Multiple Work Zeros Keeps Biting Me in The....

[hot_chip]

Is there any way to default Mastercam to use one work zero auto-magically no matter where your tool plane is? As in creating toolpaths for 4th axis or live tooling ect... If I'm rotating a tool plane by toolpath translate or not, it always wants to throw in new work zeros for every rotation and not even warn you or put it on a set up sheet. This safety" feature isn't safe it it sneaks past people.

 

Is there a way to set all the Woff# column in the view manager to 0 by default? Is there a way to set the tool path transform parameters defaults. Maybe to maintain the sources operation instead of "Off". where Off doesn't really mean "Off", it means just make up work zeros and throw them in for fun instead?

 

Is it just me or does this seem like an important little detail that could be better managed within the software.

[Jayson Kramer]

Talk with your dealer to add used offset to the head of your post. My Haas and Fadal posts I did this years ago for my customers.

if use more offsets it will list like shown below. Just a thought.

example of a old program header:

O3333 ( 400-160001-001-D_4TH OP1 REV: )

( 400-160001-001-D_4TH OP1 )

(MACHINE TOOL : HAAS VMC )

(DATE - 15-08-10 )

(TIME - 20:27 )

(*)

(MATERIAL: )

(STOCK SIZE: X = 2.375 Y = 2. Z = 2. )

(HOME POSTION COORIDNATES ARE THE FOLLOWING)

(X= )

(Y= )

(Z= TOP OF PART)

(*)

( TOOL - 1 2 -1/2" FACE MILL )

( TOOL - 2 1/2 CARBIDE 3FLT EM )

( TOOL - 3 3/8 FLAT ENDMILL )

( TOOL - 4 1/4 SPOTDRILL CARBIDE 90 DEG )

( TOOL - 7 NO. 27 DRILL )

( TOOL - 5 NO. 36 DRILL )

( TOOL - 6 NO. 6-32 TAPRH )

( TOOL - 8 1/4 CARBIDE 3FLT FLAT EM )

( TOOL - 10 LTR. K COLBOLT DRILL )

( TOOL - 11 1/4 EXTENTED LENGTH CARBIDE EM MIN EXT 1.95 )

( TOOL - 9 3/4 COLBOLT DRILL MIN 2. EXT )

( TOOL - 12 3/4 CARBIDE 3 FLT 2" FLT WITH 2.1 EXT )

(*)

(USING FIXTURE OFFSETS: G54 )

(*)

N100 G20

N110 G0 G17 G40 G49 G80 G90

N120 T1 M6

( FACES TOP OF STOCK )

 

 

Post info:

 

psof$ #Start of file for non-zero tool number

"(*)", e$ #Add line

"(USING FIXTURE OFFSETS: ", pwcs_list, ")", e$ #Add line

"(*)", e$ #Add line

if norm_meta = 1, pstock_out #Added line

if norm_meta = 1, pmeta_slt # Metacut view #Added line

[Jayson Kramer]

Or using these option in the Control Def. as another

 

Use the Work coordinate selection to select the type of coordinate system used by the control:

Setting

Typical post interpretation

Home position

G90/91

Local work offsets

G92

Work offsets

G54, E1

Other

Custom

 

In previous versions of Mastercam, these were typically set in the Miscellaneous values dialog box (by entering 0, 1, or 2). You can still use that technique if you wish, or you can replace it with this control definition setting.

Use the Tplane list to tell Mastercam which Tplanes to include when automatically generating work offset numbers. You can choose to assign work offsets to all Tplanes or just those which are being transformed.

Use the Translate NCI coordinates to Machine View with aggregate checkbox to map the toolpath coordinates when using an aggregate head.

[Guyinthedesert]

I find this very irritating as well. What reakky gripes me, is why your operations go dirty if you change the work offset value.

[MrFish]

Our DMG post has a question at posting that asks you what offset/datum preset you want to use that then over rides all offset outputs. Not good if you want to use more than one offset in your program but awsome for 5 axis work with mulitple tool planes.

[K2csq7]

Hot_chip,

If you would like some help modifying your post to PERMANENTLY only output G54....

Put up a topic in the post forum, I will help.

I have done it to a couple of my posts, it's a pretty easy modification.

[rocheey1]

I've found that listing the work offsets in the Setup Sheet (and the Ops that use them) may jog the programmers memory to go back and double check. Same for D Offsets and Coolant.

[Newbeeee™]

This is where you want to run X+ set sheet from Gunther.

We run it for a quick ceheck before posting, and have it configured for work offset number (as well as a host of other things) and when it runs, it shows offset number against operation number so you can catch this.

Kudos to Gunther