mb66vb tool change procedure

hello, i just finished my 1st tool change procedure for the mill ; i did not attached it to a G code ( macro ) yet

actually, i do not know how

availabes syntaxes :

CALL OCHG VC190=active tool VC191=next tool
CALL OCHG VC190=active tool
CALL OCHG VC191=next tool
CALL OCHG

... it moves spindle to right if above senzor
... after "next tool" is prepared, M64 comes in, to avoid magazine "lift up" during cutting
... it handles EMPTY values, in case a variable gets "nill" ? or how would you call it ? kindly !

Good work on the macro. What control does your MB66 have? If its an E-100 control or later, did you know that rather than using a CALL statement that you can alias this macro routing to a G or M code. G/M Code aliasing is found in Parameters. For tool change macros, most Okuma users use G116.

Tskinner said:

Good work on the macro

Click to expand...

thank you

Tskinner said:

What control does your MB66 have?

Click to expand...

osp-p300m

Tskinner said:

If its an E-100 control or later, did you know that rather than using a CALL statement that you can alias this macro routing to a G or M code. G/M Code aliasing is found in Parameters. For tool change macros, most Okuma users use G116

Click to expand...

i will attach it to a macro .... i have never used macros before, and i wish to document about macros, *.lib, etc ...

deadlykitten said:

... it moves spindle to right if above senzor

Click to expand...

i wish to explain this a bit : if you cut a single part, than this is not necessary, because, in general, spindle is up, moves @ xy, and after that it lowers

on multiples parts, there is no need to raise the spindle to max, but only above the fixtures, and so, "above the fixtures" may be pretty closed to "senzor height", and in this case, such a behaviour, makes things safer

ps : i did not learned it the hard way

Macro looks good. What sensor are you referring to? I may need to create a tool change macro as well so that I can automatically handle the through spindle air blow and spindle nose air blow before changing to the next tool.

I'll have to look at the manual again, but I think there are even some M codes to control the magazine (i.e. go to pot X), which would be neat for making everything happen at once. We have a side mount 48 pot tool changer, so it can take awhile if for some reason the next tool is on the other side of the magazine.

Macro looks good

Click to expand...

thx

What sensor are you referring to?

Click to expand...

senzor for measuring tools, located in top-left corner; mine works only for Z it has a surface of 100x110mm2, and, by code, i move away from that area

so that I can automatically handle the through spindle air blow and spindle nose air blow before changing to the next tool.

Click to expand...

i understand through spindle air blow, but why also spindle nose air blow ?

also, i am working on "blows"

good luck with yours

deadlykitten said:

i understand through spindle air blow, but why also spindle nose air blow ?

Click to expand...

Our machine uses CAT50 big plus tooling, which has spindle taper contact and flange contact. There is an air nozzle oriented right at the spindle nose so that chips, etc. are cleared before a tool change. We actually have more regular CAT50 tooling than we do big plus, so it's not too big of an issue.

Also deadlykitten, if you want to save up on your precious few common variables (I only have 200), you can change up your code to pass arguments to your OCHG macro. I can't quite remember the format, so you'll have to refer to your manual, but I think it would look something like this:

CALL OCHG T20 Q21
-or-
G116 T20 N21

Then your macro would use PT (active tool) and PN (next tool), thus freeing up two of your common variables. Here is Edster's macro for reference:
http://www.practicalmachinist.com/vb/cnc-machining/okuma-mill-program-263659/#post2011985

hello Jefflikesbagels

Also deadlykitten, if you want to save up on your precious few common variables (I only have 200)

Click to expand...

i also have 200 ; don't you think 200 is enough ? do you need more ?

...you can change up your code to pass arguments to your OCHG macro

Click to expand...

i will "macro" this soon ...

Here is Edster's macro for reference:
http://www.practicalmachinist.com/vb/cnc-machining/okuma-mill-program-263659/#post2011985

Click to expand...

i looked at all examples from that forum ; actually, i received a few time ago a macro from somenone, and i did not understand it at 1st; only after i wrote mine, i was able to understand the exemple that i was given ; that example looked pretty much the same as the one from the link you send me.

Our machine uses CAT50 big plus tooling, which has spindle taper contact and flange contact. There is an air nozzle oriented right at the spindle nose so that chips, etc. are cleared before a tool change. We actually have more regular CAT50 tooling than we do big plus, so it's not too big of an issue.

Click to expand...

"1lock" : taper
"2lock" : "1lock" + flange
"3lock" : "2lock" + taper expanding

[ advantages ]

"1lock" : what can i say ; is used in most cases
"2lock" : reduces radial play, thus less deviation between cone axis and spindle axis; a bit more stabble cutting
"3lock" : "2lock" + taper expanding : less torque required when cutting; thus more stability

[ 1lock ] pull stud is raised so, all pull force clamps the taper ( pull force = taper clamp )

[ 2lock ] pull stud is raised until flange contact appears; in this moment, the taper should be clamped, but with less force than in "1lock" ( pull force = taper clamp + flange contact) ; thus, there is a specific moment, where the taper gets close to plastic deformation(d*), but it not reaches it, because flange contact appears; d*, the distance until plastic defformation point is always the same, being taken into consideration when such cones are developed

for things to work well, "taper clamp force" / "flange contact force" = specific_value, which means in reality :
... machine clamping force should not increase over time; otherwise, spindle may get deformed, bit by bit, with each clamp
... machine clamping force should not decrease over time; otherwise, there will be only taper contact, and less flange contact
... "2lock" cone craft tolerance is lower than a "1lock", thus shanks provider must be trustfull if you buy '1lock' cones, with different craft tolerances:
...... same angle, but the cone is larger or smaller, machine will always clamp it the same, if you wish at a specific nominal circle : thus, if a smaller '1lock' cone appears, machine will pull it a bit more; also, if a bigger '1lock' cone appears, machine will pull it a bit less ... so, in time, spindle contact surface stays the same
...... different angle, than machine will clamp :
......... near smaller diameter : lower stability when cutting
......... near bigger diameter : same stability when cutting, but spindle gets deformed

so, always buy from same provider, or, verify each cone after purchase !

if a machine works a lot with '1lock', and suddenly a '2 lock' appears, than there is a risk to clamp it more on the flange, and less on the taper because spindle cone has a "bed" where all your '1lock' are sitting ok, but this bed may not be ok for the '2lock' ... '1lock' is not crafted at such tolerances as a '2lock', thus spindle gets different wear/'bed' on 1lock for a long time, comparing to a 2lock for a long time .... in the oppossite, if '2lock' is used a lot, than there should be no worries when going to '1lock'

so, using alternatively 1lock and 2lock will ruine the spindle 2lock requires much more caution

a machine only for '2lock' should not be used for '1lock'
a machine only for finishing should not be used for roughing

if you wish to take this matter in your own hands, than take a spindle that has wear on it, and refresh it, to be like new; craft your own 2 lock cones :
... use materials that are stable over time
... use quality heat treatment
... grinding accuracies to the best ... and you will have your own cones, at least for collets, or face mills; 2lock with hidraulics, shrink fit, etc, are harder to build by normal humans

in my opinion, a 2lock may fail overtime, because taper is long, so you may get to a point where contact is at smaller diameter or at bigger diameter; thus :
... i just find at nikken an alternative with a shorter cone; i guess it costs a lot
... i am waiting for a system that delivers clamping in 2 steps :
...... clamp the taper
...... after, clamp the flange with another mechanism > such a construction is harder to achieve, but will eliminate all disadvanteges that a 2lock has

[ 3lock ] is special : it allows your machine to be more stable at heavy cutting; in my opinion, just use smaller tools, so to avoid all efforts delivered by bigger tools be gentle with the machine smaller rough tools, with many teeth, high rpm, 80..90% normal feed, coolant all over the place

ps : is it a limit when uploading images ? images contain infos, and they have their resolution decreased ; also, i can not upload archives ... why ?

deadlykitten said:

in my opinion, a 2lock may fail overtime ...

Click to expand...

i just find out that somewhere this did happen on machine where were used '2lock' for rough milling ... because of wear, taper contact reduced, and thus, to remediate it, they reduced flange width on all holders nice move ...

Interesting stuff, I didn't know about Lyndex Nikken's different locking methods, I've only ever seen Big Kaiser's system. Thanks for the info!

hello i just discovered the VTPNO [ tool_numer ], which returns the pot that contains the tool " tool_number "

please, when such a variable is needed ? are there some cases ? if not, than i think i will forget it ... kindly !

You can use VTPNO for several uses. One would be to see if a tool exists in the ATC matrix. If VC100 = VTPNO[20] is returned as a zero (0), then that tool is not present in the ATC.

Tskinner said:

You can use VTPNO for several uses. One would be to see if a tool exists in the ATC matrix. If VC100 = VTPNO[20] is returned as a zero (0), then that tool is not present in the ATC

Click to expand...

yup, the tool may be in the pot, but not declared in virtual setup please, is there another reason ?