8 replies to this topic

[M_CODE1]

I'll looking to do some surface milling on our swiss lathes to help debur a part.  For that machine my X number needs to be in diameter.  So I basically need to double all my X's.  Anyone know of an easy way to do this.  I don't want to have to change them all by hand.

The post I am going to modify is the Generic Fanuc 3x.


Thanks

[Jimmy Wakeford from Barefoot CNC]

Here is a simple way of doubling x at the point of output. . You have to also add the xabs_ dia variable.(Note it will not work with incremental values without adding more logic.)

fmt "X" 2 xabs_dia
pfxout		  #Force X axis output

	xabs_dia = xabs * 2

	  if absinc$ = zero, *xabs_dia, !xinc
	  else, *xinc, !xabs

pxout		   #X output

	xabs_dia = xabs * 2

	  if absinc$ = zero, xabs_dia, !xinc
	  else, xinc, !xabs

[M_CODE1]

Jimmy

I modified the post in 3 spots.  But now I get an error when I try to post the program.  Any ideas what might be wrong?



fmt  X  2   xabs_dia    #X position output (changed "xabs" to "xabs_dia")


pfxout          #Force X axis output
xabs_dia = xabs * 2 (ADDED THIS LINE)
if absinc$ = zero, *xabs, !xinc
      else, *xinc, !xabs


pxout           #X output
      xabs_dia = xabs * 2 (ADDED THIS LINE)
if absinc$ = zero, xabs, !xinc
      else, xinc, !xabs

[Zoober]

What is the error on posting?

[Jimmy Wakeford from Barefoot CNC]

Oops

Do not change:
fmt X 2 xabs to fmt X 2 xabs_dia
But... add fmt X 2 xabs_dia like:

fmt X 2 xabs
fmt X 2 xabs_dia

Also in the pfxout and pxout post blocks instead of outputting xabs you want to out put xabs_dia

[Jimmy Wakeford from Barefoot CNC]

Also, I got the idea that you were just wanting this post to use for the situation you mentioned. This is just a "down n dirty" way of doing what you want. To incorporate this into a lathe post there is some logic we'd need to add.

[M_CODE1]

Quote

Also in the pfxout and pxout post blocks instead of outputting xabs you want to out put xabs_dia

Not sure where to change to the xabs_dia?  I changed the two in bold and it did change the x's to double.  But now the Z is outputing as a Y, and its not outputting a Z? Example below?


pfxout          #Force X axis output
xabs_dia = xabs * 2
if absinc$ = zero, *xabs, !xinc
      else, *xinc, !xabs


pxout           #X output
      xabs_dia = xabs * 2
if absinc$ = zero, xabs, !xinc
      else, xinc, !xabs



(I added this line)

fmt  X  2   xabs        #X position output
fmt  X  2   xabs_dia    #X position output


(THIS IS ORIGINAL THAT I STARTED TO CHANGE THE X's by Hand)
T252 M6
G0 G90 G54 X0. Y-.1901 S3500 M3
G43 H252 Z.25
Z.0876
G1 Z-.0124 F5.
X.0512 Y-.1892 Z-.0136 F40.
X.1016 Y-.1866 Z-.0172
X.1506 Y-.1822 Z-.0231
X.1976 Y-.1762 Z-.0312
X.2422 Y-.1689 Z-.0411
X.2842 Y-.1602 Z-.0529
X.3236 Y-.1504 Z-.0661
X.3604 Y-.1395 Z-.0808
X.4264 Y-.115 Z-.1139
X.482 Y-.0874 Z-.1513
X.5106 Y-.0695 Z-.1755
X.5358 Y-.0508 Z-.2009
X.576 Y-.0112 Z-.2548
X.6026 Y.0307 Z-.3118
X.6152 Y.0739 Z-.3707(I STOPPED CHANGING X's BY HAND)
X.3071 Y.1176 Z-.4304
X.3033 Y.1448 Z-.4675
X.2969 Y.1715 Z-.5041
X.2879 Y.1976 Z-.5398
X.2765 Y.2228 Z-.5744
X.2627 Y.2469 Z-.6075


(THIS IS THE NEW OUTPUT)
N120 T252 M6
N130 G0 G90 G54 X0. Y.25 S3500 M3
N140 G43 H252 Z0.
N150 Y.1
N160 G1 Y-.0124 F5.
N170 X.0512 Y-.0136 F40.
N180 X.1015 Y-.0172
N190 X.1505 Y-.0231
N200 X.1975 Y-.0312
N210 X.2421 Y-.0411
N220 X.2842 Y-.0529
N230 X.3237 Y-.0661
N240 X.3604 Y-.0808
N250 X.4262 Y-.1139
N260 X.4819 Y-.1513
N270 X.5106 Y-.1755
N280 X.5359 Y-.2009
N290 X.5761 Y-.2548
N300 X.6026 Y-.3118
N310 X.6152 Y-.3707
N320 X.6142 Y-.4304
N330 X.6066 Y-.4675
N340 X.5937 Y-.5041
N350 X.5758 Y-.5398
N360 X.553 Y-.5744
N370 X.5254 Y-.6075

[Jimmy Wakeford from Barefoot CNC]

Are you using the y axis on machine or the c axis? If your doing the path in the right cplane then your x is going back z into part and y is up and down. send me a sample file your trying to do andthe post so far to look at along with desired output if you have it.

[M_CODE1]

The machine is a Tsugami SS-32 swiss lathe.  My part is in the sub spindle and I am going to put a 1/4 ball endmill in the live tool pockets. So I will be using the Y axis, but I will have my c axis turned on for proper orientation. Its just like a vertical mill programing in the Top view, except the X value's need to be in diameter.

What is your email?