[dec11ad]

does anybody have the x, y and z probe cycle for an mp10 probe on an okuma mb56va with an osp100m control?

[broby]

Turn on your probe first using
CALL OO18

To probe on an axis use the following coding:
PMOD is used to designate the axis to probe.
PMOD=1 is used to probe X axis
PMOD=2 is used to probe Y axis
PMOD=3 is used to probe Z axis

PEI is used to designate the edge position, i.e. Target point.

A Simple version of the call command would be:
CALL OO10 PMOD=x PEI=xxx.xxx

To use the value obtained from the probe cycle use the following coding:

CALL OO20 PHN= PX= or PY= or PZ=

Where
PHN= is used to set the Coordinate system
PX= Value for X axis
PY= Value for Y axis
PZ= Value for Z axis


To turn OFF the probe use:
CALL OO19

You can also use POVT to set amount of movement PAST the target point or PUDT to specify the amount of Under Travel (before) the target point.
i.e.
CALL OO10 PMOD=1 PEI=100 POVT=10 PUDT=3

This would tell the machine to hit the target point X100 within 3 mm of the start position and before it moves 10mm past the target point.
If the probe hits an edge within the target zone the probe will trigger and the position will be captured.
Using
CALL OO20 PHN=5 PX=100
will set the touched surface to X100 for coordinate system 5

There are lots of other "cycles" that you can also use. i.e. probe the ID or OD of parts between steps etc...
Hope this helps to get you started.
Brian.

[dec11ad]

i have very little experience with probing. we just got a new used mill with the reciever unit (omm) fitted and the previous owner used an mp10 probe but had it removed. it turns out our first mill also had an mp10 so we tried to see if it would communicate in the new one. so im wondering now, you are turning on the probe by calling 0018 and we turned it on by using m127. so what is the difference here...can i look at the programs being called?

[dec11ad]

broby, is there a guide with the other functions somewhere. i do want to start with finding the coordinate positions and will try it out asap but will most likely wish to use other functions like hole center probing in the future.

[broby]

Pretty sure that the sub program OO18 does use the code M127 to start the probe comms between the MP10 and the OMM receiver.
Just that the OO18 program calls handles the whole issue of checks etc...
I have attached the probing manual for your assistance.
Take it one step at a time and build up your knowledge bit by bit as trying to jump in and learn everything you can do in one bid step will just lead to brain explosion.
Start with learning how to probe on a single axis first.
Then move on from there.
Keep asking plenty of questions and I am sure that this community will do their best to assist.
Regards
Brian.

[dec11ad]

ok it seems like the macros were already loaded in the machine but when i try to run it i get an error saying 2308 alarm b untended: command missing 4 what am i doing wrong? i only get that error when i try doung x y and z edge measuring but i can complete the hole measure and bose measure cycles. so what am i doing wrong?

[dec11ad]

the program looks like this

and according to the instructions of this macro i should only have to enter g111 in mdi mode (i have it registered at g119) and alarm goes on at line call OO10

[Superman]

"Untended" is basically saying the receiver is NOT getting any signal from the probing unit

- check the battery in the probe, then, turn the probe ON and check the triggering action
( receiver should show "ready" colours, and flash when triggered, the control should also indicate triggering on the position page )

[dec11ad]

well i just probed about 6 holes without a problem, just cant get the xyz macros to work. also the battery is about 1week old now.

[broby]

Alarm 2308 is basically stating that there is a Missing argument in the CALL process.
Have you programmed the call to your sub-program as follows?
G119 X1.25 H1

The program indicates that it is linked to G111 BUT then you stated that you have it linked to G119?

I would suggest that you get the coding working in a simple program first THEN get it working as a subprogram. Much easier this way.
Attachment 258924

[dec11ad]

i am entering the cycle and data it needs to complete the cycle in mdi mode but on the xyz macros the instructions just mentioned the gcode to activate the cycle. which makes me wonder how it decides which work offset it populates and which direction it travels to probe the edges? i tried entering it as g119 X1 and it started the cycle but i have no idea what i told it to do..

[dec11ad]

The program indicates that it is linked to G111 BUT then you stated that you have it linked to G119?

yes, figured thats just for a guide, used it on g119 cause g111 was already used. could it make a difference?

Have you programmed the call to your sub-program as follows?
G119 X1.25 H1

no i have not, what does x1.25 h1 do?

[broby]

yes, figured thats just for a guide, used it on g119 cause g111 was already used. could it make a difference?



no i have not, what does x1.25 h1 do?

I was just using a sample value of 1.25" as I noticed that your screen shot showed imperial units...
The H1 value is setting Coordinate System 1

It seems that the code snippet you showed is part of a Library file.
A .LIB file is loaded into memory on Power ON.
Library files are LINKED to G codes via a Parameter screen on the Controller.
The filename is NOT IMPORTANT but it does need the ".LIB" extension not the standard ".MIN" that is generally used for machining programs.
Look through your parameter pages for the G/M Codes page and check what subprogram names are associated with each G code.
Using Library programs is not for beginners by any means as there are lots of things to bring together to get it to work successfully, but don't give up!
I cannot stress to much that you NEED to get your code working in a simple machining program format before you venture into subprograms and then into custom G code (Library files...) as you need to make sure that your code is working first as there are too many things to track down otherwise.
Time to apply the KISS principle! (Keep It Simple Silly)

The subprogram you displayed tells me several things.
The name that needs to be associated with the G code is OPBX
It also take TWO parameters:
X and H
On the line CALL OO10 you can see the code PEI=PX
what this means is that the subprogram is expecting a parameter called X
on the next line the code PHN=PH means that the subprogram is expecting a H parameter to be passed in.
i.e. if the G code is associated with G Code 111 then you can use the program like this:
G111 X(target value) H(target Coordinate System)
so if you were trying to setup the side of a job to X10.525" and set this value into coordinate system 10 then you use this:
G111 X10.525 H10

If you position your probe to the right of the edge, within approx 3/8" and manually zeroset your position to a value appropriate to your approx position, i.e. X10.750 the above code will make the probe move towards the target surface and touch off and then set the edge to X10.525 on coordinate system 10.

If you position to the Left of the target edge, manually zero set to a value smaller than the target value and the probe will move in the X+ direction towards the target surface.

Hope this information helps a little more.
Keep trying.
Brian.

[dec11ad]

Look through your parameter pages for the G/M Codes page and check what subprogram names are associated with each G code.

yes, i have done that already and assigned the .LIB programs to the macro Gcode i still had available..

G111 X(target value) H(target Coordinate System)
so if you were trying to setup the side of a job to X10.525" and set this value into coordinate system 10 then you use this:
G111 X10.525 H10

so by programming it as G111 X10.525 H10, X10.525 would define the anticipated travel distance, if im understanding this correctly? or what do you mean by target value?

Thanks For The Help!

Oh ok i think it clicked, :idea: maybe..... do you first position the probe about 3/8 or so away from the edge surface which you want to probe and look in current position screen to approximate the position you would like to probe and enter that value for X?

[broby]

so by programming it as G111 X10.525 H10, X10.525 would define the anticipated travel distance, if im understanding this correctly? or what do you mean by target value?

Thanks For The Help!

Oh ok i think it clicked, :idea: maybe..... do you first position the probe about 3/8 or so away from the edge surface which you want to probe and look in current position screen to approximate the position you would like to probe and enter that value for X?

TARGET value is the position of the face you are trying to establish, NOT the travel distance!
i.e. if I had a tool 2.000" in diameter and I wanted to position it so that the OD was 0.010" from the "TARGET" face, and assuming that the machine was already correctly zero set, then the position on the display would be X10.525+0.010+1.000= X11.535"

For the first time you are setting up a job, you generally have no idea where the job is located in 3D space within the machine area. (Well you might if you have nice fancy jigs...)
So what I do is position the probe within 10mm (3/8") of the target surface and then manually calculate the zero set position.
Then call the probe routine.
If you don't do that you may be totally in the wrong position, as far as the machine/probe is concerned. Thus leading to the probe moving in the wrong direction.
Do you know how to manually calculate a Zero Set position?
Regards
Brian.

[dec11ad]

For the first time you are setting up a job

this is what i'm trying to accomplish

Do you know how to manually calculate a Zero Set position?

ok, correct me if im wrong...you position the probe next to the edge to be probed then go to the work offset page and select the offset number desired then press calc for xyz then call the probe cycle? and so now that the offset number is 000 for xyz you only need to enter .375 for x target value?

[broby]

It depends on where your program ZERO point is.
OK. Assuming the following information is true for my example:
1. you have a block of material that is 10.525" wide and you are going to machine down the RH edge of the block to machine it to 10.500" wide.
2. Program X0 is set to the LH edge of the part for programming purposes.
3, For some reason you cannot get the probe in to the LH side of the block because it is up against a stop...
4. The RH edge is suitable for probing.
5. Probe is positioned approx 3/8" away from the RH edge of the part at what would be X10.900"

TARGET is going to be X10.525"
Once the probing cycle is complete the RH edge will be set to X10.525"

With the Probe manually positioned at what would be X10.900" (or there abouts, does NOT need to be spot on) ignore the X axis current position, it is NOT important.
Go to your Work Offset page and select the desired coordinate system, i.e. H10
Calculate X10.900
Check your position page and if you have H10 selected, your X axis will show a position of X10.900
If not check that H10 is active.
if not, use G15 H10 in MDI mode to make it active.
NOW use
Gxxx X10.525 H10
where the Gxxx is the code you have assigned to the macro.
Cheers
Brian.

PS time to go home for me, where are you located?

[dec11ad]

ok, so works like my other macros for finding the center of a hole or bose feature, (both of which i have used successfully) ill explain the hole finding macro, first you place the probe inside the hole so that the ball is below the surface and lets imagine i used g114, so now id input g114 d(approximate hole diameter) x0 y0 h(work offset preffered) press enter and cycle start in MDI mode. then id have the center of the hole displayed in guaging results..

[broby]

ok, so works like my other macros for finding the center of a hole or bose feature, (both of which i have used successfully) ill explain the hole finding macro, first you place the probe inside the hole so that the ball is below the surface and lets imagine i used g114, so now id input g114 d(approximate hole diameter) x0 y0 h(work offset preffered) press enter and cycle start in MDI mode. then id have the center of the hole displayed in guaging results..

Yes, works in a similar way.

[dec11ad]

got them working, thanks for the help!