G code is not working...

Does it give a hint what G-code it doesn't like?

Try pasting the G-code listing to www.pastebin.ca where we can have a look at it.

EMC is certainly not lying to you... if you feed it bad g code it will complain.

Did you select an EMC or compatible post processor for your CAM program?

Did you check the offending line of code with the manual to see if it is correct?

You do have to be a bit more specific to actually get some help.

John

I can't test run it here but can you tell us which line the error occurs on?

John

G70 is not an EMC2 G-code.
#EMC thinks that G70 means "inch mode" in some G-code dialects,

EMC2 uses G20 for inch and G21 for mm. Looking at the size of the part, swap the G70 for a G21

I am not sure what the : on the next line is doing. If it is meant to be a block-delete then change that line to /N030 T0 M6

With those two changes your G-code loads fine. I guess it is an impeller?

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