Quick Q about OMP40 stylist change

One of the guys broke the stylist on the Okuma M560 with a OMP-40 part probe. Changed the probe and set the run out with a tenths indicator and used a ring gauge now ready to set the new Z off set. Its a OSP 300 control with the Renishaw App. The question is do we just bring the stylist over the tool probe and and run the set Z off set routine with in the app? That's the way I've done it on other machines just want to check to be sure there isn't something different with Okuma's setup.

TIA

If you have a laser tool setter then this will work as well as your level of calibration, if you have a touch setter, then no, you will not get accurate results. You will need to calibrate to a known length (calibration tool).

No it has a touch sensor. I do have a master tool with recorded length and can use that to measure the probes length difference with a dial indicator, then do I just record that length in the tool offset length.

I have been scouring all the renishaw documentation but nothing specific about where the results are recorded I'll try editing the tool probe Z off set and give it a shot.

If anyone has written instructions I would love to see it.

Captdave said:

One of the guys broke the stylist on the Okuma M560 with a OMP-40 part probe. Changed the probe and set the run out with a tenths indicator and used a ring gauge now ready to set the new Z off set. Its a OSP 300 control with the Renishaw App. The question is do we just bring the stylist over the tool probe and and run the set Z off set routine with in the app? That's the way I've done it on other machines just want to check to be sure there isn't something different with Okuma's setup.

TIA

Click to expand...

No laser tool setter (you do not know really where the lowest styli point is in XY coordinates), neither electromechanical tool setter (spring loaded OMP40 against spring loaded TS) will give you accurate calibration result. in any case you will have to run both the XY and the length calibration procedures included in Okuma's OSP.

Captdave said:

No it has a touch sensor. I do have a master tool with recorded length and can use that to measure the probes length difference with a dial indicator, then do I just record that length in the tool offset length.

I have been scouring all the renishaw documentation but nothing specific about where the results are recorded I'll try editing the tool probe Z off set and give it a shot.

If anyone has written instructions I would love to see it.

Click to expand...

Easy to do if you have a tool with a known/calibrated length.

Put your calibrated tool in the spindle, and bring it to your surface you will use for calibration. I usually use the same 2" ring gage I am using for calibrating the X&Y. If your machine Z distance is Z-14.7900", and your tool length is 3.6307", than your surface to gage line value is -18.4207"

Knowing that, you can now run the 9801 cycle. I make a little program like this:

%
O186 (Z LENGTH CALIBRATION)
(START PROGRAM WITH Z AT HOME POSITION)
(SET G55 Z TO 0.)
G90 G55 X0 Y0 (CENTER OVER AREA TO PROBE)
M59 (PROBE ORIENTATION USE M58 TO CANCEL)
G43H151G0 Z-18.2207 (SET Z APPROX .200 ABOVE KNOWN Z POSITION)
G65P9801T151Z-18.4207 (CALLS CALIBRATION PROGRAM)
(USES Z GAGE LINE VALUE)
M58 (CANCELS PROBE ORIENTATION)
M30
%

After running this you will see that your tool length offset was properly adjusted.

I didn't include 9810 in the program above because it's just what I use when I am calibrating probes, if you are unfamiliar with the calibration cycles, use single block and/or use 9810 for all movements external to the macro call.

Dave Cross said:

Easy to do if you have a tool with a known/calibrated length.

Put your calibrated tool in the spindle, and bring it to your surface you will use for calibration. I usually use the same 2" ring gage I am using for calibrating the X&Y. If your machine Z distance is Z-14.7900", and your tool length is 3.6307", than your surface to gage line value is -18.4207"

Knowing that, you can now run the 9801 cycle. I make a little program like this:

%
O186 (Z LENGTH CALIBRATION)
(START PROGRAM WITH Z AT HOME POSITION)
(SET G55 Z TO 0.)
G90 G55 X0 Y0 (CENTER OVER AREA TO PROBE)
M59 (PROBE ORIENTATION USE M58 TO CANCEL)
G43H151G0 Z-18.2207 (SET Z APPROX .200 ABOVE KNOWN Z POSITION)
G65P9801T151Z-18.4207 (CALLS CALIBRATION PROGRAM)
(USES Z GAGE LINE VALUE)
M58 (CANCELS PROBE ORIENTATION)
M30
%

After running this you will see that your tool length offset was properly adjusted.

I didn't include 9810 in the program above because it's just what I use when I am calibrating probes, if you are unfamiliar with the calibration cycles, use single block and/or use 9810 for all movements external to the macro call.

Click to expand...

Dave,
This is calibration routine of Inspection Plus for Fanuc.
Captdave is working with Okuma's OSP300 with it's own cycles.

I care less about the probe measuring the table correctly, I just want the tools that I measure on the machine to match the probe length, i.e. probe a part, program to cut 0.0050 from part surface, and be exactly there.

I measure a sharp end mill on the tool length probe (2 times to make sure it's consistent) then mill a flat on a scrap piece of aluminum I've clamped in a vise. Set the work piece offset by teaching the freshly milled surface to be 'Z 0'. Now MANUALLY probe the fresh surface and adjust the 'probe length' so the measured Z surface exactly matches the offset determined with the end mill. Now you can probe a part and remove exactly what you intended to. Non of my work is placed on the mill table to be finished, which is the only reason to match probe lengths to spindle gage line height.

PROBE said:

Dave,
This is calibration routine of Inspection Plus for Fanuc.
Captdave is working with Okuma's OSP300 with it's own cycles.

Click to expand...

I didn't see how we know if he is using regular Renishaw macro's or the osp flavor, but he did suggest he was looking through Renishaw documentation. Or is there some reason that on OSP control they don't use regular Renishaw macros? I know on Mazatrol controls you use either the Mazatrol macro's or the Renishaw macros, and it is important to differentiate between the two, particularly when calibrating.

Red James said:

I care less about the probe measuring the table correctly, I just want the tools that I measure on the machine to match the probe length, i.e. probe a part, program to cut 0.0050 from part surface, and be exactly there.

I measure a sharp end mill on the tool length probe (2 times to make sure it's consistent) then mill a flat on a scrap piece of aluminum I've clamped in a vise. Set the work piece offset by teaching the freshly milled surface to be 'Z 0'. Now MANUALLY probe the fresh surface and adjust the 'probe length' so the measured Z surface exactly matches the offset determined with the end mill. Now you can probe a part and remove exactly what you intended to. Non of my work is placed on the mill table to be finished, which is the only reason to match probe lengths to spindle gage line height.

Click to expand...

Nobody is "measuring the table". You are adding in two stages of error (calibration errors from the tool setter, and deflection from cutting), making it a less accurate method. It sounds like you are using - values for tool lengths? I hadn't considered that some people might use negative tool lengths with their probes. If that is the case, then the method I gave above is not going to work. IMO if you are probing, it's time to learn how to use positive/gage length tool offsets.

Setting the proper gage line length for tools has nothing to do with "the table". Using the gage line length is used because it is a standard length, which allows you transfer tools between machines and not have to re set tool length (provided they are all setup to use gage length tool offsets). The other reason is particularly critical when doing work that involves the tool getting very close to the work piece, things like molds, multiaxis machining etc. Knowing the gage line allows you to properly simulate the tool path in your cam system and check for collisions.

So here where were at now. Looks like some of the 09000 programs may have been deleted or moved on the control (which I highly doubt sine their write protected) so running the RPROBECAL.MIN programs throws up alarm 5212 subprogram call 09801 instructions not found. I had saved on the sever the original files that were loaded on to the machine during install EZSET.LIB, RENS1.SBB and RENS2.SBB. I guess at this point I will try to reload them and give it a shot.

I just can't believe its this stinking hard to do such a simple task. On a Hurco its soft key driven for either the part probe or the tool probe calibration, probably less then 5 min to do both.

Captdave said:

So here where were at now. Looks like some of the 09000 programs may have been deleted or moved on the control (which I highly doubt sine their write protected) so running the RPROBECAL.MIN programs throws up alarm 5212 subprogram call 09801 instructions not found. I had saved on the sever the original files that were loaded on to the machine during install EZSET.LIB, RENS1.SBB and RENS2.SBB. I guess at this point I will try to reload them and give it a shot.

I just can't believe its this stinking hard to do such a simple task. On a Hurco its soft key driven for either the part probe or the tool probe calibration, probably less then 5 min to do both.

Click to expand...

FWIW we have a recurring issue where 9000 series programs go missing (this is on a Haas). I stuck the USB backup in a folder on the network in the same location as all our programs so I can reload without having to dig out the USB from the back of the machine (where it can't get lost).

Captdave said:

So here where were at now. Looks like some of the 09000 programs may have been deleted or moved on the control (which I highly doubt sine their write protected) so running the RPROBECAL.MIN programs throws up alarm 5212 subprogram call 09801 instructions not found. I had saved on the sever the original files that were loaded on to the machine during install EZSET.LIB, RENS1.SBB and RENS2.SBB. I guess at this point I will try to reload them and give it a shot.

I just can't believe its this stinking hard to do such a simple task. On a Hurco its soft key driven for either the part probe or the tool probe calibration, probably less then 5 min to do both.

Click to expand...

Stuff like this is the reality of running a control with a 'front end" on it.

Do you run the OSP macros when you are actually probing parts? If not, I would ditch the osp stuff and just upload the Renishaw macro's, calibrate accordingly, and only use those from now on.

The renishaw files are in the ezset.lib rens1.ssb and rens2.ssb files.

The machine is still pretty new, you shouldn't have a problem calling or emailing the apps guy that set it up for answers.