G code is not working...

yes that is an impeller. but i cant really understand that what is wrong with EMC bcoz it must support this code..bcoz this code is running totally fine on other professional machines(i know bcoz i tested it).

There is nothing wrong with EMC. No two control systems implement g code in the same way once you get past G0 and G1 period. You have to adapt your code to run by EMC not your other machine.

John

You will probably find a choice of G-code postprocessors in Unigraphics. They all do things in slightly different ways. (G20 and G21 to choose the measurement units is rather more normal than G70, in fact)

According to en.wikipedia.org/wiki/G-code G70 is a repetative cycle code so I can't decide whether it was unit choice or repeat in your code. Does the :0030 mean "this line is a continuation of the line above, and I want T00 (zero) repeats, and do a tool change with no defined tool, too. That makes even less sense.

What units (inch or mm) is the part defined in? What controller type do the other machines have (which do run that code?)

In Haas G-code G70 takes I J L parameters and is a repeat code ( atyourservice.haascnc.com/faaqs/haas-cnc...g-bolt-hole-circles/ )
Visual CNC uses G70 to enter Inch mode ( nilno.com/cnc/gcodes.html )
CNCexPro uses G70 for Lathe Finishing. ( www.cncezpro.com/g70t.cfm )
Heidenhaan uses G70 for inches
Press-Brakes use it as a rapid move ( www.amada.com/site/default.asp?format=html&page=gcqref.htm#g70 )

Given that it has at least 4 different meanings, I think the decision by EMC2 to not use it at all is probably wise. Imagine getting a roughing cycle when you wanted inch mode?

Andy,

That was quite a bit of research you did. Excellent answer.

John

Hi,

I'm also trying to get a working g-code from Unigrapgix NX6. I builded a new postprocessor and changed G70 to G20 and G71 to G21. The first error is gone but now there is another error:

"near line 13" pastebin.ca/1993311

can anybody help me to build a working postprocessor or found a working configuration vor NX6 and EMC2?

Axel

The error is pretty clear your radius is off for your arc by a whole bunch. This usually means you were not properly positioned at the start of the arc or your offsets are not correct. You can turn off the line numbers on your post processor as they are not needed.

When I'm writing a post processor for any control I start with a line then add an arc and get that to work in all directions and quadrants before trying a complex part. This rather simplifies the process. I also start with arcs of a known size and that makes it easy to see if the code generated it what I expected. I also use the Arc Buddy to generate my code to check my post against.

John