[Soteer]

First I'd like to thank you all for the great help yo provide for each other

next , here is my problem

I've been using Edgecam for 2 years now and it is quite handy i use it in the company i work for we have there two okuma CNC Machine

but the problem is that i use different (machine definition) for each

lately one of my friends bought a new machine and it is Taiwan made

i found that he uses powermill but without the need for a machine definition when i opened the g code i found that it transfer the whole axis to the new position of start
uses the following

%
:0001
N10G91G28X0Y0Z0
N20G40G17G80G49
N30G0G90Z2.
N40T1M6
N50G54G90
N60( Toolpath Name: 1.000)
N70( Output
N80( Units: MM)
N90( Tool Coordinates: Tip)
N100( Tool Number: 1)

unlike edgecam

he told me that he can generate a g code that will work on any machine but he knows it only on powermill and he doesn't even know why (he is not an engineer )

so is there is a way to do so in edgecam

thanks all

[jsanders]

It sounds like your friend uses a common code across all the CNC machines, and can therefore use a single post processor.

If you can determine what CNC code will work universally in your CNC machines, you could use a single Edgecam post processor. However, the machine simulation with the accompanying kinematics and models are typically specific to each CNC machines. In consideration of this, a user would have a master post processor that provides edit-free CNC code to the "universal code format", and then make copies of that where the machine configuration for each different CNC machine model is defined.

[Soteer]

thanks for your reply

but the main problem is that i want to be able to make g-codes for some people
and i dont have the ability to go there

how is it possible to do so
all i know is that it uses fanuc or okuma

is this enough

and if the code doesnt contain complicated orders can it be easier

sorry for causing a headache

[jsanders]

Generally speaking, tegardless of the CAM system, a different post processor is required for each unique CNC code format.

[Soteer]

you are right

but lets say im using one tool at the time (end mill)
and that the program is points only
using
G00
G01
G02
M00
M02....... etc

all are common and any machine can interpret them

is that possible

[tummen]

If you just use one of the standard post processors from the demo pack, you will get G codes, if this later can be used or not in all your mashines is up to the maschines not EdgeCam.
You can go into the codeWizard and chang things to a format you want but if several mashines will accept your code or not is 100% up to the mashines.
Can you even hand write a program and then load it into all mashines? If so, then you can make this same program from EdgeCam

[jtreanor]

Hello Soteer,

My company purchased 8 new - identical milling machines,
there were shipped to 8 separate locations,
installed / setup by 8 different technicians,
the same program would NOT run in all 8 machines,

yes, all fanuc machines recognize G02 as an arc move,
but different machines require IJK or R parameters
and wether the values are absolute or incremental,
or is a +- sign required.

G04 is dwell, some machines require the letter X
and some the letter P, is it measured in time or
revolutions, with a decimal point or without.

there are so many options and settings I would say it is
not possible to generate a complete program using
generic G code that will work on any machine.

Your post said -
"i want to make g-code programs for people,
and i dont have the ability to go there"

If the people can provide you with an example of a good program
that runs in their machine, you can use Code Wizard to create
a postprocessor specific for that machine.

JimT