4 vises and 4 work offsets

[kojack]

I have a very large program 19 megs running right off the hard drive

I really dont want to mirror tool paths

So i figure I could have one program and 4 work offsets

what would be the right way to call the program to each work offset

Thanks for the help

[Cory]

I think you'd just want to call out each work offset, then run a subprogram using incremental moves so that you can call it at each new offset location.

[pit202]

You can try somthing like this :

G55 G90
M98 P(number of your 16megs program)
G56 G90
M98 P(number of your 16megs program)
[...]
M30

and so on , don`t forget to delete work offsets from your 16megs program, and put M99 instead M30.

[automizer]

are you willing to edit your program? If so I would break it up in to sub-routines based on each tool and have each tool run threw all 4 work zeros. This saves on tool changes. I have found that this will speed up the program a lot if you have 20 tools in an umbrella style tool changer.

[kojack]

Originally Posted by automizer are you willing to edit your program? If so I would break it up in to sub-routines based on each tool and have each tool run threw all 4 work zeros. This saves on tool changes. I have found that this will speed up the program a lot if you have 20 tools in an umbrella style tool changer.

Its only one tool ... very detailed surfaces

Thanks for all the help guys

[kojack]

Originally Posted by pit202 You can try somthing like this : G55 G90 M98 P(number of your 16megs program) G56 G90 M98 P(number of your 16megs program) [...] M30 and so on , don`t forget to delete work offsets from your 16megs program, and put M99 instead M30.

I think im going to try your method ...

what is the m98 and m99 ?

I dont have a g and m code list @ home

[Switcher]

M98 = Call subroutine
M99 = Return from subroutine


.

[Geof]

Originally Posted by Switcher M98 = Call subroutine M99 = Return from subroutine .

On Haas M98 is the subprogram call to an external Onnnnn program.

M97 is the subroutine call to a line number location within the calling program.

[kojack]

Originally Posted by Geof On Haas M98 is the subprogram call to an external Onnnnn program. M97 is the subroutine call to a line number location within the calling program.

How Does this work when your main program is running direct from hard drive

Do i need to make the Offset program runnging from the hard drive also?

[automizer]

if you need a g and m code card here
http://www.haascnc.com/custserv_updates.asp#custserv
but you need to replace your M30 with M99 because when it reaches the end of the program it will stop and reset not move to the next work zero. Your M30 will then be placed in your M98 call program.
it may be simpler to make a sub-routine call for 4 work zeros with in the program so you will not have to worry about one being on the hard drive and the other not.
If you do it this way follow the same as described by pit202 but put it at the top of your program and use M97 not M98 and your P number calls a N line number with in the program

[Geof]

Originally Posted by kojack How Does this work when your main program is running direct from hard drive Do i need to make the Offset program runnging from the hard drive also?

I don't think it does work.

As I understand it running a program from the hard drive is equivalent to drip feeding through the serial port, but much faster.

Also as I understand it for M97, and maybe M98 everything has to be in the controller memory. When it is on the hard drive it is not in the controller memory; chunks are transferred into a buffer memory and executed. The controller can only look ahead within the portion that is in the buffer; the M97 will not work because the line being called will be on the hard drive not in the buffer.

[Geof]

I looked it up in the addendum for ethernet and hard drive; it looks like you can do M98 from the hard drive.

Go to this link, scroll down until you get to manual addendums and then you will see Ethernet/Hard drive Option. Click on that and you will find what you need on pages 4 and 5 under the section about File Numeric Control (FCN) Operation.

http://www.haascnc.com/custserv_updates.asp#manualupd