Strange lathe motion.

If I understand what your trying to do... I re-wrote the arcs. I left the radius unchanged but ended each arc properly by moving the X end point. I then added a move to the original end point. Does this look more like what you'd expect?

Original code:
N20 G2 X46.5 Z36.5 I0. K3.
N28 G2 X49.1 Z36.5 I0. K4.3
N30 G3 X54.7 Z40.8 I2.8 K0.
N37 G2 X50.5 Z36.5 I0. K5.
N39 G3 X54.7 Z40.2 I2.2 K0.


Changes:
N20 G2 X43.5 Z36.5 I0. K3.
G1 X46.5

N28 G2 X44.8 Z36.5 I0. K4.3
G1 X49.1

N30 G3 X51.85 Z40.8 I2.8 K0.
G1 X54.7

N37 G2 X45.5 Z36.5 I0. K5.
G1 X50.5

N39 G3 X52.7 Z40.2 I2.2 K0.
G1 X54.7

I've attached the plot

Yes, looks like you are right.
The start and end point not concerned, the software doesn't know what to do, try to search the point, hence the moving is unpredicted.
I will test your changes in lathe, Great THX!

forhire wrote:

If I understand what your trying to do... I re-wrote the arcs. I left the radius unchanged but ended each arc properly by moving the X end point. I then added a move to the original end point. Does this look more like what you'd expect?

Original code:
N20 G2 X46.5 Z36.5 I0. K3.
N28 G2 X49.1 Z36.5 I0. K4.3
N30 G3 X54.7 Z40.8 I2.8 K0.
N37 G2 X50.5 Z36.5 I0. K5.
N39 G3 X54.7 Z40.2 I2.2 K0.


Changes:
N20 G2 X43.5 Z36.5 I0. K3.
G1 X46.5

N28 G2 X44.8 Z36.5 I0. K4.3
G1 X49.1

N30 G3 X51.85 Z40.8 I2.8 K0.
G1 X54.7

N37 G2 X45.5 Z36.5 I0. K5.
G1 X50.5

N39 G3 X52.7 Z40.2 I2.2 K0.
G1 X54.7

Tried to apply. No luck!
The emc wrire error about center not corresponding ....
With the old values (not changed) all works.

andypugh wrote:

forhire wrote:

I ran your file in my back plotter.

Does your plotter understand G7 mode? The arcs all look fine in EMC2 with that code if G7 is active.

In fact, the whole file runs OK on my EMC2 sim lathe config.

It understands G7 diameter now that I enabled it! I was wondering why my plotter was so crazy...

Plots fine now. No errors!

I corrected the code, remove all comments.
Now it is:

(8.06.2011)
N3
T3M6
G90G56G18S1000M3M8
G1G43H3X21.Z42.F700
G1Z36.645F100.
G1X21.98F100.
X29.397Z-0.5F120.
X21.F150.
G0Z60.
N2
T2M6
G55S700M3
G0G43H2X21.Z55.
G1Z33.5F500
X38.1F150.
G0Z37.X21
G1 Z32.5 F150.
X36.F150
Z33.5
X40.5
G2 X43.5 Z36.5 I0. K3.
G1 X46.5
G0 X22.Z37.
G1 Z31.2 F120.
X38.6
Z32.2
X40.5
G2 X44.8 Z36.5 I0. K4.3
G1 X49.1
G3 X51.85 Z40.8 I2.8 K0.
G1 X54.7
G0X22.Z37.
G1Z30.5 F170.
X40.
Z31.5
X40.5
G2 X45.5 Z36.5 I0. K5.
G1 X50.5
G3 X52.7 Z40.2 I2.2 K0.
G1 X54.7
G0Z31.6
G1X22.5Z29.F150.
X26.Z31.45
G0Z55.
N1
T1M6
G54S1000M3
G0G43H1X86.Z43.
G1Z40.F250.
G1X45.
Z40.8F2000.
G1X80
Z22.F270.
G0X81.5Z40.8
G1X74.F270.
X78.Z38.5F270.
X80.
Z40.
X78.F100.
Z22.F200.
X77.9
X79.
G0X79.Z170.M9
G49
M5
M30

But I tried to open in end the error message appears

aike wrote:

I corrected the code, remove all comments.

Remove the changes I posted earlier! They are not correct! My back plotter was NOT in G7 mode. Use your original code. Thankfully, andypugh caught my mistake

Like andypugh said... add G7 to your original code and it should run properly.

linuxcnc.org/docs/html/gcode_main.html#sec:G7-Diameter-Mode

SOLVED!
The error:
N39 G3 X54.7 Z40.2 I2.2 K0. - Original
N39 G3 X54.9 Z40.2 I2.2 K0. - HAS TO BE
so as the starting point calculated from previos position:
N37 G2 X50.5 Z36.5 I0. K5.
N38 G1 Z38.
X=50.5
Z=38
The end point for X = 2.2*2+50.5=4.4+50.5=54.9
The end point for Z = 38+2.2=40.2
Hence the G3 command looks like:
G3 X54.9 Z40.2 I2.2 K0.
The lathe behave itself strange in THIS point.
Please, correct the sintax interpritator in EMC 2.5. PLEASE!