G55 Posted instead of G54

[Trevor Rogers]

I'm running Mastercam X4 MU3...Twice in the last 2 weeks I have had a toolpath post out with a G55 instead of G54. This happens when I have booked multiple toolpaths under one filename. I was able to repeat this with one of my Mastercam files but not the other. The first time it happened, I posted the toolpath where the G55 showed up by itself and it posted with G54. When I booked it together again with the other 2 it posted G54 for the first toolpath, G55 for the 2nd toolpath and switched back to G54 for the last toolpath. This has only happened twice out of thousands of toolpaths I have posted. I'm getting my butt chewed and I don't like it very much... Fortunately it has sent the spindle to maximum Z instead of into the table, but one of these times I ain't gonna be so lucky...HELP!!! Has any one else seen this issue?

[gibbs machine corp]

Trevor, I've seen something similar. I now make sure all my work offsets are set to 0 instead of -1. You can set this in the View Manager for the WCS's. If you need to change a bunch of operations you can use Edit Common Parameters in the Operations Manager by picking all (or just some) the ops and right click. You should see a Planes button, it will bring up a list of the WCS's. After you set all the ops to work offset 0, they might dirty up and you will have to regen. I do this EVERYTIME, NO EXCEPTIONS! Better safe then sorry! Hope this helps.

[Thee Rickster ™]

Try re-picking your MMD and see if that helps.

 

Once in a while I create a machine group and it

grabs a 5 axis mmd for no reason. I have deleted

all the machines except the only one I ever use,

(after initial install) and it occasionally finds

this 5 axis one, some how.

 

Re-picking clears many a problem for me.

 

Hope this helps

[Trevor Rogers]

To Rickster: Yes, I did try re-picking the mmd... one of the first things I tried... didn't help in this case...

 

Gibbs: yeah, I'm gonna have to do that from now on unless someone comes up with a better solution... what is most frustrating is that I've been using Mastercam for years, and in particular X4 for quite some time and this has never happened til now... caught me by surprise (the operator too from what I heard) owe him a beer for scaring the crap outta him!!!

 

Any one else with ideas?

[Bob W.]

Trevor,

 

I have had this happen and it is very frustrating. DON'T TAKE ANYTHING FOR GRANTED WITH MASTERCAM! Check the code on the machine with dry run, set all unused offsets to a safe level so when this does happen you don't run through a vise or something. Also, number your work offsets to something other than -1.

 

Why can't we set a default for the work offset in Mastercam so it will not skip to other work ossets randomly? Seems like you can customize about everything EXCEPT a default work offset of 0. Doesn't make any sense because when this is overlooked and Mastercam does output a random work offset the results can be expensive.

[Trevor Rogers]

Amen to that Bullet Bob... like I said in my first post, I got lucky that the spindle went up instead of thru the part or into the table. Is this problem strictly an X4 issue or has it happened with past versions? And yeah, why can't we set a default for the work offset? It seems like that would make a lot of sense...

[Josh T™]

How about Lock On First WCS?

[Bob W.]

I often transform toolpaths to other work offsets so having the post lock on the first WCS would be a PITA.

 

I have been using Mastercam for a number of years as well and I have only run into this issue a few times. It would be better if it happened all the time so we wouldn't get a false sense of security. It is so bad because it is completely random, doesn't happen very often, and just springs up out of nowhere.

 

I had it happen on a program that I had completely proven but simply tweaked a few depth cut values and reposted. Whammo, G55 out of nowhere!

 

What kind of sauce is CNC putting in their spahgetti code anyways :-)

[Cuda84]

Trevor

 

Its not a new problem. I saw this when Covert first got MasterCam (V9, X). I had Fastech hard code the G54 into the posts, so the post dose not get the info from the program or workplane it just always posted G54. Do you have a new post that you got after I left? If not it could have just got changed after running thru the update post 3 times since I left.

 

[Trevor Rogers]

Good to hear from ya Dave! Yeah I think you may be on to something... when I switched to X4 I ran the update post utility... I bet that's what happened... I will relay that to Fastech and see what they come up with... Thanks...

[Acro Engineering]

I too have had this happen in the last few days, along with a few other srange things since Maintenance has elapsed... Seems like a ticking time bomb tied to a maintenance date?

[Tyler Robertson]

Hey Trevor - nice to hear from you, but too bad about the reasons!

 

Do your machines have a minimum Z setting, as well?

 

On a lot of robots I see people set a minimum Z at like 2mm above the table. So while a part isn't saved, at least if it's a move below it, you're safe

[Trevor Rogers]

Hey Tyler, back at ya... the machines in question are CNC machining centers... using the same post for multiple machines. I think the post from Cuda84 is going to be right on the money... he used to work here and he had our post set up to only post G54 and I think from updating these posts to newer versions of Mastercam it has reverted back. I have Fastech in Findlay, Ohio looking into it now... as soon as I hear from them, I will post what I find on this forum...

 

If anyone else has any ideas, I am definitely all ears...

[Rob @ Target Machine]

Maybe a warning message will save a scare now and then.

 

Define the message:

code:

---

swcswarn      : "WARNING - MULTIPLE WORK OFFSETS POSTED"

---

Test for the condition and call the message box:

code:

---

pwcs            #G54+ coordinate setting at toolchange

if wcstype = two | wcstype > three,

[

sav_frc_wcs = force_wcs

if sub_level$ > zero, force_wcs = zero

if sav_mi9 = 1, workofs$ = sav_workofs

#

if workofs$ > 0, #<----Here

[

result = mprint(swcswarn)

] #<----to here

#

if workofs$ > 153,

[

result = mprint(swcserror)

exitpost$

]

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

[

if workofs$ < 6, #G54 - G59

[ #0 - 5

g_wcs = workofs$ + 54

*g_wcs

]

if (workofs$ > 5 & workofs$ < 54), # G54 J2 - G59 J9

[ #6 - 53

p_wcs = workofs$ - 6

*sjwcs

]

if workofs$ > 53, # G54.1 P1

[ #54 ++

p_wcs = workofs$ - 53

"G54.1", *p_wcs

]

]

force_wcs = sav_frc_wcs

!workofs$

]

---

HTH