Okuma 4020 Tool Offsets :(

[phatfred8]

Hey all,

Friend of mine has a Okuma Cadet 4020 Mill, 1998ish year. Great machine and we are getting used to the control. I had a few parts to run last night and went over to do the work. Aluminum parts that get profiled and a few holes drilled. Wrote the code in Mastercam and posted to the machine with no problems. The problem is when we changed tools and the length offset not working. I looked in the manuals that he has and really did not fine anything that explained this setup.

So first we found the corner of the part and set the machine to zero with G92 on the X and Y. Installed the referance tool or tool #1 and touched off the top of the part. Used G92 to set z zero and then went to the tool page and highlighted tool #1 H Offest and hit "Cal", "0", "Write" which changed the value to zero. We then changed to tool #2 using MDI with M6 T2 and broght that down to the top of the part at the same plane we set zero on tool #1. Then went to the tool offset screen and highlighted tool #2 Offset and hit "Cal", "0", "Write". It then inserted about .640 for an offest value. Which if you where to measure the tools from the spindle, tool #2 was longer than tool #1.

When we ran the program and the tool changed to Tool #2 the tool would not take into account for the offest amount. The M6 T2 was followed by a line of code that enabled the H2 tool offest and then a "Z" command to rapid down to. We tried different numbers with no luck. Finnally gave up and decided to just profile the parts and put the holes in later with bridgeport.

Is the above the correct procedure or are we doing something wrong? I have programmed other equipemnt in the pass but this has us stumped.

THanks in advance,

Brian

Similar Threads:

• Need Help!- ERROR CODES MANUALS OKUMA MCV 4020
• Need Help!- Okuma Cadet 4020 VMC with OSM5020M Control
• Need Help!- Okuma 4020 Alarm
• Can Okuma vmc 4020 load program from diskette?
• Compressor Required for Okuma 4020

[Superman]

It is a little bit dangerous this method, as your reference tool must always be in the machine, and cannot be altered for this job. If you do alter this tool, then all the other tools would have to be re-length gauged.
-you could have a dedicated tool assembled ( say a 1" dowel in a collet chuck) ( no need to store it in the machine ) that is used to set the G92 Z-datum ( have you tried using G15 --- see lower down )

The value stored in the tool lengths is the difference in length, relative to the reference tool, if you get a +ive value, then that tool is longer than the reftool by that amount.

G56 (ammended) is the code used to call in the tool length value and subtract it from all Z co-ordinates in the NC code. ie a -ive H value would make the spindle head travel further than the reference tool length

Major issues with all programs is:-
- wrong D & H numbers defined in the program ( don't match the T# ) ( this can depend upon shop procedures )
- that a wrong length was put in for that tool

Mastercam could have:-
- the wrong WCS and / or T/C planes selected for those operations
- check to make sure that D & H #'s match the T# in the Mcam operations

G15
usage:- G15 H1
this calls up the work offsets that is set and stored, external to the program, it replaces the entire G92 XYZABC line.
-it is like you defining a point in space, giving it a ID number, and your program calls up this ID point as your work origin. ( no editing of the NC file is needed ) ( access is on the Work Offset page- you should have 20 offsets available---H0 is the machine's co-ordinate system )

ADDED NOTE
The H value on the G15 line is not from the same data page as the one used on the tool length take-up line, they are 2 seperate catagories

UWP_Wes----I think you had better amend your G54 to G56 as well !!

[UWP_Wes]

G43 does not work with Okuma.

Tool length offset is done with G54. You use G54 H1 for tool one, G54 H2 for tool two, etc.

G15 H1 is the fixture offset.

To set the tools:
MDI type in "G15 H0" this will clear the offsets.
Load your tool up.
Jog it down to a gauge block on the table and touch it off.
Go to the tool page and find your offsets.
Page to the length offset for the tool you want and hit "cal".
Then using "add" subtract the length of your gauge block.


Do that for all the tools.

To set the G15 H1:
Use one of the tools and touch off to the work piece.
Go to the Zero Set page and highlight Z for position one.
Hit "cal".
Then using "add", subtract the length of the gauge block and the length of the tool (the offset length in the tool page).

I use a tool that is exactly 5" to make it easy.

The manual is pretty fuzzy on all this.

[DouglasR]

I avoid G92/G50 commands at all costs. Incredibly risky way to set it up. UWP is correct and his method is far safer.

[phatfred8]

I will have to give the method above a try later next week. With the holiday weekend I will not be running any parts. I will agree that the books with the machine are very fuzzy on this subject.
The one shop that I worked at the machinist always set tools off the table surface and a gage block. Hopefully the G56 will make the tool offset work.

I will let you guys and thanks for hte help.

Brian

[broby]

G43 does not work with Okuma.

Tool length offset is done with G54. You use G54 H1 for tool one, G54 H2 for tool two, etc.

G15 H1 is the fixture offset.

To set the tools:
MDI type in "G15 H0" this will clear the offsets.
Load your tool up.
Jog it down to a gauge block on the table and touch it off.
Go to the tool page and find your offsets.
Page to the length offset for the tool you want and hit "cal".
Then using "add" subtract the length of your gauge block.


Do that for all the tools.

To set the G15 H1:
Use one of the tools and touch off to the work piece.
Go to the Zero Set page and highlight Z for position one.
Hit "cal".
Then using "add", subtract the length of the gauge block and the length of the tool (the offset length in the tool page).

I use a tool that is exactly 5" to make it easy.

The manual is pretty fuzzy on all this.

G43 -> Well it does work, but it is defined as 3D Compensation Cancel... so I guess it is used with 3D milling?

G54 Hx is INCORRECT!!!! You MUST use G56 Hx!!!

You can also use G56 HA and the machine will automatically pickup the tool length offset for the tool in the spindle. HA is defined as the first offset used by the tool, HB is the second offset and HC is the third.
DA is the first offset (main one) used when programming cutter radius compensation programming, DB is the second offset and DC is the third.

Typing in G15 H0 WILL NOT CLEAR YOUR OFFSETS!! What it does is make the machine select the machines base co-ordinate system.

The info on setting a tool length is good tho...

Cheers
Brian.

[littlerob]

So PhatFred, (funny I have a friend named Fredfern. no joke) We like to hear the outcome of what happened, did you get everything sorted out?

Robert

[phatfred8]

Hey all,

This week has been busy with fabrication work at the house, main part of the eveing business. I am planning to head over to my buddy's next week and work out the code and try what was sugested above. I will definetly let you know the out come.

I do have another question. When we go to start the program and have the first tool loaded in the spindle the machine give us a error saying some thing like the tool does not match. Even though the T1 is loaded in the spindle and it is calling for T1. This is not a problem if at the end of the program you change tools to something different than the starting tool. Not a big deal if you are using more that one tool but if you are only using one tool than that will waste a lot of time changing tools and stuff. Next week I am there I will get the exact error code and post it here.

Thanks for the help,

Brian

[broby]

Hi Brian,
If your machine is anything like our horizontals, you should be starting your program with no tool in the spindle at all.
The start of the program should call up the first tool T6
Then M6 to put this tool into the spindle.
Then call up (pre-stage) your next tool using T7
.
.
.
Program for T6 actions goes here
.
.
.
When finished with T6 program an M6 to change to the "Pre-Staged" tool (T7 in this example)
If no more tools are then required, program an M63 to tell the machine that there is "No Next Tool".
.
.
.
Code for T7 use goes here
.
.
.
Program another M6 when done with Tool 7 and that will return T7 back to the magazine.
Job is now done and no tool is in the spindle.

e.g.

N1 T6 (pre-select Tool 6)
N2 M6 (Tool Change T6 moves into Spindle)
N3 T7 (pre-stage Tool 7)
N4 G15 H1 (Select/Activate co-ordinate system number 1)
N5 G0 G56 H6 Z800 (Move at Rapid, activating tool length compensation for Tool 6 to Z800)
N6 .
N7 ... Program for Tool 6
N8 .
N9 M6 (Tool change command, T6 (spindle) exchanged for T7 in the Sub Pot, T6 returned to magazine)
N10 M63 (Command to tell machine that there no more tools required)
N11 G0 G56 H7 Z800 (Move at Rapid, activating tool length compensation for Tool 7 to Z800)
N12 .
N13 ... Program for Tool 7
N14 .
N15 M6 (Tool change command, T7 removed from Spindle and returned to magazine)
N16 M2 (Program End)

Note that if you do not use M63 to tell the machine there are no more tools required, you will get an alarm stating "No next tool".
Hope this helps
Regards
Brian.

[OkumaWiz]

To eliminate several of the errors/alarms you will typically get on your Okuma M/C's we use the following program. It checks the current status of your tool in the spindle/pot and makes logical decisions based on what you are trying to do.

Main programming difference is that we use G111 T6 Q7 to call tool 6 and prep tool 7. G111 is a user defined G code and "calls" OTCHK. We nomally register this as a LIBRARY program(such as OTSET.LIB) so that it remains memory resident.


OTCHK
( SET GCODE PARAM. G111 TO OTCHK )
( AT TOOL CHANGE KEY IN G111 T= TOOL NO. Q = NEXT TOOL EX: G111 T1 Q2)
IF [ VTLCN EQ PT ]NST1 (ACTIVE TOOL)
IF [ VTLNN EQ PT ]NRT1 (NEXT TOOL)
IF [ VTLNN EQ 0 ]NOT1 (NEXT TOOL)
M64
NOT1 T=PT
NRT1 M06
NST1
IF [ PQ EQ EMPTY ]NEND (IF READY TOOL EMPTY/JUMP )
IF [ VTLNN EQ PQ ]NEND (IF PREP TOOL IS AT NEXT TOOL POS./JUMP)
IF [ VTLNN EQ 0 ]NTT1 (IF NEXT TOOL HAS NO VALUE)
M64 (NEXT TOOL POT RETURN)
NTT1
T=PQ
M356 (NEXT POT ADVANCE)
NEND G56 H=VTLCN
D=VTLCN
RTS
PQ DEF: WHEN P IS ATTACHED TO A LETTER IT BECOMES READABLE


Hope this helps you as much as it helps us!

Best regards,


[budgieW]

Or just use this format

G00 G17 G21 G40 G80 G90
G30 P32
IF [VTLCN EQ 7] N1 (SPINDLE TOOL CHECK)
T7 (16MM TIPS - TOOL 7)
M6
N1 (SPINDLE TOOL JUMP)
S9500 M03
G15 H1
M11
G00 G90 X49.866 Y1.065 A15. M15
M10
G56 H=VTLCN Z100.

[broby]

I must admit to failing to understand the need for these macros, as a programmer, YOU are setting up the order of tools and when they are called up in the program.
Having a macro check the state of what tool is in the spindle and what tool is next is rather a waste of time because YOU are controlling that in the program, if you do not know what tool is where then you have a major problem!
Operators should be trained to recognise what tool is in the spindle by checking the information on the tool data page. There will be a screen showing you what tool number the machine has in the spindle and what tool number is in the sub pot.
But then again, maybe things are very different where you are?
Maybe I am missing something?
Regards
Brian.

[OkumaWiz]

I must admit to failing to understand the need for these macros, as a programmer, YOU are setting up the order of tools and when they are called up in the program.
Having a macro check the state of what tool is in the spindle and what tool is next is rather a waste of time because YOU are controlling that in the program, if you do not know what tool is where then you have a major problem!
Operators should be trained to recognise what tool is in the spindle by checking the information on the tool data page. There will be a screen showing you what tool number the machine has in the spindle and what tool number is in the sub pot.
But then again, maybe things are very different where you are?
Maybe I am missing something?
Regards
Brian.

You are missing something...

Invariably tools break as you are running the part and cycles get interrupted for various reasons. This throws off your sequence of events that as a programmer you have perfectly planned. Now you need to restart either from the beginning or at some point in the cycle. Without the macro, you will be treated to LOTS of alarms. With the macro, you will be blissfully content with the machine doing just what you'd expect without any annoying tool change alarms.

Saves mucho time and irritation.

Best regards,

[broby]

So basically speaking, what you are saying is that your operators do not know how to pick out the correct line number or sequence to restart on...?
That totally smacks of poor training to me.
All the apprentices (and new tradesmen) that are trained on both the Okuma Lathes and Okuma Mills in our workshop are trained to recognize where and how to restart a program and if they have a problem they actually ask! How's that for a concept?
If an operator has the skills to restart a program, for what ever reason, and they can not recognize if they have done so correctly, then why the hell are they being allowed to perform a restart???
Cheers
Brian.

[OkumaWiz]

So basically speaking, what you are saying is that your operators do not know how to pick out the correct line number or sequence to restart on...?
That totally smacks of poor training to me.
All the apprentices (and new tradesmen) that are trained on both the Okuma Lathes and Okuma Mills in our workshop are trained to recognize where and how to restart a program and if they have a problem they actually ask! How's that for a concept?
If an operator has the skills to restart a program, for what ever reason, and they can not recognize if they have done so correctly, then why the hell are they being allowed to perform a restart???
Cheers
Brian.

You are still missing something...

The operators know how to restart fine, but in the middle of an interrupted cycle, the Okuma control knows that for example tool 5 is prepped and tool 4 is in the spindle, but when the restart occurs, you will get alarms when it attempts to change to tool 1 and prep tool 2, or when it sees the same tool already in the spindle or the same/wrong tool prepped.

If you use the macro I supplied (which in my opinion should be in standard software) you will not get any of the alarms or have the potential for an operator to make a mistake by "fighting" with machine alarms.

It is MUCH faster to have the machine tool changer automatically put back the wrongly prepped tool, change to the correct tool and then prep the correct one automatically without all the operator intervention and potential alarms.

The Macro takes care of all these issues and "fixes" what this post is all about.

Best regards...try it you'll LIKE it!

[broby]

Well, I beg to disagree, from the point of view that we DO NOT have restart errors 99.9% of the time, as there are easily identifiable restart points in our programs, stuff that was taught to us by Okuma Australia many many years ago.
Correct programming practice and operator training overcomes your obvious problem with restarts...
Tool errors at restart do not seem to be an issue for us, maybe there is a difference in the way you and I program...?
Cheers
Brian.

[Superman]

I think I'll side with Brian on this one. but I can also see Wiz's line of thought. We do have machines that use a custom G/M-code for toolchanging

Any error you get WILL occur when you restart on either the toolchange line or prep-tool line ( depending on the control ).

These T-code events have already occured, so why restart back at the toolchange point. Normally you would restart at a retract plane, just above the interupted position. I advise our newer operators to never restart at a cutting point on the job, too many things can occur, the experienced guys have already learnt this and do it without a 2nd thought. But there are times where a restart is required mid cut, this operation is approached with caution.

[littlerob]

I personally will side with OkumaWiz. Although I hate the stupid macro, I find myself being grateful it is there. But maybe Broby and Superman are right maybe I am programming wrong. I'll have to re-evaluate my process, it has been so long doing it one way that, that is what it is.


Robert

[OkumaWiz]

Well, I beg to disagree, from the point of view that we DO NOT have restart errors 99.9% of the time, as there are easily identifiable restart points in our programs, stuff that was taught to us by Okuma Australia many many years ago.
Correct programming practice and operator training overcomes your obvious problem with restarts...
Tool errors at restart do not seem to be an issue for us, maybe there is a difference in the way you and I program...?
Cheers
Brian.

There is a definite difference in the way we program. I use the macro and have no problems. Restarts or otherwise. Why are you so convinced that we're having problems when you are the one admitting to having to create special restart points and having special training in order to ensure that your operators "do it right"?

I'm just here to help this guy out, not argue.

Brian, do me a favor, you are a decent guy and offer lots of good suggestions on here. Try the macro I posted and then try to get the tool changer to mess up. You'll be hard pressed to make it happen.

That's the only reason I posted it. It works well. It's simple. G111 T6 Q7. Done.

No worries, no restart errors no special training.

I'm not forcing anyone to use it, but I know if they do they will be much faster getting the job done since they will have less errors and they will be very satisfied with the way it works.

Yes, if you have years of programs that you would need to change you may not want to change to use this style, but that is up to the individual. I highly suggest using this for the "newbie" that is having these types of problems. (way back when I think that is what this post is about... sorry for the hijack phatfred8!)

Phatfred8 is going to do whatever he wants, right?

C'mon Brian...try it - you like it!

Best regards,

New alias: Sam I am...

[broby]

I have NEVER said that you are having problems! have I? Each to their own I say. If it works for you and you are OK with it, well then go for it!
I can see some of the benefits of your macro and one day will give it a go with out a doubt.
BTW, I do not program in "special" restart points in my programs, it is just that the operators know the programming format that we follow, thus they can pick up the restart line very easily.
Just had a quick peek, there are something like 8500 files that would need to be updated to use this macro, should we decide that this would be the way to go. Even at an average of 10 tools per program that is one crap-load of editing to undertake... no thank you!
Not to mention error checking to make sure no tool changes are mucked up.
I would agree that at the start up, this macro would be interesting way to go, but not now after all this time.

So... what was the original question asked in this thread again???
Cheers
Brian.