Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

$1million to the Okuma Guru that can answer this!!!


Recommended Posts

ok, maybe slightly less than $1million. :harhar:

 

machine: Mac-turn 30 osp7000

 

G126
G136
N100 MT=5203.
M321
G21HP=1
M403
SB=2500 G52 TL=5252 BA=0.
M404
M110
G21  HP=4
G138Y0.
G136
M146
G00 C0.
G137
M13
G00 X1.9978 Y0 Z2.
G00 Z.1
G94 G101 Z0 M08 F12. (**positions and cuts end of bar just fine**)
X.9978 F38.
G102 X-.9978 L.9978
X.9978 L.9978
G101 X1.9978
G00 Z2.
G136
G00X300
G21 HP=1
M12
M146
M109
M9
M02

 

 

 

 

 

 

G126
G136
G21HP=1
N100 MT=5203.
M321
M404
G21HP=4
G138Y0.
G136
G00X300Z300
SB=1800 G52 TL=5252 BA=90.
M403
G21HP=4
G138Y0.
M110
M146
G00 C180.
G138
G127B90.G52
G17
M13
G00 X.25 Y.7115 Z4.
G00 Z1.35
G94 G1 Z1. M08 F12. (**measured thickness of flat oversize by varying amounts depending on parameters**)
Y-.4615 F38.
G00 Z3.
M146
C0.
M147
G00 X.25 Y.6839
G00 Z1.35
G1 Z1. F12.
Y-.4339 F38.
G00 Z4.
G126
G136

 

 

turret comp values alter the z calibration of the tool setter, which probably why i can mostly hit z- zero on end of bar just fine.

 

local applications doesn't seem to know much more than me on the turret comp.

 

i'm dying here :wallbash:

  • Like 1
Link to comment
Share on other sites

 

 

G127B90.G52

 

A G52 does not need to be included in the G127 call. G52 is a tool offset rotation command. G127 is a coordinate rotation command. Different functions that are used together but in separate commands. That may be what is causing your problem.

Link to comment
Share on other sites

Yeah, I tried it without also. Grasping at straws. I've been using it consistent with TL, so maybe delete that too?

Instruction sheet I posted in other thread to doesn't even mention G127 for calibrating parameters.

Very confusing instrucrions

I'm able to measure and calibrate param for the difference between mill side and lathe tool side along z (.029). Doing this results in getting the same TLO length number for the same tool, in both positions. Not clear if .029 needs to be in t1 parameters or t3.

 

Link to comment
Share on other sites

The G127 does not need any calibrating. It is just a coordinate conversion. As far as the T1 to T3 calibration from the mill head to the lathe head, I have never worked on one so I really can't offer any help. I know on newer Multus/Macturn there is a procedure to measure the B axis pivot distance. It is those parameters that the G52 call uses to comp the TLO to match the B angle specified. 

  • Like 1
Link to comment
Share on other sites

The error comes from your offset call

 

TL=5252 BA=90.

 

A Macturn has 2 offset sets BT=0 BASE-A and BT=1 BASE-B  BT=0 is the default so if nothing is programmed then we use the horzontal BASE A BT=0 offset. This is why you need the G52, to recalculate the offset at the BA=90 angle. I think it will work better if you use the BASE B offsets

 

Please try TL=5252 BT=1 with NO G52

 

MACTURN.jpg

  • Like 1
Link to comment
Share on other sites
  • 1 month later...

:unworthy: :unworthy:

this machine has BT40 holders, so no M-axis tool index is optioned. so i'm not sure how applicable the nice chart above is. but thanks.

 

From this:

M403

TL=5252 G52  BA=90.

SB=1800 M13

M404

G21 HP=4

G138 Y0.

G127 B90.

G17

 

I changed to

M403

TL=5252 G52  BT=1

SB=1800 M13

M404

G21 HP=4

G138 Y0.

G127 B90.

G17

******tool offset didn’t take effect and machine looked like it was going to try to cut with the turret*********

also just tried "TL=5252 BT=1" and seems to get the same crash result

Link to comment
Share on other sites

This program is supposed to cut a 2” circle on the face (.04 deep) then rotates to cut a .500 wide flat @1.0" from centerline.

 

With t3 comp set at X.008 and Z.029 the circle cuts at 2.070 and the flat seems right on at .500wide but at 1.025 from centerline.

With t3 changed to X-.067 , the circle cuts at 2.000 and the flat width reduces by the .070 as the machine applies the comp at B90.

 

I don’t understand why with .008 in T3 comp cuts wrong at b0 and relatively right at b90….

 

( CAXIS ONLY FACE CONTOUR, HEX, LEAVES 2.0IN BOSS )
(  1/2 FLAT ENDMILL )
G126
G136
N100 MT=5203.
M321
G21HP=1
M403
SB=1800 BT=0 TL=5252 BA=0.
M404
M110
G21  HP=4
G138Y0.
G136
M146
G00 C0.
M13
G137
G00 X0 Y-2. Z2.
G00 Z.21
G00 Z.06
G94 G101 Z0 M08 F12.
Y-1. F38.
G102 X-1. Y0 L1.
X0 Y1. L1.
X1. Y0 L1.
X0 Y-1. L1.
G101 Y-2.
G00 Z.21
( CAXIS ONLY FACE CONTOUR, HEX, LEAVES 2.0IN BOSS )
(  1/2 FLAT ENDMILL )
M09
G00 Y-2.25
G00 Z.06
G101 Z-.04 F12.
Y-1.25 F38.
G102 X-1.25 Y0 L1.25
X0 Y1.25 L1.25
X1.25 Y0 L1.25
X0 Y-1.25 L1.25
G101 Y-2.25
G00 Z.21
G00 X8. Z5.
G136
( C AXIS ONLY CROSS CONTOUR, CUT ALONG PART Y AXIS )
G138
G00C-90.
M12
G21 HP=1
M403
TL=5252G52  BA=90.
SB=1800 M13
M404
G21 HP=4
G138 Y0.
G127 B90.
G17
G00 X-.26Y-1.45 Z1.25
G00 Z1.1
G1 G94 Z1. F12.
X.29 F38.
Y-.75
Y.75
Y1.45
G00 Z1.25
( 2D CONTOUR, BOTT PLANE )
G00 Y-1.45 Z9.
G00 Z1.629
G1 Z1. F12.
G41 Y-.75 F38.
Y.75
G40 Y.95
Z1.629 F55.
G00 Z9.
G126
G136
X300
G21 HP=1
C0.
M9
M02

Link to comment
Share on other sites

Remove the G52 from the BT=1 line,

Also try it with and without the G127 block, If you are cutting on the face of the part we should not need to rotate the coordinates with G127

 

 

M403

TL=5252 BT=1

SB=1800 M13

M404

G21 HP=4

G138 Y0.

G17

 

 

******tool offset didn’t take effect and machine looked like it was going to try to cut with the turret*********

also just tried "TL=5252 BT=1" and seems to get the same crash result

i tried TL=5252 BT=1, had to stop before crash.

...g52 bt=1 had same result.

 

 

Machine has 96 offsets. Each has X,Z and X,Z for tool nose radius

 

manual shows pages for horiz AND vert turret position error comp. ****machine only has one page****?????

Link to comment
Share on other sites

far as i can tell only t1 and t3 have any effect which seems reasonable since were using those two positions for turn and milling, respectively.

T3 X has effect explained above. T3 AND T1 Z seem to only effect TLO while using the tool setter. Setup with the correct differential they can make a tool have the same length offset for both the milling and turning side (useful for drills that can get used both ways).

Link to comment
Share on other sites

my machine has IGF.

no experience with it...

 

 

 

Doesn't seem right that comp values would be in the .070" range. There must be something simple setup on the machine that I'm not seeing.

i put an indicator on the chuck to find machine X zero from the taper on the lathe side. IIRC it was around .050" off from how i received the machine. I assumed this was something to do with an operator trying to compensate for the head being out of alignment.

 I've used the installation/technician guide to measure the pivot point parameter which was basically right on the money at about 6.3xx".

maybe i need to zero these T1/T3 turret comp values before checking X zero????

Link to comment
Share on other sites

uuugh, yep; something simple indeed.

 

with the local applications guy we zeroed in the turret comp best we could based on very confusing instructions, finally double checking X zero with indicator in lathe side spindle taper.

 

anybody see the issue with that? :whip:

 

the values in turret comp were altering the numbers for X centerline, which throws off the mill side X zero.

 

Boy, don't I feel pretty dumb now, but the good news is it seems to be cutting right on the money now.

thanks for everyone's efforts

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...