[alphaorange]

I just bought a couple of MX45s with OSP7000M and can't figure out how to input programs via the 3.5 floppy drive. I have the manuals but they read like 1990 dos instructions. I can write programs and put them on a disk, but when I insert the disk and follow directions it doesn't read it. I press aux/edit...dir...type in F0: after the DI...push write..no go. FD0 gets me alarm 312 and FD1 gets me alarm 334. Time is running tight for me and I could really use some help. IBM...OSP...what the hell? Once I can get this figured, I think I'll be fine. Thanks in advance

John

[broby]

You should be using FDO: to access the floppy disk.
Cheers
Brian.

[Superman]

I just bought a couple of MX45s with OSP7000M and can't figure out how to input programs via the 3.5 floppy drive. I have the manuals but they read like 1990 dos instructions. I can write programs and put them on a disk, but when I insert the disk and follow directions it doesn't read it. I press aux/edit...dir...type in F0: after the DI...push write..no go. FD0 gets me alarm 312 and FD1 gets me alarm 334. Time is running tight for me and I could really use some help. IBM...OSP...what the hell? Once I can get this figured, I think I'll be fine. Thanks in advance

John

This is the correct method.... if you use a floppy that is formatted in OSP format ( with Brian's ammendment )

You should get ( on the command line ) [ ]= optional, item is set as default, FD0: = 1st floppy drive, MD1: = control's drive for program storage, the comma is used as a delineator
CO FD0:filename[.MIN}, MD1:

If the disk is an IBM format, then you need to EXTend, EXTend till you see the MSdos feature to be able to copy files between the disk & the control

Best method is to get the RS232 connection giong and be able to transfer between PC & control ( via PIP ).
- good if the floppy reader decides to pack it in, or your floppies get contaminated & turn into coffee cup coasters

[Algirdas]

You can use special Okuma software for Windows to record files on 3½ Floppy in OSP format.
RS232 interface is better, of course

[alphaorange]

Thank you Superman...with a little effort I am able to get them in/out. Now this must be an easy one but damn if I can find it......how do I register a program to make it the active program? I can see it on MD1 but can seem to find the method to call it. The book is not helping me with this one...

[broby]

Thank you Superman...with a little effort I am able to get them in/out. Now this must be an easy one but damn if I can find it......how do I register a program to make it the active program? I can see it on MD1 but can seem to find the method to call it. The book is not helping me with this one...

Press the "Auto" soft key to select "Automatic Operation Mode" as against say Manual or Edit mode...
The first softkey F1 should display the "Program Select" function.
Press the F1 key to activate program selection, then press the * key to tell the machine you want to select from a list of ALL programs available in the MD1: memory.
ie you should see on screen:
PS *
then press the "Write" key. You should then be presented with a list of all programs with the extension of .MIN on them that are stored in MD1:
If you type in FD1:* you will get a list of programs stored on the Floppy disk.
Scroll through the list to highlight the desired program and then press the "Write" key to select it.
You should be good to run now.

BTW Algirdas, HOW would a Windows program have helped this person? The question was based on the machine NOT on the PC!
Once again you have not read the question correctly.

[alphaorange]

Ok....Got them both going and I have to say these are kick ass machines. Milled some shapes, including circles and nothing varied more than +/-.0001". Spindle is so quiet that you can talk in low tones at 7000...hardly hear them. Best deal ever @22k. I do have some questions if you guys don't mind. What are the best ways to enter tool lengths after touching off? Do I have to type in the numbers? What about work offsets? I don't see any place where it shows any positions other than the existing work positions in the table. Can't be that hard, can it? It's also my first experience with arm style tool changers. Suppose I run tool #1 but have to stop the program and restart. Tool #1 is in the spindle so what is the procedure to start again? What should the program look like as far as pre calls and changes? You guys have been life savers, now I could use some tutoring to help me to be more efficient .....thanks so much.

John

[broby]

Ok....Got them both going and I have to say these are kick ass machines. Milled some shapes, including circles and nothing varied more than +/-.0001". Spindle is so quiet that you can talk in low tones at 7000...hardly hear them. Best deal ever @22k. I do have some questions if you guys don't mind. What are the best ways to enter tool lengths after touching off? Do I have to type in the numbers? What about work offsets? I don't see any place where it shows any positions other than the existing work positions in the table. Can't be that hard, can it? It's also my first experience with arm style tool changers. Suppose I run tool #1 but have to stop the program and restart. Tool #1 is in the spindle so what is the procedure to start again? What should the program look like as far as pre calls and changes? You guys have been life savers, now I could use some tutoring to help me to be more efficient .....thanks so much.

John

Hi John,
Zero Set information is displayed on the Zeroset page. You could have upto 50 or more zeroset coordinates available to use, or if you program them into your program, as many as you want to program!
Do you have a tool setter in the machine? If so, use that to set your tool lengths, otherwise I would suggest using a dial gauge set to Zero against the end of a Setting tool (Zero Z length) that way you can bring in each tool in upto the dial gauge Zero point and calculate the Tool Length offset from there.
If you have a probe, that will save you bucket loads of time in setting your zero point. If not... oh I feel sorry for you.
As for setting up your tool calls...
This is how I program our MC600H and MA600H with comments in brackets

T1 (pre stages tool 1 ready to go into machine)
M6 (Tool Change tool 1 into spindle)
T2 (Pre Stage tool 2)
N1 M3 Sxxxx
M8
G15 Hxx (select desired coordinate system)
.
.
.
Program as required for tool 1
.
.
.
M5
M9
M6 (tool 2 into spindle, tool 1 returned to magazine)
T3 (Tool 3 pre-staged)
M63 (no more tools required so tell the machine upon next tool change that there will be no more pre-staged tools)
N2 M3 Sxxxx
M8
G15 Hxx (select desired coordinate system)
.
.
.
Program as required for tool 2
.
.
.
M5
M9
M6 (tool 3 into spindle, tool 2 returned to magazine, no other tool pre-staged)
N3 M3 Sxxxx
M8
G15 Hxx (select desired coordinate system)
.
.
.
Program as required for tool 3
.
.
.
M5
M9
M6 (Tool 3 returned to magazine)
M2 (end of program)


You can restart on N1 for T1, N2 for T2, N3 for T3, just make sure the right tool is in the spindle and if necessary the right tool is pre-staged.
If you want to return a pre-staged tool to the magazine, use M64 and that will return the tool to the magazine.
If you don't use M63 after pre-staging the second last tool, you will get an alarm on the last tool change.
Enough for now... chew on that and ask more later.
Cheers
Brian.

[Algirdas]

a little addition concerning entering digits. You can avoid keying-in digits from keyboard with OSP. I'll explain with example. Go to HP page. Place marker to X value of HP 11. Find soft key "Calculate" which is F3 as usual. You need to F8 extend menu in some cases. Press "Calculate" (F3) and here it is: present X axis position is set to HP 11 X zerro.
Use Your imagination: the same "Calculate" works with tool offsets as well.
one more. setting the tools.
Manual mode, find tool set page. Set the tool to spidnle using manual tool set buttons. When tool is clamped to spindle, press ATC button and here it goes - tool is automatically placed to magazine, and You have empty spindle again.
You don't need to go to magazine side for tool settings.
one more to play:
F3 (the same as entering the command CALC could be any value. It is 0 if ommited.
Example: You have touch sensor which is 50mm height. You touch the probe with tool and calculate tool length as 50 like that:
CALC 50

[iMillJoe]

I just bought a couple of MX45s with OSP7000M and can't figure out how to input programs via the 3.5 floppy drive. I have the manuals but they read like 1990 dos instructions. I can write programs and put them on a disk, but when I insert the disk and follow directions it doesn't read it. I press aux/edit...dir...type in F0: after the DI...push write..no go. FD0 gets me alarm 312 and FD1 gets me alarm 334. Time is running tight for me and I could really use some help. IBM...OSP...what the hell? Once I can get this figured, I think I'll be fine. Thanks in advance

John

My shop has a few MX45's to get programs off of a microsloth formatted disk, we use the following steps

AUTO-> EDIT AUX-> EXTEND (SOFTKEY)-> EXTEND -> MSDOS -> COPY -> FD0

Use the arrow keys to select the file you want,

WRITE

type ,MD1: (comma MD1 colon)

WRITE

and bobs your uncle, the file is on the machines hard drive.

To select a file to run,

AUTO-> PROGRAM SELECT -> MD1

then use the arrows keys to select your file, and press WRITE

I always prefer that we run the machine from MD1, rather than DNC, you can't use IF and GOTO staments when running DNC.

Our masterCam post outputs tool headers like so

M01
( C-BORE M8 SHCS HOLES 2 PLACES )
IF [VATOL EQ 2 ] NAT2
T2 M6
NAT2
M01

because Okuma's don't like it when you tell it to change to the tool already in the spindle. The NAT2 is a line number saying I'm at tool 2.