[decent]

Hello,
Please excuse a theoretician gracing himself in the world of machining but we have an Emco Turn 50 with code generated from InventorHSM. As it's our first run, it's a simple end knock down of a 3/4" delrin round stock. We set work shift, tool shifts, and upload code. We dry run, and the code looks good. BUT, we run without dry run mode and it locks up on a G0 command right at the tip of the piece. Here's the code. Mind you, InventorHSM wants to provide G54 command but WCS is not on this machine (that I know of-it throws an invalide Gcode command). As far as I can tell it hangs up on N21.

O1015 (34 STOCK) 
N10 G90 G95 G18 
N11 G20 
N12 G92 S6000 
N13 G28 U0. 
 
(PROFILE5) 
N14 T0202 
N15 G94 
N16 G97 S1000 
N17 M3 
N18 G0 X1.4588 Z0.1969 
N19 G0 Z0.0409 
N20 X0.7846 
N21 G1 X0.7202 F0.004 
N22 G18 
N23 G1 G42 X0.6071 Z-0.0156 
N24 Z-0.4572 
N25 G2 X0.6714 Z-0.4731 R0.085 
N27 G1 G40 X0.7846 Z-0.4165 
N28 G0 Z0.0409 
N29 X0.6559 
N31 G1 G42 X0.5428 Z-0.0156 F0.004 
N32 Z-0.3906 
N33 G2 X0.6471 Z-0.469 R0.085 
N35 G1 G40 X0.7602 Z-0.4125 
N36 G0 Z0.0409 
N37 X0.5759 
N39 G1 G42 X0.4628 Z-0.0156 F0.004 
N40 Z-0.3906 
N41 G2 X0.6714 Z-0.5139 R0.125 
N43 G1 G40 X0.7846 Z-0.4573 
N44 X0.8222 
N45 G0 X1.4588 
N46 Z0.1969 
 
N47 G28 U0. W0. 
N48 M30 
%

[sinha_nsit]

This code is not in G-code system A. It is in B or C. Most lathes are set to use system A. You would need to study your machine manual to find out what it needs.

[Superman]

What controller does it have ?

A quick goggle indicates a possible Fanuc
- it is only a lathe, yes ?

then explain the g-codes you use ie G94,/G95 as these are milling codes for feed control, lathes use G98/G99
- also look at the tip offset direction (0-8) when using cutter comp as this is a b?tch to get correct

use single step to find the offending line ( or lines ), as the error could be reading ahead.
( to see if cutter comp is giving the problem, remove the G42, & see if it runs )
( make sure your retracts allow for the comp cancellation moves )

[decent]

Hi and thanks for the responses. Yes, I should have said Fanuc 0, just a lathe. However, I believe it to be Type B or C as the documentation I have on it specifies G94 and 95 as feed rates and G98 as return to start plane.

[sinha_nsit]

Change it to system A; otherwise nobody would be able to help you. Very few people use B or C.

[underthetire]

Don't think it's locking up, I think your in feed per minute (g94) with a feedfrate programmed in inches per rev, so it's just going reallllly slow.

Sent from my A3-A20FHD using Tapatalk

[decent]

Don't think it's locking up, I think your in feed per minute (g94) with a feedfrate programmed in inches per rev, so it's just going reallllly slow.

Sent from my A3-A20FHD using Tapatalk

Wow, I think you're right. I'll take a look when I'm in the lab next. The funny thing is that the dry run "looked nice" but apparently it's not compensating for the feed rate in that mode. Thoughts? Thanks!

[underthetire]

Dry run is in in inches per minute usually, that way you can dry run without the spindle rotating.

Sent from my A3-A20FHD using Tapatalk

[decent]

Good point. I think this will get us on our way. Definitely been a learning experience. Thank you.

[decent]

This solve our problem... thanks again.