G COMP ON RAPID MOVE help

[CVLVNB]

hi it there a way to force  G COMP ON RAPID MOVE

 

N19 G00 G42 X1.2813 Y13.   **  G COMP 42 OR 41
N20 G00 Z.2
N21 G01 Z0 F30.
N22 G01 X.7813 Y13. F150.
N23 G02 X-.2188 Y14. R1.
N24 G03 X-27.7813 R-13.7813
N25 G03 X-.2188 R-13.7813
N26 G01 X-.2161 Y14.15
N27 G00 Z.2
N28 G40

 

I TRY TO FORCE OUT , however  IT ONLY COME OUT G40

 pcan1, pbld, n$, [if gcode$, *sgfeed], *sgcode, *sgabsinc, pwcs,*sccomp, pfxout, pfyout, pfcout, e$  # first rapid fr tool change

[CVLVNB]

HELP  PLEASE

[Guest]

I may if I have a few minutes today see if I can work out the how....

 

Curious though, what kind of machine is requiring that kind of output?

[Guest MTB Technical Services]

I can't imagine that there is actually a machine that requires this type of output.

 

Why on earth would you want to do this?

This is a poor programming practice.

You should only comp a toolpath at the point where it begins interpolated motion

and then cancel comp at the end of the interpolated motion.

You rapid between the end of one and start of another.

 

The default Mastercam posts are already setup to output comp properly.

[djstedman]

I totally agree with Tim, I didn't look into this because it appears to be an attempt to avoid having to verify clearances when turning comp on and off.

 

Many machine types wouldn't even allow turning on comp on a rapid move without throwing an alarm. I am also pretty sure that turning on/off comp prior to/after changing Z heights would also throw alarms on many machines.

 

IMO rather than modifying the post, it would be more prudent to learn how to create code with the existing post that works properly.

[CVLVNB]

yeah, i know it crazy, however; it work on this  old controler

cms router. allen bradley (osai)  10feet x 6 feet table 2 head twin spindle .  program written to the center, we use machine comp

 

for ex; 6 x 4 rectangle 

t1m6

s18000 m03

h1                    ( h= height offset "z" and  tool dia offset "D" )

go g42 x-.1 y0.

g0 z.2

g1 z-.25   f30.

x6. f150.

y4.

x0 .

y0.

g0 z.2

g40

we use machine comp  if t1=.5 dia   offset tool table  dia =.5

this control it old, the   offset tool  parameter it  take positive # only can't be - (negative )

if the part  come out  .01 bigger , in the tool table offset  can't  take  negative number.

if program to the ( computer ) comp.

we array and nest alot of pcs . we comp in rapid move before enter the  g01 plunge

that why we  program to the center of the part  and use machine comp.

if  the part .01 bigger , we adjust offset tool talbe.   offset dia=.49

yes, i had been teach  different way, im new at this company have to fallow their rule.

they use  camworks  and their post come exactly what they requested .  im a mastercam  (new seat)

try to write the post to  match their post.

[Guest]

Get in touch with your reseller, they have an OSAI post processor

[djstedman]

There are 3 types of tool compensation in Mastercam,

 

Computer - this is essentially no comp and is programmed based on the centerline of the cutter using the programmed cutter diameter as a constant

 

Wear - this is the one most people are most familiar with, the tool offset value in the machine is the amount of 'wear' on the cutter, the tool is also programmed from centerline of the tool and the machine alters the path based on the amount of 'wear' on the cutter as defined in the tool offset

 

Control - this sounds like the comp your control is using, this is programmed based on the actual geometry of the part you are going to cut not based on tool centerline, the control on the machine offsets the tool by half of the value in the tool offset on the machine when comp is turned on and when it is turned off. This tends to be why people have an issue with turning comp on and off when using control comp because it moves the cutter if the lead in/out is setup wrong in Mastercam.

 

That control is using control comp and not wear comp, that is why tool offsets are equal to the full diameter of the tool, and why it does not allow negative offset values. There is no such thing as a tool that has a negative diameter.

 

Posting standard code will work so long as you have the proper lead in/out defined in Mastercam, lead in/out should be set to perpendicular and should be at minimum 50% of the cutter diameter (if using a radius on lead in it should also be set to a minimum of 50% of the cutter diameter)

 

If you set your values for lead in/out to the amount you actually want for line and arc values.. and then add 50% of the cutter to them both.. it should work just as you see it on screen in Mastercam.

 

The reason that they are turning the tool on and off above the part is because they are unable to predict the tool movement when comp is turned on and want to avoid gouging the part, the correct way to address this in Mastercam is to correctly set your values for lead in/out, not by modifying the post.

 

If you don't want to go that route, another way to accomplish the same thing as what you are attempting with the post.. is on the lead in/out page there are two checkboxes one on lead in and one on lead out which read Plunge After First Move and Retract before last Move , check both boxes and set your lead in/out value for line at 50%, this will make the code so that the comp gets turned on above the part on the linear lead in and shutoff above the part on the linear lead out, it wont require any post mods and will still create code that looks like the code you posted above.

[Guest MTB Technical Services]

yeah, i know it crazy, however; it work on this  old controler

cms router. allen bradley (osai)  10feet x 6 feet table 2 head twin spindle .  program written to the center, we use machine comp

 

for ex; 6 x 4 rectangle 

t1m6

s18000 m03

h1                    ( h= height offset "z" and  tool dia offset "D" )

go g42 x-.1 y0.

g0 z.2

g1 z-.25   f30.

x6. f150.

y4.

x0 .

y0.

g0 z.2

g40

we use machine comp  if t1=.5 dia   offset tool table  dia =.5

this control it old, the   offset tool  parameter it  take positive # only can't be - (negative )

if the part  come out  .01 bigger , in the tool table offset  can't  take  negative number.

if program to the ( computer ) comp.

we array and nest alot of pcs . we comp in rapid move before enter the  g01 plunge

that why we  program to the center of the part  and use machine comp.

if  the part .01 bigger , we adjust offset tool talbe.   offset dia=.49

yes, i had been teach  different way, im new at this company have to fallow their rule.

they use  camworks  and their post come exactly what they requested .  im a mastercam  (new seat)

try to write the post to  match their post.

 

Nesting parts is irrelevant to the issue.

 

JParis is right.Get the right post from your dealer.

 

Trying to do what you want to do CAN be done but will require reading ahead for (buffering) the op data.

The reason your current post edits don't work is because the ccomp state at the point it is output is off (G40).

[CVLVNB]

thanx you. i use the 2 check box for plunge . it works ,close enough