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

Welcome to eMastercam.com

Register now to gain access to all of our features. Once registered and logged in, you will be able to create topics, post replies to existing threads, give reputation to your fellow members, get your own private messenger, post status updates, manage your profile and so much more. This message will be removed once you have signed in.Login to Account Create an Account

# POST EDIT HELP

Started by
M_CODE1
, Feb 24 2011 02:17 PM

###
#1
Posted 24 February 2011 - 02:17 PM

###
#2
Posted 24 February 2011 - 04:18 PM

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

###
#3
Posted 25 February 2011 - 07:42 AM

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

if absinc$ = zero, *xabs, !xinc

else, *xinc, !xabs

pxout #X output

xabs_dia = xabs * 2

if absinc$ = zero, xabs, !xinc

else, xinc, !xabs

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

###
#4
Posted 25 February 2011 - 10:00 AM

###
#5
Posted 25 February 2011 - 10:33 AM

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

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

###
#6
Posted 25 February 2011 - 10:37 AM

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.

###
#7
Posted 25 February 2011 - 11:26 AM

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

###
#8
Posted 25 February 2011 - 12:46 PM

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.

###
#9
Posted 25 February 2011 - 01:40 PM

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?

What is your email?