Rotation questions - B address

[spade117]

Couple of questions:

 

In the code below, is there a way to prohibit the g-code from using #'s higher than 0-359.999 for B address? I'm not a fan of the negative B numbers or the B360, B540, etc.

 

Also after N block 4950, it posts out B0. when it is un-needed. That seems to be happening once per program, and I don't know why.

 

 

code:

---

()

(1/4" SPOT DRILL 32142 )

()

N4800 (SPOT .206 HOLE B0)

N4810 T19 M106

N4820 G00 G17 G90 G55 B360. X.395 Y1.963 S7400 M03

N4830 G43 H19 Z.1 M08 T14

N4840 G94

N4850 G98 G81 Z-.676 R-.5 F40.

N4860 G80

N4870 G91 G30 Z0.

N4880 (SPOT .206 HOLE AT B180)

N4890 G00 G90 G56 B540. X-.395 Y1.963

N4900 G43 H19 Z.1

N4910 G98 G81 Z-.362 R-.2 F40.

N4920 G80 M09

N4930 M05

N4940 G91 G30 Z0.

N4950 G30 B0.

N4960 M01

()

(13/64 JOBBER DRILL, .2031" )

()

N4970 (DRILL .203 HOLE AT B180)

N4980 T14 M106

N4990 G00 G17 G90 G56 B180. X-1.14 Y2.365 S6500 M03

N5000 G43 H14 Z.1 M08 T12

---

[Grievous]

This is from my post for C axis output. Check your adressinstead of "cout_a" use your adress for B.

 

pfcout #Force C axis output

pspindle_nr_select

cout_a = cabs

if one_rev & cuttype = 3,

[

while fmtrnd(cout_a) >= 360, cout_a = cout_a - 360

while fmtrnd(cout_a) < 0, cout_a = cout_a + 360

]

 

For the B0 on the N4950 line check your retract routine.

[spade117]

quote:

---

For the B0 on the N4950 line check your retract routine.

---

If it was the routine, wouldn't it happen every time?

[YoDoug®]

Look in the top of the post for "limit rotation to 360" and turn it on, set it to 1. This will stop the B540 junk and also will eliminate the unwind you see in line 4950.

 

From mpmaster

 

code:

---

 one_rev     : 0     #Limit rotary indexing between 0 and 360? (0 = No, 1 = Yes) 

---

[Guest CNC Apps Guy 1]

It's probably in the peof postblock which could explain why you're only seeing it once per program.

 

Just a thought.

[spade117]

That worked Doug.

 

Thanks.

[Dead Money]

Spade has this issue fixed but I just ran into another.

 

I have multiple work offsets that have the same "B". In my program I machine some features @ G56 B270 then move to the other side of the tombstone and machine @ G57 but the post is not posting a B. How can I force B outputs for all work offset changes?