Changing work offset numbers

[Sticky]

Can you change Mastercams default 0=G54 1=G55 etc work offset scheme to just G54, or G56 etc? I'd like to be able to do extended work offsets as well. G56 J21 etc... I'd love to be able to just type this in the view manager or the specific tool ops I want the work offset tied too.

 

I could get over Mastercams defaults if at least 1=G54 2=G55 etc just like you write workoffset data with G10's Fanuc or Yasnac, or even renishaws probing cycles.

 

The problem I am having is integrating probing routines and G10's into Mastercam, and trying to keep my operators clear on "0" offset in mastercam is G54, but the g10 data write P1 is G54 and the renishaws probing cycle S1 is writing to G54 as well...

 

Thanks!

[Brando]

do you mean so when you type in 54 as a work offset # mc it will output g54 in the program? and of you type 1 or 2 it outputs g54 p1 g54 p2?

[CJep]

If you assign a value to a plane in the view manager then when the code is posted the work offset will be output,..

 

-1 grabs the next available offset

0 = G54

1 = G55

2 = G56

3 = G57

4 = G58

5 = G59

6 & up will activate the auxiliary offsets, but it will depend on the post, the gen Haas will output G110, to output G154 or G54.1 P-value you could start with the MpMaster post

[Sticky]

Brandon, the first half of your sentence yes, the second half no. I'll try to explain better.

 

Cjep, Yes I understand that is how it works now, what I am saying is that I don't liek it that way:) Its retarded and counterprodcutive

 

What would be most convienent is if I could just type in whatever work offset I want, LITERALLY, into the view manager or tool path. So if I want to use G54, I just type in G54, and nothing else. If I want G56, then that is what I type in. If I want to use extended offsets then I would like to just type in G5x J21 or G5x J12 etc.

 

The reason being is that at the start of every program I have a manual entry that writes the work offsets for that program, like such:

 

G10 Q2 P(m) J(n) X…Y…Z…B…

 

G10=Data write

 

Q2 specifies work offset write (the command for tool data is different)

 

P is the work coordinate system “m” to write to:

 

P or P1=G54

P2=G55

P3=G56

P4=G57

P5=G58

P6=G59

 

The J(n) command is the offset extension address,

 

No J specification, J0 and J1 are all = to null or the base P command ie all equal G54

J3 = J3

 

So if you want to write to G57 J20 you command:

 

G10 Q2 P4 J20 X…Y…Z…B…

 

To further the point when using renishaw easyset calls to the commands to write to workoffsets use the same numbers

S1=G54

S3=G56 etc

 

So the issue is that there is too much potential for confusion when we are already writing workoffsets using a certain numbering sequence and then they have to try and remember the MC way on top of it which is close but no tthe same. Does anyone know why MCC does this anyways? All the other cam stystems I have used you just specify the ACTUAL offset you want to use, instead of a conversion...

 

So to cap it off I'd be happy to either have MC use 1=G54 3=G56 etc or just let me type in the actual offset.

 

Thanks for the help!

[Brando]

ever done a post edit? i modified my post to output it as such , mc type in "54" i get prg g54, and in my case i use the 1-49 extented offsets so i mc type in 1 and i get prg g54.1p1

[Sticky]

ever done a post edit? i modified my post to output it as such , mc type in "54" i get prg g54, and in my case i use the 1-49 extented offsets so i mc type in 1 and i get prg g54.1p1

 

Unfortunately I don't know anything about editing MC posts. But is that all that needs to be done? Just a post edit?

[Brando]

depending on the post you are using , the post uses the value you type in that field and does a little logic action on it a decides of you want a g54 or g54.1p1, or haas style g129,, the default recongnizes 0 as g54 and 6 as g54p1, (if am wrong its been so long since ive used the default)

certain things are easy to modify like the work offsets deal once you figure out what the heck your looking at when you open up a post file, some stuff is way beyond me though too, im pretty sure changing the work offset logic would be considered childs play post wise to an expert

anyway are you using a post that came with mc? like generic fanuc 3x or something along those lines?

[Sticky]

depending on the post you are using , the post uses the value you type in that field and does a little logic action on it a decides of you want a g54 or g54.1p1, or haas style g129,, the default recongnizes 0 as g54 and 6 as g54p1, (if am wrong its been so long since ive used the default)

certain things are easy to modify like the work offsets deal once you figure out what the heck your looking at when you open up a post file, some stuff is way beyond me though too, im pretty sure changing the work offset logic would be considered childs play post wise to an expert

anyway are you using a post that came with mc? like generic fanuc 3x or something along those lines?

 

Its an MP master 4 axis fanuc hmc post lightly modified by In House (my reseller). Sounds like someone there should be able to do it for me then. I've requested it 2-3 times now and always get blank stares. I'll get back to bugging them about it.

[Brando]

yep they should be able to do it for you no problem,

[Sticky]

Thanks Brandon!

[Newbeeee™]

Yes - post edit. We did ours to output as you want (enter 54 post outputs G54 etc).

Also it outputs an alram at posting if 53 or below, or 60 and above get entered.

Ours can't do the G54.1, but it maybe best to input 541 for 54.1, 542 for 54.2 (I'll have alook at this as we 'nearly' needed extended offsets the other day...)

Just entering 1 for 54.1 maybe confusing as someone who is used to getting G55 output may not realise G54.1 is output...(crash bang wallop )