[fxstc]

We are trying to machine a simple contour using G02 and when it gets to that step the axis reverses direction and continues on the arc until it limits out. Changing between G02 and G03 didn't change it, nor did changing from x,z,r to x,z,i,k.

Is this a Mach problem?

We are using Surfcam to generate the toolpath.

[benji2505]

are the i,k or r values set torelative movement or absolute on the settings screen?

[btu44]

I assume your talking about the duality lathe. If so, I had the same problem.
First you will need a liability release from Tormach.
This will give you access to the Mach 3's settings.
There you will find a setting that reverses lathe G02 & G03 movement. This has been set. Why...I have no idea???
Keep in mind that any code generated from a Mach3 Lathe wizard will be hosed after making this change.

[fxstc]

We are running in absolute.

Thank you very much for the information about the release from Tormach, I'll try that right away!

[btu44]

I just double checked. The setting your looking for is "Reversed Arc's in Front Post"

But if I may say, there are some other negatives to signing a liablity release. I believe your warranty will be voided and Tormach may not be able to provide support for some issues. Also it's easy to be tempted to tinker with other setting that could be disasterous.

Good luck

[dbrija]

.

[benji2505]

Sorry if I am chasing things that might be obvious, but go on the settings page in Mach and check whether the j,K (radius) values are interpreted as relative to the most recent position or whether they are interpreted as absolute coordinates in the system. Our setting is for relative movement. We never had an issue with G02/G03 (so far?).

[btu44]

Below is examples of code I generated to make an OD Fillet.
The material is 2" round and would be turned down to 1" with a .2" rad fillet.
The toolpath goes from diameter inside to out.

This code is from Mastercam:

%
O0000
(PROGRAM NAME - OD FILLET MC)
(DATE=DD-MM-YY - 29-04-11 TIME=HH:MM - 22:18)
(MCX FILE - T)
(NC FILE - \\MILL-PC\PCNC3\GCODE\LATHE\OD FILLET MC.NC)
(MATERIAL - STEEL INCH - 1030 - 200 BHN)
N100 G20
(TOOL - 1 OFFSET - 1)
(STYLE AL TPMM222 INSERT - TPMM-222)
N101 G0 T0101
N102 G97 S1600 M03
N103 G0 G54 X1. Z.1
N104 G98 G1 Z-.3 F3.
N105 G2 X1.4 Z-.5 R.2
N106 G1 X2.
N107 G0 X2.25
N108 G28 U0. W0. M05
N109 T0100
N110 M30
%


This code is from the Mach 3 Wizard OD Fillet:

G18 G40 G49 G90 G94 G80
M3
G0 X3 Z0.75
F0.1
G0 X0.5
G1 Z-0.3
G3 X0.9 Z-0.5 I0.2 K0
G1 X3
G0 Z0.75
M5
M30


The Mastercam code use the G2 which is correct. But the Mach3 code has a G3 which is wrong for a typical CNC lathe.
I'm guessing that Tormach felt that most users would be using the Wizards and not CAD-CAM. This might explain the reversed arcs setting.

[fxstc]

Benji2505, I'll check that and see if it makes a difference.

btu44, I think you are correct Mach is doing its own thing on this application, instead of properly handling basic G02/G03 commands.

I checked out the example code for the pawn piece that came with the Duality lathe, it cuts fine on the lathe, but regardless of the simulator, it made the arcs on the wrong side (but it cut correctly!). So now with this in mind, I'll write the commands wrong and see what happens on the lathe.

I've never been impressed with Mach, but for the money it is hard to beat. Stuff like this is nonsense, whomever watches over this code should be ashamed.