...pretty much exactly how the part is sitting on the screen from top view.

I changed to C-axis slant bed but no better result. It verifies just fine but wont post out correctly

[crazy^millman]

When you say will not post out correctly. Can you post up the code?

 

Here is what I got and it looks right to me.

 

%
O0000
(PROGRAM NAME - HT6185-4 375-LEVER-REVC)
(DATE=DD-MM-YY - 11-12-13 TIME=HH:MM - 08:45)
(MCX FILE - C:\USERS\RON\DOCUMENTS\MY MCAMX7\MCX\HT6185-4 375-LEVER-REVC.MCX-7)
(NC FILE - C:\USERS\RON\DOCUMENTS\MY MCAMX7\LATHE\NC\HT6185-4 375-LEVER-REVC.NC)
(MATERIAL - STEEL INCH - 1030 - 200 BHN)
G20
(TOOL - 1 OFFSET - 1)
(0.067 CHAMFER MILL)
G0 T0101
M23
G0 G54 X1.0432 Z-.272
C0.
G97 S1000 M51
X.9432
G98 G1 X.5432 F25.
X.5499 Z-.2432 F5.
X.5521 Z-.2142
X.5499 Z-.1853
X.5433 Z-.1565
X.5322 Z-.128
X.9432 F50.
G0 X1.0432
Z-.272
X.9432
G1 X.5432 F25.
X.5499 Z-.2432 F5.
X.5521 Z-.2142
X.5499 Z-.1853
X.5433 Z-.1565
X.5322 Z-.128
X.9432 F50.
G0 X1.0432
Z-.272
X.9432
G1 X.5432 F25.
X.5499 Z-.2432 F5.
X.5521 Z-.2142
X.5499 Z-.1853
X.5433 Z-.1565
X.5322 Z-.128
X.9432 F50.
G0 X1.0432
G28 U0. W0. H0. M55
T0100
M30
%

[alloutmx]

%

O0000

(PROGRAM NAME - HT6185-4 375-LEVER-REVC)

(DATE=DD-MM-YY - 11-12-13 TIME=HH:MM - 11:57)

(MCX FILE - C:\USERS\ACCURA\DESKTOP\TRIAL.MCX-7)

(NC FILE - C:\USERS\ACCURA\DOCUMENTS\MY MCAMX7\LATHE\NC\HT6185-4 375-LEVER-REVC.NC)

(MATERIAL - STEEL INCH - 1030 - 200 BHN)

G20

(TOOL - 1 OFFSET - 0)

(0.067 CHAMFER MILL)

G0 T0100

M23

G0 G54 X20. Z-10.

C90.

G97 S2500 M52

G98 G1 F2.

G28 U0. W0. H0. M55

T0100

M30

%

 

Im attaching the file again because I have changed it so many times... When i say sPlines, I am refering to the Part feature. They are actually suPPose to be arcs...thats why I drew arcs on a sePerate level. They came in as sPlines.

TRIAL.MCX-7

[crazy^millman]

Okay I see the problem know. You need a TOP WCS and Back T-Plane if they are both the same it will not post correctly. Also go into the Line Arc/Filter settings and make sure the create arcs in the G17/G18/G19 is checked and should be good.

[crazy^millman]

I can take the same geometry and do it in X6 and get the following output. Bring that file in X7 and it works, but doing in starting in X7 I get no G3 output. Weird one I am going to submit to qc.

 

%
O0000
(PROGRAM NAME - RON)
(DATE=DD-MM-YY - 11-12-13 TIME=HH:MM - 09:25)
(MCX FILE - RON)
(NC FILE - C:\USERS\RON\DOCUMENTS\MY MCAMX6\LATHE\NC\RON.NC)
(MATERIAL - STEEL INCH - 1030 - 200 BHN)
G20
(TOOL - 8 OFFSET - 8)
(1/4 CHAMFER MILL)
G0 T0808
G19
M23
G0 G54 X.5222 Z.3499
C0.
G97 S2500 M51
G18 G98 G3 Z-.3499 I-.2611 K-.3499 F40.
G1 X.7222
G28 U0. V0. W0. H0. M55
T0800
M30
%

[alloutmx]

okay...Planes are straightened out...but still Posting as if its a sPline... any ideas?

 

G0 G54 X.5432 Z-.277

C0.

G97 S2500 M51

G98 G1 X.5499 Z-.2482 F2.

X.5521 Z-.2192

X.5499 Z-.1903

X.5433 Z-.1615

X.5322 Z-.133

X.9432 F50.

G28 U0. W0. H0. M55

T0100

M30

[alloutmx]

ahhh...just read your last Post

Thanks for your helP

[crazy^millman]

I think you will need to go back to X6. I think it might be a bug and I have asked for assistance. Please contact your reseller if OptiPro is them and let them pass it up the ladder.

[alloutmx]

Yeah, i asked my boss to go back to x6 a while back....his cheaP comPuter with the broken P button, has a rough time running 7. He wont listen to me though.....he knows everything. Ohh well...I wont be here much longer

Thanks again

[Colin Gilchrist]

Hey guys,

 

I'm not seeing a bug here. If the center of the arc is at XY zero (from the Top T/C Plane), you get an Arc in the posted code. If the center of the arc is not at Y Zero, then it breaks the arc into pieces. This is the same in X6 and in X7.

 

I took your sample arc, and moved the center to Y 0.0. Here is the code from the Generic Fanuc 4X MT_Lathe Post:

 

(NC FILE - C:\USERS\CMG\DOCUMENTS\MY MCAMX7\LATHE\NC\HT6185-4 375-LEVER-REVC.NC)
(MATERIAL - STEEL INCH - 1030 - 200 BHN)
G20
(TOOL - 1 OFFSET - 0)
(0.067 CHAMFER MILL)
G0 T0100
M23
G0 G54 X.7482 Z-.277
C0.
G97 S2500 M51
G98 G2 X.7372 Z-.133 I-.3741 K.0579 F2.
G1 X1.1482 F50.
G28 U0. W0. H0. M55
T0100
M30
%

[Colin Gilchrist]

The logic that causes MP to break the Arc is in 'pcir0$', and is identical from X6 to X7. The only difference between the test files you've been using in X6 and X7 have been if the center of the arc is on the centerline of the part, or not.

 

When the center of the arc is on the center of part in XZ, then you get arc output. If the center of the arc is not on the centerline of the part, then the post will linearize the arc.

 

Here is the snippet of code from 'pcir0$' that causes the post to linearize the motion:

 

if cir_at_zero = zero linarc$ = one

 

I was able to edit the line in question and force the post to still output an arc move. This may or may not work for your machine, you'll have to test it to be sure. (ALWAYS backup your post before you attempt to make changes)

 

Here is the modified code:

 

pcir0$		   #Pre-circular interpolation postblock
  pmap_plane
  if posttype$ <> two,
    [
    preset_mod
    pshft_map_xc
    if y_axis = zero & millcc = zero,
	  [
	  #Set linarc, breakarcs and cir_at_zero
	  if fmtrnd(xca) = zero & fmtrnd(yca) = zero,
	    [
	    #Set breakarcs and cir_at_zero
	    breakarcs$   = zero
	    breakarcsxz$ = zero
	    breakarcsyz$ = zero
	    #C axis move
	    if mach_plane = zero,
		  [
		  cir_at_zero = one
		  czero_csav = csav
		  if brk_cir,
		    [
		    breakarcs$ = one   #Break at quadrant
		    breakarcsxz$ = one #Break at quadrant
		    breakarcsyz$ = one #Break at quadrant
		    ]
		  ]
	    #Arc output
	    if mach_plane = two, cir_at_zero = m_one
	    ]
	  #if cir_at_zero = zero linarc$ = one #Old line, breaks arcs that aren't on center
	  if cir_at_zero = zero & cuttype <> three, linarc$ = one
	  ]
    ]
  !ynci$

[crazy^millman]

Well there is your difference. Why would it matter if the arc is at X0 Z0 an arc is an arc?

[Colin Gilchrist]

I believe the code was put in to handle cutting arcs on the Face of the part. Depending on the mode you are in you might want G3 motion, or C Axis motion. I think that is the reason we have 'cir_at_zero' as a variable. I'll bring it up to the post department and see if we can revise that logic. The reality is that the broken motion will still cut the same shape, it just won't do it in a single move like an arc, and it wouldn't be as smooth since it is broken into several linear moves.