OSP5000M-G tool offset setup, MC4-VA

[GuntisK]

Hi!
Can someone explain step by step how to correctly do a tool offset settings? Still trying to learn this system, thought it will be easier...
I have only OSP5020M manual in hands, but my machine has OSP5000M-G, so something can be different. Manual says the first thing to do is setting a work zero offset (Y and X, so Z is left for the tool in next step?). After that we should move to the TOOL DATA screen, touch the reference surface with tool tip, press a CAL button, enter current position (0.00mm?), press write. Later call an offset by G15 H1 or other Hxx, tool offset G56 H1 and everything should be fine. I have followed these steps but only the first tool moves correctly to workpiece zero, others not.
Correct me if Im wrong in this, really want to understand whats wrong with my steps.
Guntis

Similar Threads:

• Need Help!- Tool Offset and Work Offset Locking on Fanuc OiMD
• 5 axis machine setup creates weird offset in tool position DMG DMU50v
• Intial Tool Offset setup on 840D
• Fanuc 6M-B Offset setup both work and tool
• part setup Z &tool length offset

[NeoTech]

This is general tip for setting up tools..I do this method but using a siemens controllers equivalent of CAL

1) Set your machine zero Z0, either by touching your spindle tooling contact face (not drive dog) to a measuring block or a height gauge and remove the height of your gauge.
2) Load tool to measure.
3) move machine to XY Zero. Z <whatever clearance your comfortable with>
4) Move tool to a known offset (say 50mm) or using a toolsetter with a known offset (usually 50mm...)
5) Go into tool table, goto tool length hit "CAL 50" - if you follow this method. (This takes the 50mm offset block/gauge into account and subtracts that from the length).
6) Repeat for all other tools.

When it comes to Diameter of a tool there is different ways as well i usually do the "paper" variant against a flat side of the vise.. just hold a strip of paper and slowly jog - a spinning tool (SLOOOW spin) until it rips the paper out of my hand.
Then you know you are a paper thickness away from the vise - and if you set the X zero to the side of your vise you can hit CAL <paperthickness> into your tool diameter.

[broby]

Hi!
Can someone explain step by step how to correctly do a tool offset settings? Still trying to learn this system, thought it will be easier...
I have only OSP5020M manual in hands, but my machine has OSP5000M-G, so something can be different. Manual says the first thing to do is setting a work zero offset (Y and X, so Z is left for the tool in next step?). After that we should move to the TOOL DATA screen, touch the reference surface with tool tip, press a CAL button, enter current position (0.00mm?), press write. Later call an offset by G15 H1 or other Hxx, tool offset G56 H1 and everything should be fine. I have followed these steps but only the first tool moves correctly to workpiece zero, others not.
Correct me if Im wrong in this, really want to understand whats wrong with my steps.
Guntis

Hello Guntis,
First step is to establish your X,Y and Z zero point on your job.
It is easier if you have a probe, but let's assume you don't.
Place a tool in your spindle of a known diameter, say a 10.00mm solid blank.
if you are after precise zero, use a Slip guage and move the tool near the edge of your part, closer than the thickness of your slip guage, and slowly wind away from the surface until the slip guage fits between the edge and the tool blank in your spindle, if you are using, say a 10mm slip block, then you will be 15mm away from the edge.
NEVER wind your tool upto the slip block on X, Y or Z incase you go too far, you will 1. Damage your slip block, 2. Shift your job or 3. Just do something stupid, always move away from the edge until the slip block fits.
Go to the zero set page and select the desired co-ordinate system you are going to use in your program.
For e.g. system 1 (This will be referenced in your program by using G15 H1)
Select the axis you are setting and press CAL 15.0 and then press the "Write" key to get the system to "Calculate" the position as entered.
Do this on X and Y, you can be either + or - just remember to calculate the correct value!
Z Axis is setup the same, but you need to use a tool, or a setting bar if you have it, that represents the Z0 point from the face of your spindle.
i.e. if the tool had a z0 tool length offset and you correctly set Z0 on the top face of your part, entering G0 Z0, without a tool offset command, your tool should reach the same surface.
ALL Tool lengths are set either + or - from your Setting tool, + if longer than the tool and - if shorter than the tool.
Referencing the tool offset in the program is by using G56 Hxxx where xxx is the tool offset number you are using.
To set your tool length, bring the tool up to the Z0 surface and on the tool data page, select the tool offset number you want to use, and then with the tool at the surface, press CAL 0 with the Cursor highlighting the Z position.
To check, simply MDI your tool into a know position, usually away from the surface by a set distance so that if something is off, then you hopefully wont hit the surface... you ARE running slow at this stage aren't you?
Several other things to remember:
1. Always check your active Coordinate system
2. Select the correct corresponding Tool Offset number is highlighted.

In your program you will start with something like this (and more)
G15 H1 (Select Coordinate system)
M6 Txxx (Select Tool and do a Tool Change, there may be more involved on your machine if you have pre-stage tooling or not)
G56 Hyyy Z800 (Move to Z800 activating tool offset for tool yyy)

Hope this information helps you a little, good luck on your journey.
Brian.

[GuntisK]

Wow! :O Thanks for such a detailed explanation. The problem with all Japanese machine manuals is that something is always missed in the description (I've come across this many times). I will try to set up the tools today after returning from work. I hope that this time I will have a positive result.
With regards-
Guntis.

[GuntisK]

I think I managed to do that! One thing I didn't get at first was that before setting each tool, we should call in MDI G56 Hxx (were xx is tool number), prior to setting offset in TOOL DATA for EACH TOOL!!! H1 for T1, H2 for T2, and so on. Only after that I managed to do setting with CAL button by entering distance from Z0 (with red asterix simbol in front of tool number). Also a g-code generation should follow this rule that when doing a tool change we should call individual Z offset for each tool- Txx M6 G56 Hxx. Only in this case each tool tip will be positioned exactly at programmed point. I thought that there is one H offset for all tools, when we are setting a program zeroes. Such approach was something new and unexpected for me (my previous small milling machine control was LinuxCNC, there everything is little different). And such small, at first sight insignificant things were a culprit!
Thanks everyone for help!

[broby]

I think I managed to do that! One thing I didn't get at first was that before setting each tool, we should call in MDI G56 Hxx (were xx is tool number), prior to setting offset in TOOL DATA for EACH TOOL!!! H1 for T1, H2 for T2, and so on. Only after that I managed to do setting with CAL button by entering distance from Z0 (with red asterix simbol in front of tool number). Also a g-code generation should follow this rule that when doing a tool change we should call individual Z offset for each tool- Txx M6 G56 Hxx. Only in this case each tool tip will be positioned exactly at programmed point. I thought that there is one H offset for all tools, when we are setting a program zeroes. Such approach was something new and unexpected for me (my previous small milling machine control was LinuxCNC, there everything is little different). And such small, at first sight insignificant things were a culprit!
Thanks everyone for help!

Hello Guntis,
You should not need to MDI the tool offset command first. You only need to set your coordinate system.
In fact you should find that you would not be able to CAL value without being in manual mode.
Regards
Brian

[Algirdas]

Congratulations! It is a bit aside from what Okuma provides, but it works for you - most important.
Check the table of tool offsets in the tool settings screen. Have you different Z offsets for tools with different lengths?

[GuntisK]

You should not need to MDI the tool offset command first. You only need to set your coordinate system.
In fact you should find that you would not be able to CAL value without being in manual mode.

Yes, but after calling MDI command I move to MANUAL mode, and only then I can set tools using CAL. Too bad a very few words are on tool setiing in manuals- for sure they are not written for dummies. The way how I did this of course looks like a way too much of a movement, but at least it works somehow.

[GuntisK]

Congratulations! It is a bit aside from what Okuma provides, but it works for you - most important.
Check the table of tool offsets in the tool settings screen. Have you different Z offsets for tools with different lengths?

Thanks! On tool offset screen Z offset numbers are indeed different values for different lenghts.
P.S. Is there any dowloadable manual available where is complete description of tool setups mentioned? I have on my hands only Okuma_Manual_1635, but it is for OSP5020M and TOOL DATA SET COMMANDS looks written very condensed.

[deadlykitten]

NEVER wind your tool upto the slip block on X, Y or Z incase you go too far, you will 1. Damage your slip block, 2. Shift your job or 3. Just do something stupid, always move away from the edge until the slip block fits

hy broby intersting point of view, safety 1st i treat most things with care, while also considering them to be mere consumables; kind of "let's take care of this little slip block" vs "do you have another ? or should we really use them"?

ALL Tool lengths are set either + or - from your Setting tool

yup, that's the frequent method, relative type; i use absolute :
... wcs z0 = table lavel; part height will be wcs z
... offset z0 = spindle face

other example, for vice setups, i use a wcs located in the corner of the static jaw, then simply measure with a caliper distances from that point, and modify the reference wcs, to suit the new part; and other things ...

Z Axis is setup the same, but you need to use a tool, or a setting bar if you have it

yes, or possible to eyeball it, cut, measure, input corection, then finish

The problem with all Japanese machine manuals is that something is always missed in the description

i can say that manuals are a bit messy, but even if they wouldn't, it would be hard to understand them at 1st glance

after a time, i simply realized that most information is accurate, even if it is japanoso-anglisky is all about how much one can read between the lines

biggest problem with manuals is that some info is missing, or is being spread across different manuals, and same topic may be explained better in a lathe, or in a mill manual

we should call individual Z offset for each tool - Txx M6 G56 Hxx

later on, Txx Hxx became Txx HA

Is there any dowloadable manual available where is complete description of tool setups mentioned

those guys got you covered on most used aspects of tooling; is there something else you wish to know ?

for example:
... how to avoid tool library
... how to calibate a touch setter and/or renishaw/probe and/or 3d taster
... multiple offsets / tool
... detect broken tools
... spindle attachements : 2 axis, or diy air driven spindles for high rpm
... heavy / large tools
you name it / kindly

[broby]

Yes, but after calling MDI command I move to MANUAL mode, and only then I can set tools using CAL. Too bad a very few words are on tool setiing in manuals- for sure they are not written for dummies. The way how I did this of course looks like a way too much of a movement, but at least it works somehow.

When you change to Manual mode, the machine "Resets", i.e. forgets tool offsets, any Zero Offsets that are not written to memory (i.e. CALculated)
So by "Calling a tool up using MDI" does nothing for you.
Do you have a "Standard Tool"? i.e. The Setting Tools we have on our Machining Centres are a 50mm diameter solid tool that is around 200mm long (from memory).
If I put this tool in the spindle, and touch the end of the tool against the centreline of the table (ours are Horizontal Machines) then CALculated Z0 I would get the machine Zero position of Z-115.95mm as the Zero point.
This WILL BE DIFFERENT on your machine.
The important step is that you need to establish your Z0 point by using what ever method works for you.
If or when you get a Probe, this step will become fast and reliable and very easy... but that is food for another day.
Now, putting any other tool in the spindle and bringing it up to the surface you have just Set as YOUR Z0 point, you just need to go to the Tool Offset page, select the desired offset number, highlight Z and press the CAL button, enter the value you are CALculating and then press the WRITE key.
With your Rapid Override set to ZERO!!!!! select MDI mode and key in "G0 Z0 Hxxx" (where Hxxx is the tool offset you are using) then press WRITE. if your Distance to go shows a value, you have not correctly set your tool length offset, if the distance to go, stays at ZERO, then you are good to go!
Remember, choosing the tool offset number can be any number, but to save yourself a migraine, always use the same number as the tool...
More advanced offset commands such as using G56 Zxxx HA or HB or HC was mentioned in passing by others.
These commands reference the current tool number mounted in the spindle and is a more advanced way of referencing the current tool, rather than referencing a fixed tool offset number.
For now, ignore this, just figure out how to walk first then jog then RUN!
When you get the hang of this, you will wonder why it was so hard to start with
If you have an external mount for your tool, i.e. a BT50 / BT40 taper mounted on a flat surface, you can use a height guage to measure your tool length easily, set the Zero point on the height guage to your Setting Tool end face and then measure your actual tool, the value on the guage is your tool length offset. + if tool is longer, - if tool is shorter.
Hope this helps?
Brian.

[broby]

[QUOTE=deadlykitten;2473182]hy broby intersting point of view, safety 1st i treat most things with care, while also considering them to be mere consumables; kind of "let's take care of this little slip block" vs "do you have another ? or should we really use them"?


Depends on availability of your parts you use for manual setting! If you want to risk the biscuit, well you go girl, smash the crap out of your setting blocks, not me.
Also, why risk any damage or movement to parts etc?
But hey, your machine and parts, do what you want!

[deadlykitten]

hy broby i understand the meticulosity and patience required for your approach; of course, going rough or smooth depends on setup

as for smooth measuring, i use the method described in attached image, when small tools are there, or when i can't use the setter; method's accuracy depends on dial indicator, and it can easy reach <0.01; in comparison to other metods is not only faster, but also accurate using the part as the reference surface, it will go over any errors that are related to probes, as this method is faster than probe calibration, etc

With your Rapid Override set to ZERO!!!!! select MDI mode and key in "G0 Z0 Hxxx" (where Hxxx is the tool offset you are using) then press WRITE. if your Distance to go shows a value, you have not correctly set your tool length offset, if the distance to go, stays at ZERO, then you are good to go!*

checking like this works, yet it requires many keystrokes : G0 Z0 H** enter run; i check within 1 keystroke : after reset, z value has to be equal to tool offset, mill and lathe; also, as for the method of zeroing (before checking), i use less keystrokes, like executing a custom macro : instead of mdi, tool call, spindle, cut, etc, i use manual positioning without mdi statements, program select, run; it works, as being based on system variables, that can snap actual tool position, without that real movement that compensates between a position without offsets, and the same position, but with offsets; i call this a "hoovering trick"

[broby]

hy broby i understand the meticulosity and patience required for your approach; of course, going rough or smooth depends on setup

as for smooth measuring, i use the method described in attached image, when small tools are there, or when i can't use the setter; method's accuracy depends on dial indicator, and it can easy reach <0.01; in comparison to other metods is not only faster, but also accurate using the part as the reference surface, it will go over any errors that are related to probes, as this method is faster than probe calibration, etc



this works, yet it requires many keystrokes : G0 Z0 H...; i check within 1 keystroke : after reset, z value has to be equal to tool offset, mill and lathe

OK, DK you have me intrigued... you say "After Reset, z value has to be equal to tool offset"
How is this possible? you are already in Manual mode, so pressing "Reset" will acheive sod all and change nothing.
On a plus side, the idea of using the dial and flat plate is a good quick way of doing a tool length setup.

[deadlykitten]

hy maybe methods differ a bit between machines, maybe i was unclear, i don't know, but i don't reset while in manual mode; why would i ?

after setting z0 in mdi, actual z on screen will become 0; press reset, then compare z on screen with z tool offset

flat plate is a good quick way of doing a tool length setup

is a trick that i learned from veterans, on classic machines i just added the dial

[broby]

hy maybe methods differ a bit between machines, i don't know, but i don't reset while in manual mode; why would i ?

after setting z0 in mdi, actual z on screen will become 0; press reset, then compare z on screen with z tool offset



is a trick that i learned from veterans, on classic machines i just added the dial

Ah, see you left out being in MDI mode... a small detail at best, but a VERY important step.
But then, CALculating tool length offsets is usually done only in Manual mode.
Can't have a tool length offset in action when CALculating a new length, ADDing can be done any time.

[deadlykitten]

if program 0 was just set in mdi, then reset, and z on screen should be z offset from tool table

if a tool 0 was just set in manual, then, again, z on screen should be z offset from tool table ( no reset this time )

for both, there is no futher check in mdi / is it ok ?

[broby]

But setting your program Z0 in MDI is still adding in Key Strokes.
Doing it from Manual mode with NO artificial change to Z0 and then checking via MDI using the actual tool offset command, as used in the program, would be error proof.
Steps are the same every time.
Set your Z0 point in the desired Coordinate system, then set your tool lengths.
Bearing in mind to that once your tool length offset is set, you don't have to reset this value unless the tool has been changed since setting it.
All you need to do is setup the coordinate system for each job on the table.

[deadlykitten]

hy common steps : manual positioning, maybe facing, zeroing wcs/tool, checking

normally, each step requires to push some buttons, but things can be speed up :
... checking ( described earlier)
... zeroing ( program that replaces keystroke chain for zeroing; being a program, it simply eliminates the need for checking )
... facing ( program that starts cutting regardless of actual machine position, then does zeroing )
... manual positioning ( can be done to detect uneven stock, then triggers facing & zeroing )

i presented those in reverse order, as complexity increases : for example, only for checking there is no program needed ( it can be done visually), while, the last one, that handles uneven stock, requires a few more lines

once the common proof method is no longer used, then is needed to compensate, by :
... a higher level of atention ( you do it faster, but being more alert )
... a proofed code

is not always needed to use such alternatives to replace all steps, as not every setup requires all of them but checking is always recomended, so i simply decided to present an alternative way only for it, as being the simplest and most frequent used

such codes i call 'assitants', and their file names begin with z, so, when someone decides to select a normal program, assistans will always be at the bottom of the list, so to allow the main program to always be at top, visible, easy to select and execute

Bearing in mind to that once your tool length offset is set, you don't have to reset this value unless the tool has been changed since setting it.

or, if it is a rare case, tricked offset. like one that will work only for that setup : for example, there are situations when is not possible to use the atc, but is needed to use a big/large tool; there is no wcs, there is not possible to measure the tool, but zeroing can be done by touching that tool with the part, even if both of them, have no 0; i call this 'floating' setups

just saying, nothing extra fancy in the end / kindly

[Superman]

Brian...
Stop playing with the cat, you know you end up with headaches