SteveStallings is now known as steves_logging
why are there 2 channels?
this one is for development discussions (why certain code does what, changes to be made, etc)
the other is for user questions, like how to set up EMC2, how to get it to do something, etc.
i am having a problem in that you can not change from G99 to G98 (and G98 to G99) in a cycle as it seems to ignore the change in G99 and G98 - i have a test program
[18:54:05] <robh__> http://pastebin.com/sNfkj8gL
on which line(s) is the motion different than you expect?
it does it right
but on line 15 it does not do a full retract as exspected
i would exspect as detailed in the ( ) i ran it in Sim to check it on what i saw on the machine
so if I delete everything after line 15 up to %, and then delete 13 and 14, I'll still see the problem?
if u did 17 and on correct, as 15 should be done still with retract of Z2 then lift to Z20 to go to line 16
i watched EMC status window and noticed it does not change the G98 to G99 when reading the lines
the modal codes on the mdi tab represent the readahead state not the current motion line state
i ment if u do EMC status from menu in Axis
that's the same source of information, same limitation
aah i see sorry
is there away one can one see the current read states
a G4 in the program will force the current states to match
on line 15 the sticky Z should be -2.7, the sticky R should be 2., the old Z should be what it was at the end of line 14, and G98 should be active
the last motion on line 14 is to Z2., so that's the old Z on line 15
G98 is active so you get option (2) retract to old Z which is 2.
yes but at end of the motion on L15 should return to G99 Z
so it can pass onto L16 at the cleance of Z20
at the start of line 15, the Z axis is at 2 not 20
correct, it should be there untill it has completed motion then retact back to inital Z as asked then process next line
i took this program from the fanuc machine which does as i have described then found EMC did not process the quick plane change in the cycle as exspected
the initial Z (the Z position at the end of line 14 / beginning of line 15) is 2, and that's where it retracts to.
if you change that line to
G98 X51. R1 (drill co-ord in G99, on finish G98 - retract to celarnce Z20)
you'll see that it still retracts to Z2, not the specified R
you expect "the original Z" to mean a different than than emc does. Maybe your definition is something like: the Z position back on line 12 when G82 was first programmed
its staying in cleanernce plane, my inital is alwasy 20 as Z has never changed only the R planes have. so it should rember that G98 is inital plane and not clearnce like G99
but emc's definition is "the Z position when starting to interpret this line of gcode"
one way to to chancel cycle, and redefine all the time, but its very wastfull time of programing etc where a quick change on the plane type and R and Zs and you can soon jump over clamps or boss's
i hope i am making sence what i am trying to explane
I think I understand what you expect. I've tried to explain why what emc does is consistent with what its documentation says. I don't have an opinion about which one is better.
maybe this helps, http://imagebin.ca/view/OI11Ho3M.html
i understand i just through it might a improvment to make EMC more power full and user friendly so what some of us cnc guys are used to, this is why i brought it up
robh__: what control are you using that has the behavior in the top picture?
(by the way your picture is awesome and helpful)
yes which one?
from Fanuc 6 to 31I does it
i can do a video if u like
I don't think that's necessary
what if line 15 said explicitly G82 ... ? would the fanuc still look like your 'expected' picture?
I believe you -- I was wondering if I could find a matching manual online that describes it
and what if it said G83 instead?
we use it alot if we have a grid of holes with boss's clamps or islands in the way, so u can put in all the co-ord then just skip up and over anything and no redefines etc
fanuc manual details it as i have talked about,
i dont know of any online ones sorry
never tryed it, i belive it would ignore it as it would see its still in G82 there
EMC seemed to start the program out ok, which made me thing maybe theres a bug or something, as not many people try and use it in this way i have done here
if you do the R1 on line 15 you'll see what emc is thinking -- that the old Z is 2, not that it's not really getting into G98 for that line..
I do see your side of things
cradek, we have a spare fanuc 10 manual, if you would be intrested?
robh__: does that have all the details about how the gcodes work? I'd be super interested if so.
its programmers manual
big thick book
its Mill i dont think we have a spare Turning one we might
robh__: I have a fanuc lathe manual but I don't remember the model. it is a really old one with no roughing cycles
from your HNC?
no, that was a GE
this is one some other helpful person sent me
well if you PM me your address or some where to send it, i will post it out no problem all free of charge
that would be great, thank you
(wish fanuc would put them all online...)
i keep telling them that, when we see the reps
as every once else does now days
but fanuc service people still have to pay for online access to them, which is quite costly
that's sure stupid
i found they will send the older stuff out now but you have to twist there arm
maybe they can't afford a scanner, since everyone's using EMC instead of buying from them now :-)
that's a good one :-/
like when i do my fanuc mill, i will probly have to buy the servo manuals and spindle to set them up and get the pinouts as service manual does not tell you too much there
every time a machine rep comes into ours and see the EMC machine at work, they cant realy belive what they see on speed and price on a old machine :)
robh__: that is funny :)
aah soz, yel they dont laugh much when u tell them how much you can do it for tho
can anybody think of a way that changing emc to work the way robh details would change an existing emc2 ngc file to retract less far than it does today?
personally, I can't..
(the change seems safe if you never retract lower than before, but unsafe if you could ever retract lower / less far than now_
.. not that I've figured out precisely what one would change to get robh's behavior..
jepler: not me
ries_ is now known as ries