G54 OFFSET NOT POSTING

[steveo25]

Im trying to get a G54 workoffset to spit out when I post a program . I went into coordinates and typed in 0, that didn't work and then I tried just typing in G54 and its not posting. Im using the Ikegai_fanuc 18i-t post. Can anyone give me a hand?

Thanks

[K2csq7]

What is it giving you?

[steveo25]

just a G0 with nothing at all

[Dave.L]

You are entering this in the view manager for the WCS correct?

[Colin Gilchrist]

Try "54" with no "G"...

[steveo25]

I was putting a 0 or 54 in the coordinate option in each toolpath. I just tried to put it in the wcs view manager and I didnt get anything either. Im still learning all this stuff but it used to work by putting 54 in the coordinate option but I got the posts mixed up and now its not spitting it out.

[steveo25]

The code looks like this:

N110 G50 S700 M42

N120 T0

N130 G55 X0.0 Z0.0

N140 G18 G99

N150 G97 T1212 S1450 M03

N160 G0 X-1.3173 Z.0837 <----

N170 G96 S500

N180 G1 Z-.0163 F.01

N190 Z-1.8383

N200 G0 X-1.4587 Z-1.7676

N210 G97 S39

N220 T0

N230 G55 G00 X0.0 Z0.0

N240 M01

And I want it to look like this:

N110 G50 S700 M42

N120 T0

N130 G55 X0.0 Z0.0

N140 G18 G99

N150 G97 T1212 S1450 M03

N160 G54 G0 X-1.3173 Z.0837 <---- or 56 depending

N170 G96 S500

N180 G1 Z-.0163 F.01

N190 Z-1.8383

N200 G0 X-1.4587 Z-1.7676

N210 G97 S39

N220 T0

N230 G55 G00 X0.0 Z0.0

N240 M01

[jhjr]

Did this work for you before you mixed the posts up? Is your post set up to output g55 for every path? I understand what you want to do with both offsets being output. Check control deff so that work offsets is set for work system. Could be a post issue also. You might have to force your coordinates to be output. Check the control deff first & if that's ok maybe a post guru in here might help you out. Search for pwcs in here & lots of topics come up that might help you.

[Jim Evans from CNC Software]

You will beat yourself bloody without someone taking a look at the post and the MCX file. It could be anything, especially if you have edited the post in anyway. I strongly suggest you contact your reseller for some help so it can be debugged.

 

But if you insist on trouble shooting it yourself and on the forum you should at least post the psof postblock so we can see the code.

[steveo25]

I was mistaken the old post never output a G54, G56 or any workoffsets. So I went back to the original post. How do I post the psof postblock?

Thanks for your help

[steveo25]

This is the code in my post:

 

pwcs #G54+ coordinate setting at toolchange

if home_type >= one,

[

sav_frc_wcs = force_wcs

if sub_level$, force_wcs = zero

if workofs$ <> prv_workofs$ | (force_wcs & toolchng),

if sub_level$, result = mprint(swrkserror)

g_wcs = workofs$

*g_wcs

 

force_wcs = sav_frc_wcs

!workofs$

[Jim Evans from CNC Software]

Steve,

 

The home_type variable is probably controlled from the Miscellaneous integers - most likely number 1. So in your Toolpaths make sure you set the Misc int #1 correctly.

 

Also, the PWCS postblock controls the output of G54, G55 ,etc but you still need to make sure it is called in the start of file (psof) and toolchange (ptlchg) postblocks. Bascially somewhere in the those postblocks a call to pwcs must be made. If it is then refer back to the first paragraph.

 

Most posts are written to use 0, 1, 2, etc for controlling the work offsets 0 =first, 1=second, and so on.

 

again, Is strongly suggest contacting your reseller unless you have time to waste.

 

If you want to keep posting sections of your post switch to the full reply form and use the Code option to and put your post code in between the ubb code brackets as it makes it easier to read - see below.

 

code:

---

psof$            #Start of file for non-zero tool number             

if ra_error = 1, [if mprint(sra_error, 2) = 2, exitpost$]

toolchng = one

if ntools$ = one,

[

#skip single tool outputs, stagetool must be on

stagetool = m_one

!next_tool$

]

pbld, n$, *smetric, e$

pbld, n$, *sgcode, *sgplane, scc0, sg49, sg80, *sgabsinc, e$

sav_absinc = absinc$

if mi1$ <= one, #Work coordinate system

[

absinc$ = one

pfbld, n$, sgabsinc, *sg28ref, "Z0.", e$

pfbld, n$, *sg28ref, "X0.", "Y0.", e$

pfbld, n$, sg92, *xh$, *yh$, *zh$, e$

absinc$ = sav_absinc

]

pcom_moveb

pcheckaxis

c_mmlt$ #Multiple tool subprogram call

ptoolcomment

comment$

pcan

pbld, n$, *t$, sm06, e$

if mi1$ > one, absinc$ = zero

pcan1, pbld, n$, *sgcode, *sgabsinc, pwcs, pfxout, pfyout,

[if nextdc$ <> 7, *speed, *spindle], pgear, strcantext, e$

pbld, n$, sg43, *tlngno$, pfzout, scoolant, pstagetool, e$

absinc$ = sav_absinc

pcom_movea

toolchng = zero

c_msng$ #Single tool subprogram call

---

[steveo25]

I do have alot of time to waste, im just trying to learn as much as I can on my own about the posts. The pwcs is called out at both of the other places you were stating. I sent my post off to cimtech so they can look it over.

I guess I was running a v10 post so it needed to be updated.

Thank you for your reply I appreciate it.

[Jim Evans from CNC Software]

quote:

---

I do have alot of time to waste, im just trying to learn as much as I can on my own about the posts.

---

Steve, that's fantastic for sure. See if Cimtech offers up a generic post class as it will be helpful. Learning the basics of the language (rules, syntax, Etc) along with the default post layout and the reasons behind it goes a long way to being comfortable with editing posts. Just learning what Mastercam provides for data in the NCI and doesn't provide is enough to keep you going for years.

 

Also after doing this for 14 years now there are very few post issues that can be fixed without viewing the code itself along with the part file as I'm sure you gathered from my comments. I can take some stabs at the issues for sure but with the part and post life is much easier.

 

Not everything is available through the standard mastercam toolpaths so the post uses tools to allow the user to pass along more information and many times this is custom type programming in the post - yes we even have to do this on our default posts. As an example with your workoffset questions, by using a Misc Integer the post writer is trying to offer the user some options for configuring their output that are NOT built into mastercam and if you are NOT setting things up correctly in MAstercam then you are chasing output issues so understanding what was intended is important and usually impossible without seeing the code.

 

Hope this helps and good luck in your Journey of post writing.