Horizontal B-Axis Zero in G54 or in Program?

[Scott Garrison@Weiler Engineering]

Just a poll, if you program a horizontal using multiple work offsets with a rotary B-axis do you like to put the B-zero in the work offset or in the control?

 

Take a rectangular part using G54 for the top and G55 & G56 for the sides 90 deg. each way.

 

program:

G54 X0 Y0 B0

G55 X0 Y0 B0

G56 X0 Y0 B0...ETC...

 

control work offsets:

G54 X..Y..Z.. B0

G55 X..Y..Z.. B90

G56 X..Y..Z.. B-90

 

or do you call the B angle in the program?

 

program:

G54 X0 Y0 B0

G55 X0 Y0 B90

G56 X0 Y0 B-90

 

control work offsets:

G54 X..Y..Z.. B0

G55 X..Y..Z.. B0

G56 X..Y..Z.. B0

 

Obviously G54 B0 can be something other than 0 depending on the fixturing where it is the change in angle between the offsets that matters, in this example it is 90 degrees.

 

I tend to go with the latter because a work offset should include what angle the table is from machine B0. As long as the operator has a set-up sheet showing that G55 is at B90. and G56 is at B-90 relative to G54 at B0.

 

I realize this is using the axis more like an indexer but even if you are machining with the B-axis, wouldn't it make sense for the B coordinate to be B0 when perpendicular to the tool plane it is using? I don't see the advantage to having a "Master work offset B-zero" which is what you have the way the MP master post is set-up.

 

Any horizontal programmers out there with an opinion?

 

Scott

[rickt23]

I have always found it to be less confusing to the operators if G54, G55, G56 etc... have the same Y and B offset and you alter X and Z accordingly. Then if you rotate B axis 90 degrees you have a B90. in the program. So I have had success with your second option.

[Scott Garrison@Weiler Engineering]

Wouldn't that be the 1st option? All work offsets with the same B and call out Bxx in program?

 

Scott

[rickt23]

Your second option has the B rotating in the program. Unless I'm really confused, it is late on a Friday so I could be.

[iowajim62]

fwiw, i'm running this right now. been doin it like this for years

G90G10L20P46X-5.625Y18.895Z2.375

G90G10L20P47X-5.625Y13.395Z2.375

G90G10L20P48X-5.625Y9.915Z2.375

M01

(*)

G0G28G91Z0

G0G17G40G80G90

(SEMI-FINISH FACES B0)

N1T1M6(80 MM CENTURY MILL)

M50

M22(UNLOCK)

G0G54.1P1G90X-3.6245Y0.B0.S8500M3

M21(LOCK)

G43H1Z3.25M8

T2

Z2.85

G1Z2.708F150.

X-1.6245

X6.3755

.

.

.

X-3.6245

G0Z3.25

G28G91Z0

M22(UNLOCK)

G0G54.1P9G90X0.Y-15.5B90.S8500M3

M21(LOCK)

G43H1Z1.

(SEMI-FINISH FACES B90)

X0.Y-15.5

Z1.

Z.225

G1Z.0883F150.

Y-13.5

[Guest CNC Apps Guy 1]

I ALWAYS program with my first face as B0, regardless of where it is physically in the machine. So let's say I have my part on the 90 Deg. Face of my tombstone, and I'm using 3 work offsets to make my way around the part... G54-G56. My work offsets in the machine would be as follows;

 

G54 X(some number)Y(some number)Z(some number) B90.

G55 X(some number)Y(some number)Z(some number) B90.

G56 X(some number)Y(some number)Z(some number) B90.

 

Now, in my program I will have a B0, a B90, and a B270 (if assuming Front, Right and Left T/C Planes). WAY less confusing this way. B90 in the Work Offset basically tells the Machine that B90 is my "home" face.

 

HTH

[Jerosu]

What he said ^^^^^^^^^^^^^^^^^^^^^^^^

[Tim Johnson]

What he said he said ^^^^^^^^^^^^^^^^^^^

 

 

G54 X..Y..Z.. B0 -- face part one

G55 X..Y..Z.. B90 -- face part two

G56 X..Y..Z.. B-90 -- face part three

 

If you are machining multiple sides of one part you can use a coordinate rotation program to calculate the new offsets for the part you're machining.

[c-hook]

For me, it all depends on the part specifically. Usually I will go with however it is called out (dimensioned) on the drawing. If i'm working with a box shape that has alot of features on each side, I would probably set the B0 in the work coordinate rather than call up B90. B180. etc. But again, all depends on the parts features, and how they tie in together etc.

[Scott Garrison@Weiler Engineering]

Just seems logical to me to have the B0. in the work offset because it is just a 4th zero location for that work offset.

 

The real only reason you can do it with the angle in the program is that the B angles are simple, usually an increment of 90 degrees. If not, then this would not even be an option.

 

I do see the logic in having one angle in the offsets so that is known to be the home face and less chance of the operator putting in the wrong angle in an offset as well. Not to mention my post is already working this way.

 

I guess that this is the main programming difference between a linear & rotary axis. I think I will stick to having the angle in the program, also might be easier to follow in the program as well.

 

Thanks all for your opinions.

 

 

Thanks all.

[Greg_J]

Hi,

It all depends on what part your machining and what machine you are using.

 

If you are machining a block and you want to call each side of the block 0,90,180 & 270 each offset will have the same "B" value. Mastercam post the angle in the program and it will rotate to the side called.

 

That's how I do it.

Greg

 

[ 11-12-2007, 12:46 PM: Message edited by: Greg_J ]

[Rick Henrickson The Boeing Co.]

I am with James the other thing I consider is the offsets for front right and left to help translation B0 face is P1 right P2 left P3 then add 10 on translation op that way the operators always know P1 And P11 are front P2 and P12 etc you guys get it

 

then if they load the part on B90 they just add that to the offsets

 

Tim is right on with the autocalc on rotation ours is m300

 

but I try to program from center rotation all the time unless it is a messed up casting with tooling jacks.