G code is not working...

More
25 Oct 2010 09:22 #4824 by shiv
hello friends,, i installed emc2 today.... and my problem is = my G code is not working at all. i created my G code from "unigraphics 6" , and the EMC2 says something like = invalid G code OR unknown G code format" .....

guyz plz help me......:(

Please Log in or Create an account to join the conversation.

More
25 Oct 2010 09:47 #4828 by andypugh
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.

Please Log in or Create an account to join the conversation.

More
25 Oct 2010 11:53 #4833 by BigJohnT
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

Please Log in or Create an account to join the conversation.

More
26 Oct 2010 18:05 #4880 by shiv
Replied by shiv on topic Re:G code is not working...
ok friends, here is that Gcode....


www.pastebin.ca/1973850


click on it plz.

Please Log in or Create an account to join the conversation.

More
26 Oct 2010 18:40 #4882 by BigJohnT
I can't test run it here but can you tell us which line the error occurs on?

John

Please Log in or Create an account to join the conversation.

More
26 Oct 2010 19:35 - 26 Oct 2010 19:40 #4883 by andypugh
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?
Last edit: 26 Oct 2010 19:40 by andypugh. Reason: a 500mm impeller seemed wrong...

Please Log in or Create an account to join the conversation.

More
27 Oct 2010 11:20 #4893 by shiv
Replied by shiv on topic Re: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).

Please Log in or Create an account to join the conversation.

More
27 Oct 2010 11:29 - 27 Oct 2010 11:29 #4894 by BigJohnT
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
Last edit: 27 Oct 2010 11:29 by BigJohnT.

Please Log in or Create an account to join the conversation.

More
27 Oct 2010 12:06 #4895 by andypugh
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?

Please Log in or Create an account to join the conversation.

More
27 Oct 2010 12:11 #4897 by BigJohnT
Andy,

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

John

Please Log in or Create an account to join the conversation.

Time to create page: 0.109 seconds
Powered by Kunena Forum