We use the G111 macro, but regular old M6 still works as well.
This seems like one of those screw ups that Okuma calls "features".
Why can't M6 have the macro built in? Our Mori Seiki is set up that way. It will never alarm out if you call the tool that is already in the spindle.
Don't get me started on M53 and M54 in a canned cycle. Why no G98 and G99 like the rest of the world?
I do like the way that Okuma does program restarts though.
helical bore
Can any body help with this problem? I am having trouble with helical bore cycles on an Okuma Cadet Mate VMC it constantly alarms out. I am using Mastercam X5 for programming. It also alarms sometime if I use cutter comp. I don't have this problem with any other control.
You are missing a lot of info to diagnose your problemOriginally Posted by billm01830
What are the alarms codes ( alarm # & full description ) ?
What control on the machine ?
Sample of code ?
Is NC code manually written or from CAD system ?
What values are placed in the D offsets ?
Okuma's do not like to take up comp on arcs, it must be on a line lenght greater than the value placed in the D-offset, it has to have space to be able to take up the comp
The control is OSP700M I am using Master Cam to write the code, with a Post modified for the Okuma. Most of the time we start with no cuttercomp value, we use it to tweek in the dim that need it. So usually .001 to .005 when needed. We did change the prammeter to allow for short cutter comp lines and have not had time to try it with this change. On the Helix bore cycle it starts with no cutter comp nad turns it on only for the finish cut. But it wont even do the roughing without a circle alarm I don't have the alarm number now I will write it down the next time it happens. Maby this is enough info for you.
Thanks for your help
Sincerely
Bill Middleton
What is the G111 Macro and exactly what does it do. And were do I find it.
G111 is a user written macro.
It can be anything and do anything that you desire... the possibilities are endless!
It is linked to a library file that has been written by the user for a particular task that they wish to reduce their programming.
A G111 on one machine will be totally different to G111 on any other given machine.
As for where you find it... On the parameter screen (for Okuma mills) look for the G/M Code macros screen.
This screen is where you link a particular code to the required subroutine.
You also need to 'register' the subroutine as a Library file so that the system will know what code to call when the C/M code is called.
It may have already been stated, but in case not... I saw okumawiz answer to put in a macro, but for the question of restarting when the tool call is the same as the tool that is in the spindle, that is simply something that can be changed in the machine parameters.
I recall running into this setting up programs years back. Program was set to return up the program with appropriate input. Afterwards, new cycle start would pull the same tool existing. At that time i put in a conditional to jump that part when tool was already there.
Anyhow, having my own okuma, I've had the chioce to learn more of her secrets, only to find that was a simple fix by changing a parameterAlso, if this friend's machine did not come with about a 6" tall stack of books, he was shorted on that.
As for coordinating tool offsets, get a z height preset gage. Saves time. Set aside one coordinate offset for presetting tools too.
Also, when setting up on a part, setting the z, you will need to pull up the tool offset, G56H(tool#), then can use G92Z0, or whatever height you are at, or if in the zero offset page, you can NOT just simply highlight the Z spot and use (cal) as that will set to machine numbers. I expect that is the good thing about the G92 on the Okuma. Some other controls I've used, the G92 is a completely seperate coordinate, but on Okuma it changes the active coordinate offsets.
DO ALWAYS remember that on the okuma, setting the tool length offset IS DEPENDENT on the active coordinate, why I suggested to set aside a coordinate for that, and a specific touch point. Good part of that is, if putting in a new tool for current operation, you can preset the tool to a known point on the part.
Just to add to what broby said.... Maybe not all are the same, but what I have seen, you have user defined macros... G101-G110 are "MODIN" macros and are cancelled by G100. G111-G120 are one-shot macros.
Calling up any of these, the user is able to pass-on arguments (data). Say that your G111 is your own preference of a circle pocket. Say you have:
G111 X0 Y0 R.1 Z-1 I1.5 F10
The data is passed on in these address which must be recalled as P(address).
Say you named it OG111.LIB, which you will define it as OG111 in the macros.
OG111
N1 PTR=VTOFD[VDCOD]
N2 G0 X=PX Y=PY
N3 G0 Z=PR
N4 G1 Z=PZ F=[PF*.1]
N5 G91 G41 G1 X=[-1*PTR] F=PF
N6 G3 X=[PI+PTR] I=[[PI+PTR]/2]
N7 G3 I=[-1*PI]
N8 G3 X=[-1*[PI+PTR]] I=[-1*[[PI+PTR]/2]]
N9 G40 G1 X=PTR
N10 G90 G0 Z=PR
RTS
N1 set tool radius data in TR, as long as your tool data is still set by radius, not diameter
N2 rapid to XY position
N3 Z rapid to reference point
N4 plunge Z at 10% F
N5 Changes to incremental, Comp left On, line -X to tool radius, no actual movement
N6 arc CCW, X to I + TR
N7 full circle at radius I
N8 back to center - TR
N9 comp off, line to center
N10 back to absolute dimensioning, Z rapid back up to R point
That was just a sample.
You can use a huge number addresses to pass on or use in the program. The different addresses can be any arrangement of up to 3 characters, letters or numbers, and can be retrieved with (P) in front. Except you can not use G, M, N, or O. To pass into macros, it is just the address character, as was seen in this line:
G111 X0 Y0 R.1 Z-1 I1.5 F10
***edited*** I almost forgot to add... if you pass-on addresses more that one charater into a macro, use brackets like so, [RR]=1.234
but to use the addresses in a program, they must have (P) in front, as the PTR in line N1 set TR to tool radius. or it could have been PA, PAR, PBD4,...etc....
Also, in line N1, these machine variables....
VTOFD[xx] is the tool radius data for xx tool in the tool table,
VTOFD[1] gets tool radius data for tool 1
VDCOD is the active D code... so
VTOFD[VDCOD] gets tool radius data for the tool number of the active D code
Anyway, I'm long-winded. As broby said, possibilities are endless. I love the macros. I use the hell out of conditionals, user variables, machine variables and math in the program line. You know, all the wonderful exciting stuff you can not do with cam software, which is why I do not own any. I don't want to make the machine go, I want to program the thing. I also have a most excellent circle pocket macro I need to get finished soon. Uses every letter of the alphabet for pass-on arguments, excect the few invalids. You can set entry type, plunge or helical, set finish pass in x and y, and z. Set stepover, z step, and set helical step. Or can spiral down and out, spirals back in to center. Just a few extras that okumas circle pockets dont do. A lot actually. I need to get it finished, fully tested and share it
We are making parts
Hello All,
Thanks for all the help so far. We are making some parts and geting the tools changes down pat. I have the length figured out and from the looks of what everyone is saying there are a few different ways to skin the cat. I will not go there now but I will look back in the near future to look at different options.
I have a program to write where I need to add a second vice and repeat the program over. I have looked in the book but can I move the machine via the Machine Coordinates? I remember with one brand years ago I could use a G98 X Y and move machine Coordinates then use a G92 to reset zero. I guess what I would like to do is write a program and then move from one 0,0 to the next and then reset 0,0 to the other vice corner and repeat the program. I am not that familar with work coordinate or how to set or change them on this machine, any help would be great. I know some machines have a G56-59 for different ones. Not Sure on this machine. Books are not the easiest to understand.
If you need more info from me please ask.
Thanks,
Brian
Often different ways to do things. To answer the question of changing offsets, it is simply G15 Hxx where xx is the coordinate system number.
You can make out the whole deal in the program, you can use conditional branching, or you can use MODIN.
Also, always be sure to return back to original coordinate. I know some machines that will come back to the common or main coordinate system once you exit the run mode.
Assume vice 1 on coordinate 1 and 2 on 2. Set your zeros to each vice. you can make it all out as follows.
OPART
G15H1
...... (programmed geometry)
G15H2
...... (programmed geometry)
G15H1
....... (end movement)
M2
Conditional branching....
OPART
VC1=0
N1 VC1=VC1+1
G15H=VC1
...... (programmed geometry)
IF [VC1 EQ 1] N1
G15H1
....... (end movement)
M2
Line N1 will set VC1 to 1 and then 2, which will set G15H= accordingly. The conditional will return to N1 if VC1 = 1, or pass on if not.
Using MODIN
OPART
G15H1
MODIN OSUB
X0Y0
G15H2
X0Y0
MODOUT
G15H1
....... (end movement)
M2
OSUB
...... (programmed geometry)
RTS
annoying,
I follow on the G15Hxx part. You may have to give a few months to get into the conditional jumping. I have done alot of that with Fanuc robots but not with milling equipment.
Hopefully I do not sound to far off but would I activate the coordinate systesm, MDI G15 H1 and then use a G92 to set zero or is this part of the tool page or Parameter Page? I will have to head to the machine to look into this more later this weekend.
Am I thinking right? Happy holidays
Thanks, Brian
I expect it could be done that way, but, do you not have a "zero set" button up top next to the "tool set"?? First go into MDI to select the coordinate. Then back to manual and pick up your edge. say you are using a .200" diameter edge finder, and you are picking up the Y topside, highlight the Y for the coordinate you are setting and input "cal" and ".1" "write". Your position should be displayed below all the coordinate numbers and Y should be .1.
Also, if all your tool lengths are calibrated, you can touch of the top of your part. Say you have tool 1 in. Go into MDI and enter G56H1, write, cycle start. Then go to the "zero set" page, go to the coordinate Z and "ADD" the value displayed below in the Z actual position, which should then become 0.
annoying,
Yes the Zero button is on the top row of keys. So, the work coordinate system can also have different "z" heights, correct? Each of these can be set thru the zero page also. So, I would be bascially no longer using the G92 to set x,y,z zero? I would then need to make sure that I call up the proper G15Hxx of the vise I am working on.
I currently would set the "z" zero with the first tool, which would also then set its tool lenght to 0.00. I would then M6TX for each tool and touch off the top of the part with a 1" gauge block. I would then go to that tool number in the tool page and hit cal, write and then add a -1.0 for my gauge block. It works, maybe not the way I should be doing it but it works.
Thanks,
Brian
Hi Brian,
It seems like you are getting a bit confused over the use of G92, G15 and Tool length offsets.
Whilst you can use G92 on an Okuma mill to reset a coordinate system there is NO NEED to use this code at all!
You only need to use the G15 Hxx command where Hxx represents the coordinate system you have set for the part position desired.
So if you use multiple vices for the same job, or even different jobs, select a different coordinate system for each job/operation. i.e. if you have two vices, coordinate system H10 could represent the X0 Y0 Z0 position of this part, H20 could represent the X0 Y0 Z0 position for the 2nd part.
In the program for the first part use G15 H10 and your program will pick up from the Zeroset page the location of the part.
Use G15 H20 for the second program.
Now for your tool offsets... Your tool offsets should not be set differently for each job, they should be set relative to the length of the "Zero" tool. I use a fixed length solid Zeroset tool that is a non machining tool, that way there is consistency in setting the Z0 position for each program.
If you use a "cutting" tool as a "Zeroset" tool and that tool wears, your relative position of Z0 will vary. If you are chasing tight tolerances this might well become a massive problem.
As all tool lengths are referred back to the length of the Solid Tool set bar you get consistency across every coordinate system used.
Obviously if you have a probe, that is much quicker to set up a coordinate system than by using a solid zero set tool, but not everyone has that item
This way if you have a facing tool that is machining a face to Z0 in both parts, it does not matter what height the Z0 surface is for each part, the tool will still go to the correct height in each program, providing you have set the Zeroset page values correctly.
Hope this helps???
Regards
Brian.
Gentleman,
I was up there on Monday and was able to get the work coordinates for each vise set and able to make the program switch between the two. Works really good. I used Mastercam to generate the code for the (2) steps that needed to be machined. Told it to use cutter comp and the code that it wrote is just a alot of wasted time, comping in and out each pass. Next thing was the facemill we where going to use would not reach the full depth due to machine travel limits. We switched to a different inserted face mill but it is a crappy cutter. Have a new inserted end mill on order. I am also thinking of getting rid of the cutter comp part and just program it based on the center of the tool. The part is not that exact nor does it matter. I will keep working on it. Thanks for the help,
Brian
Well done Brian. Onwards and Upwards for you now!
As for the "wasted" time with the compensation, hey at the end of the day, if the part accuracy is not that critical, well why bother?
As you stated, moving to a program that is based on the centreline of the cutter will be much quicker for you.
Cheers
Brian.
Re: Okuma 4020 Tool Offsets :(
I hate to revive an old thread but im trying to get my okuma tool length's setup and nothing is working correctly how does one go about setting tool lengths in the OSP u10m
Re: Okuma 4020 Tool Offsets :(
Call up fixture offset using G15 H1
Then move tool to known surface and in offset mode use CAL and enter known value of touched surface. Offset will be entered.
Confirm by entering G56 H1 (or what ever tool you just touched off) and send tool to .1 above the surface you just calculated. It should stop .1 above the part.
Best regards,
Experience is what you get just after you needed it.
Re: Okuma 4020 Tool Offsets :(
ok so thanks for posting on that thread but it didnt really help at all. What i'm trying to avoid with my okuma is having to set each tool individually for each seperate part. I was hoping I could set them all of the table then use the work offset Z to set the height and only have to touch off one tool for each indivual part. what I tried doing it
go to mdi and set G15 H00
touch of every tool on table and CAL in the tool offset page
Then to set the G15 H01
touch of 1 tool on the top of the part and subtract the tool length from the Z work offset
does this sound familar at all? It's just so time consuming to have to touch off every tool every time
Re: Okuma 4020 Tool Offsets :(
hi zgc
i don't have a machine like yours, but you may need to use H [ argument <> 0 ]G15 H00
H0 is pointless, or it may mean something pretty strange, like a number hanging in there, relative to encoder origin
just like mr Wizard said, use g15h1 so to declare program origin ( part face, relative to table face )
after that, recall g15h1, so to check that everything is ok, and bring in another tool, close to part face ( use a setter, etc ), then go to tool offset page and use call ( this will input tool offset, relative to spindle line probably )
when you use both g15h0 & g15h1, you simply make things worse
so far so good, but for all these to work, you need to declare g15h1 by using a calibrated tool, otherwise, you will be spining in circles for the infinity ( you will be shifting z offset origin point ) / kindly
we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...
Reply with Quote
