[iaknown]

Hey guys, I just purchased an Okuma Crown lathe w/the OSP7000 control on it. I have run a bunch of different makes but Okuma is new to me. I have 2 basic questions that I can't find the answers too for the life of me (yes I searched).

1) How the heck do I turn the rapid feedrate down when running a program?? The control only has one knob which only seems to control the cutting feedrate. I read something about being in single block but I'd like to do it when running the program through. Someone mentioned a G-code that can do it?? Or is there a parameter I can change that will override everything?

2) I want to run multiple parts on the same piece of material without unclamping the material. So basically run a part then have it move down the material and cut another few parts or so. What do you suggest? A macro or is there another option?

As a side note, I am using Mastercam and am not familiar with the conversational on the machine (yet) so it will have to be G-code based. Any help is appreciated!!!

[Goldorak]

1) you can't it's an option.... i hate this too , the only way is to run your first part in single block, so the rapid will slow down with the button

2) copy this to your program
G91
G50Z???? (Z= shift value for next part)
G90
then yse an IF/GOTO function to return the program to the top

the m02 will clear the shift amount

"As a side note, I am using Mastercam and am not familiar with the"
In House Solution provide me a really good post processor for that OSP, i simply hate how IGF works

[iaknown]

1) you can't it's an option.... i hate this too , the only way is to run your first part in single block, so the rapid will slow down with the button

2) copy this to your program
G91
G50Z???? (Z= shift value for next part)
G90
then yse an IF/GOTO function to return the program to the top

the m02 will clear the shift amount

"As a side note, I am using Mastercam and am not familiar with the"
In House Solution provide me a really good post processor for that OSP, i simply hate how IGF works

Thanks for the quick reply.

1) Crap, that is really stupid....but I'm obviously not the only one that feels this way. So there are no G-codes that can override the feed? (I thought someone had mentioned it but not the specific code unfortunately)

2) OK makes sense however: "then use an IF/GOTO function to return the program to the top" Sorry, I never learned how to do macros, can you expound? And how should it look in my code?

M02 and M30 are the same correct? I've always used M30

I can actually manage changing the post pretty well. I've already done it for a few machines/makes. Takes me forever playing around with it but I eventually get what I want.

[littlerob]

Thanks for the quick reply.

1) So there are no G-codes that can override the feed?

2) OK makes sense however: "then use an IF/GOTO function to return the program to the top" Sorry, I never learned how to do macros, can you expound? And how should it look in my code?

M02 and M30 are the same correct? I've always used M30

I can actually manage changing the post pretty well. I've already done it for a few machines/makes. Takes me forever playing around with it but I eventually get what I want.

1) Yes there is a code for changing the feed, it's F-just not the rapid. (Sorry, I had to.) It is annoying at first but soon it will be second nature and no big deal. Use canned cycles, watch the first pass, turn off single block, and let it run

2)Why not just shift zero by so much each part? There is a macro, something like [IF] VZSHFT. Budgie or one of the other guys will correct me. I never use it because it is just way too easy to just move the part zero.

Robert

[iaknown]

1) Yes there is a code for changing the feed, it's F-just not the rapid. (Sorry, I had to.) It is annoying at first but soon it will be second nature and no big deal. Use canned cycles, watch the first pass, turn off single block, and let it run

2)Why not just shift zero by so much each part? There is a macro, something like [IF] VZSHFT. Budgie or one of the other guys will correct me. I never use it because it is just way too easy to just move the part zero.

Robert

When you say shift zero I assume you mean use the G50? Either way I need some method of a counter so I don't eventually shift zero into the chuck. So I would assume that would be some sort of macro like you mentioned. Can anyone let me know what they use? Thanks guys

[fordav11]

unfortunately there is no G55/G56/G57/G58/G59 direct equivalent on OSP

You can do something similar using an Okuma Variable in the program.

VZOFZ=123.456 (1st workshift)

CALL OMAIN (a sub-program for your part)

VZOFZ=234.567 (2nd workshift)

CALL OMAIN

VZOFZ=345.567 (3rd workshift)

CALL OMAIN

VZOFZ=456.567 (4th workshift)

CALL OMAIN

etc
etc
etc


This is the Fanuc equivalent....

G55
M98 P0001
G56
M98 P0001
G57
M98 P0001
G58
M98 P0001
G59
M98 P0001


For rapid speed you must be in single block then you can control the rapid with the feed override switch. There is no other way on Okuma.
You can easily just test your program first using the graphic simulation with machine lock on. Watch the simulation carefully and if no major problems turn machine lock off, single block on until the tool is positioned correctly then single block off and let it go.

[littlerob]

When you say shift zero I assume you mean use the G50? Either way I need some method of a counter so I don't eventually shift zero into the chuck. So I would assume that would be some sort of macro like you mentioned. Can anyone let me know what they use? Thanks guys

There is no G50 for work offsets. G50 is used for max spindle speed.

On the hard key menu you have "zero set" next to "tool data". If your part is 5mm long and your part-off tool is 2mm thick and you want 1/2mm to come off the face of the next part. 5+2+1/2=7 1/5mm or .296". Press zero set, cursor right one time to Z, press ADD -.295, press write. Now you have shifted everything .295 toward the chuck. Very simple.

You will need to use an additional variable to count parts, but is pretty basic, (wait until the other guys get on, and they'll help you with the exact macro). The reason I don't use it is; you are not going to get that many parts off one peice, without a barfeeder, what maybe 10 parts, I don't think it's worth it to record a macro.

Robert

[broby]

Here is what I have done when machining multiple parts from a bar...

Assuming your part is 10.5mm long and you are using a parting tool width of 3.10mm wide and you want to face off 0.5mm each part after moving along the bar.

Zeroset the end face of the bar to the length you program. Z11.0 if Z0 is the back face of the part or Z0.5 if Z0 is the front face of the part.
Set common variable V1=0 when starting a fresh length of material.

At the start of the program:
VZSHZ=V1*[-13.6]

At the end of the program:
V1=V1+1

What this will do is move the Z axis Zero Shift value by the "qty x length shift required".
The Z axis Zeroset value is NOT changed at all. It is only updated when the program runs the command VZSHZ=...
The system variable VZSHZ is the code for "Z"ero "SH"ift "Z"

As the first part is run off with the variable V1 set to 0 (zero) the shift amount is ZERO (as 0 times any value is ZERO)

When the part is machined the value of V1 is incremented by 1.
Thus the second part is machined with a Z axis zero shift of 1x-13.6= -13.6
The reason for that you need a negative value is because you are moving the machine in the Z minus direction for each new part!
This allows for the part thickness and the width of the parting tool and 0.5mm for the next facing pass.
Each time a part is done the next part will get Z axis Shifted by a value of QTY x Length

Providing you remember to reset V1 back to 0 (zero) at the start of a fresh bar you will be fine...

A modification to this could be to add in checks for the qty of parts that can be machined from each bar and jump to the end if V1 is not reset when the max qty is reached.
for example: if you can machine 5 parts per length program this:

At the start of the program:
IF [V1 EQ 5] NEND
VZSHZ=V1*[-13.6]

At the end of the program:
V1=V1+1
NEND M02

This will let the machine run off 5 parts and then if you press cycle start again you will see the program jump to the end of the program and no part will be machined, thus saving an embarrassing crash into the part or even worse, into the chuck!

Hope you can follow this...
Cheers
Brian.

[broby]

If you want to add a parts counter into the program just add another counter into the end of the program like this:

At the end of the program:

V1=V1+1
V2=V2+1

As you are using V1 to 'Count' the number of parts per bar you will be resetting this to 0 at the start of each bar.
But, as V2 is not being reset or used anywhere else in the program, it will just keep increasing by 1 for each part machined.
Thus if you need to know how many parts you have made, just look at the value of V2.

Cheers
Brian.

[iaknown]

You guys rock! Thanks for the replies, can't wait to give it a try.

I have a few more questions on this lathe I'm hoping you can help me with. When I get a chance I'll throw them out here.

[iaknown]

So I have a few more questions and am hoping you guys can answer them as well. Ok here goes, I'll start with the easy one (I think).....

1)I've noticed that when editing a program, after you quit and save it, it does not update the program over in Auto mode. So if you're running it and forget to reload the most recent you will actually be running the old version of the program. Does this sound right? Is there a way to have it update both when saving in Edit mode?

2)I can't for the life of me get any toolwear OR comp offset to work. I am just looking for some way to adjust the offset for wear, tweaking dimensions, etc....My tool page shows a tool offset column and a nose-r comp column. My tool nose comps are all zeroes because I program tool nose radius in Mastercam. However, even if I put a number in to adjust the cutter nothing happens. I've tried double numbers (T0202), triple numbers (T020202), etc and that is all while calling up G41 or G42 when cutting. What am I doing wrong here?

3)We are running the machine on a 40hp rotary phase converter, should be plenty according to what the converter company says. When the machine really cranks up or slows down you can hear a growl and we'll get a 4053-20 alarm: VAC Power Supply Voltage Flutter. We found a parameter on one of the main parameter pages that seemed to help: Spindle Torque Limit. It was at 100% and when we decrease it it seems to improve the problem and usually the occurence of the alarm. It is now down to 40%, the lowest it will allow. Is this the correct parameter to fix the issue? Does it sound like a power supply problem? Or is there a way to adjust the power curve or something like that?

Once again any help is appreciated guys. If I should start a new thread for something please let me know. Thanks in advance.

[broby]

So I have a few more questions and am hoping you guys can answer them as well. Ok here goes, I'll start with the easy one (I think).....

1)I've noticed that when editing a program, after you quit and save it, it does not update the program over in Auto mode. So if you're running it and forget to reload the most recent you will actually be running the old version of the program. Does this sound right? Is there a way to have it update both when saving in Edit mode?

2)I can't for the life of me get any toolwear OR comp offset to work. I am just looking for some way to adjust the offset for wear, tweaking dimensions, etc....My tool page shows a tool offset column and a nose-r comp column. My tool nose comps are all zeroes because I program tool nose radius in Mastercam. However, even if I put a number in to adjust the cutter nothing happens. I've tried double numbers (T0202), triple numbers (T020202), etc and that is all while calling up G41 or G42 when cutting. What am I doing wrong here?

3)We are running the machine on a 40hp rotary phase converter, should be plenty according to what the converter company says. When the machine really cranks up or slows down you can hear a growl and we'll get a 4053-20 alarm: VAC Power Supply Voltage Flutter. We found a parameter on one of the main parameter pages that seemed to help: Spindle Torque Limit. It was at 100% and when we decrease it it seems to improve the problem and usually the occurence of the alarm. It is now down to 40%, the lowest it will allow. Is this the correct parameter to fix the issue? Does it sound like a power supply problem? Or is there a way to adjust the power curve or something like that?

Once again any help is appreciated guys. If I should start a new thread for something please let me know. Thanks in advance.

Point 1: On the older controllers you have to "Edit Quit" and then program select, otherwise you are correct, the machine will be running on the old version of the program.

Point 2: Are you inserting your offsets in the X and Z columns on the tool data page or in the tool nose radius columns?
You need to be using the direct offset value columns (X & Z) to get the tool to be compensated.

Point 3: NFI! Go ask someone else

On the subject of either programming TNR or not... you must have to change and repost your program everytime you change the TNR on your tool...? Why not let the machine handle that for you and just output true geometry profiles instead?
If you modify the program on the machine in any way, Mastercam will not know about that and you will then lose any edits if you have to re do the Mastercam output.

My 2c worth.
Cheers
Brian.

[fordav11]

more on point 2.....
there are no wear offsets at all on OSP7000. Okuma in their infinite wisdom decided it was not required even though Fanuc had it in 1979. GREAT IDEA OKUMA!

you need to change the geometry offset to change your size. best way is to put the cursor on the offset you want to change, press ADD and type in the amount of your wear adjustment then press WRITE. you can add any number from -0.100" up to 0.100"

[Goldorak]

1- as broby said , you got to resellect the program

2- OSP 5000 don't get a Wear page like a Facun control, but newer OSP like the P-200 got it

3- check the power supply, it looks that the machine don't get enough power to handle acceleration and deceleration


for the TNR , it's a PITA to program them in Mastercam....

set your tool rad at 0 in mastercam , and use wear comp,. Then in the control of the machine set the real value of TNR.
The verify portion of mastercam wil be a little off but the G-code will be OK

don't even try to yse control comp in MCAM.......

[broby]

Personally, I really hate the idea of "Wear" offsets... either the tool "geometry" offset is correct or it is NOT!
All inserts have manufacturing tolerances and if you are chasing tight tolerances there is just no way you are going to convince me that you can control your size by way of just using a "Wear" value and resetting it to 0 (zero) just because you have a new edge in place.
Controlling your sizes by altering, potentially, two different values makes no sense to me, get your offset correct and keep it correct, whether you are using a roughing tool or finishing tool!

Fordav11, you mention that the maximum amount of change is limited to + - 0.100", well that amount is controlled by parameters. You can turn on the max change amount or not and you can control what the max change amount value is... even on the older controls.

I fail to see, must be getting blind in my old age, how a TNR compensated program can accurately control a profile. I have many times used the TNR value in the machine to get spot on Spherical shapes. If the size of the TNR is off even a small amount, getting an accurate shape is nigh on impossible without using the TNR compensation on the machine.

Cheers
Brian.

[WallyL7]

I have an older Cadet and when I set up a new program, we have to go into the parameters for the rapid and actually set them to 1/10th of what the max is. I will normally run all prototypes and sub 5 part runs with it at that speed, then if I am running production and it is running fine, set it back to max.

Having to change the parameters = lame
but
having to run new programs on this funky lathe at full rapid = stupid.

It only takes about 15 seconds or less to change them. Write them down so you know what the factory settings are (or take pictures with your phone of EVERY parameter page ...just...in...case...lol

I have the OPS5020...

[iaknown]

1) Well that's an accident waiting to happen but I'll have to get used to reloading the program after I edit!

3) I think I'm on the right track but I will probably start a new thread on this one w/that alarm. Maybe someone who has run into the same issue with a similar setup can chime in...

Now back to 2):

Personally, I really hate the idea of "Wear" offsets... either the tool "geometry" offset is correct or it is NOT!
All inserts have manufacturing tolerances and if you are chasing tight tolerances there is just no way you are going to convince me that you can control your size by way of just using a "Wear" value and resetting it to 0 (zero) just because you have a new edge in place.
Controlling your sizes by altering, potentially, two different values makes no sense to me, get your offset correct and keep it correct, whether you are using a roughing tool or finishing tool!

Fordav11, you mention that the maximum amount of change is limited to + - 0.100", well that amount is controlled by parameters. You can turn on the max change amount or not and you can control what the max change amount value is... even on the older controls.

I fail to see, must be getting blind in my old age, how a TNR compensated program can accurately control a profile. I have many times used the TNR value in the machine to get spot on Spherical shapes. If the size of the TNR is off even a small amount, getting an accurate shape is nigh on impossible without using the TNR compensation on the machine.

Cheers
Brian.

So Broby and Goldorak and others, you agree on this issue? (just want to make sure I am reading correctly). That is news to me. I started on running mills and we NEVER let the control handle comp (just wear) because I (along with some other much more experienced guys) felt it's always best to let the fancy software, like Mastercam, handle the comp. It becomes an issue with large diameter cutters, going around corners, etc. So I figured the lathes were always the same. We also run a Haas lathe here and I've always comp'd in the program and only use the control to adjust for wear when necessary and I've never had a problem whatsoever w/dimensions or anything, nor is it hard to do in Mastercam. Maybe because I'm not doing a lot of spherical shapes w/real tight dimensions?? Not sure what the trouble is you're referring to...

Regardless of which method I use, if I call up the tool offset w/radius comp, say T0202 and use the corresponding G41/G42 according to the cutting direction, shouldn't something be changing when I put anything in the TNR page?? Because it's not. Like I said I've tried T0202, T020202, then .005" or .050" in the table and it's still skimming the part in the same spot. Does that sound right?

Thanks again guys, I'm learning!!

[iaknown]

I have an older Cadet and when I set up a new program, we have to go into the parameters for the rapid and actually set them to 1/10th of what the max is. I will normally run all prototypes and sub 5 part runs with it at that speed, then if I am running production and it is running fine, set it back to max.

Having to change the parameters = lame
but
having to run new programs on this funky lathe at full rapid = stupid.

It only takes about 15 seconds or less to change them. Write them down so you know what the factory settings are (or take pictures with your phone of EVERY parameter page ...just...in...case...lol

I have the OPS5020...

Interesting....can you tell me which parameters? I definitely want to do this.....I own the machine but it's in my buddies shop, he's new to CNC and wants to learn it. But I really don't want him crashing the thing at 100% rapid. This thing makes our Haas look slow and even makes me nervous!! So I don't mind turning down the rapids and sacrificing some productivity for the Okuma guy not having to come and rebuild stuff lol.

[WallyL7]

It is easy to find on the 5020...but of course, I have to page around every time I do it. Let me see if I can find the exact one.

[broby]

Regardless of which method I use, if I call up the tool offset w/radius comp, say T0202 and use the corresponding G41/G42 according to the cutting direction, shouldn't something be changing when I put anything in the TNR page?? Because it's not. Like I said I've tried T0202, T020202, then .005" or .050" in the table and it's still skimming the part in the same spot. Does that sound right?

Sounds like you are trying to use TNR offset values to change Geometry sizing...?
Altering the TNR will have NO EFFECT on altering Diameters or Lengths at all!
Altering the TNR will only alter the tool position when turning Tapers and Arcs.
So if you are machining a Stepped shaft with only parallel diameters and 90° Faces you control sizes with the Tool Offset values NOT Tool Nose Radius values.

On your Tool Data page you should have 6 columns
Column 1 = Tool offset Number.
Column 2 = X Axis Tool Offset (Geometry offset)
Column 3 = Z Axis Tool Offset (Geometry offset)
Column 4 = X Axis Tool Nose Radius Value
Column 5 = Z Axis Tool Nose Radius Value
Column 6 = "P" Code telling the machine what direction the TNR is pointing.

The first column usage is rather obvious, Tool Offset Number is 99% used to represent the Physical Tool Number, but not always... (more on that later!)
Columns 2 and 3 represent the "offset" from the Zero Tool on both X & Z. i.e. if Tool 1 is your Facing Tool and is your "Zero" tool for Z axis, it will have a Z offset value of "0" (zero).
Tool 2 might be your Rough Turning Tool and the edge of the tool is 0.2mm behind Tool 1, therefore the Z axis Tool offset will be Z-0.200
If you follow the norms and set your X0 point as being the centreline of the ID tool holders, your X axis tool offset values will be positive values by what ever amount is needed to bring the edge of the tool to the correct programmed position.
NOTE that I have not said anything about TNR values yet...
Now, if you find your Finishing tool is cutting undersize/oversize from your desired position, simply move your cursor to the correct tool offset line and position it on the X axis offset value. Press the "ADD" button and ADD the amount of difference you want the tool to move. i.e. +0.02 if the tool is cutting 0.02 undersize or -0.02 if the tool is cutting 0.02 oversize.

To setup the TNR compensation values, I always use the P Code in Column 6 to setup the direction of the Nose Radius and then Set the size of the Nose Radius in Column 4 (* NOSE-R COMP * X axis) field.
If you press the "GUIDE" button when the cursor is on the X or Z fields for NOSE-R COMP values you will see a picture showing the tool and the required "P" code to use.
To get the correct tool picture to use you need to set the tool shape for the selected tool.
But if you can not be bothered with setting the tool shape and finding out the correct tool "P" code... then set the values for the NOSE-R COMP as appropriate.
i.e. if you are using an external turning tool with a 0.8mm TNR then X will be X0.8 and Z will be Z0.8
For a boring bar the values (with the same insert) will be X-0.8 and Z0.8
i.e. set the direction to the centre of the insert with + or - and then the size of the TNR.

Grooving tools use multiple offsets to get the width of grooves correct. Thus the statement that most of the time the Tool offset number matches the physical tool number. Otherwise why do builders provide more tool offsets that what is physically in the machine?

Hope this helps a little bit more...
Cheers
Brian.