What's new
What's new

Sharp SV-2414 Odd program behavior


Jan 11, 2009
Hillsborough NC
I have a 2012 Sharp SV-2414 with Fanuc OI-MD control. Machine is new to me and I am new to Fanuc controls (I do have experience with Centroid controls, Fanuc based, but not the Fanuc control ideology itself).

Tool offsets set, G57 work coordinate system set. When the following simple facing program is started, the machine will sometimes run what appears to be properly until the first tool change, and then the machine appears to be using machine coordinates instead of the G57 WCS after the tool change. Z0 is at nearly maximum vertical travel and the Z0.6 command will sometimes result in the tool 0.6 from the part surface (G57 Z Zero) and sometimes it attempts to travel to the Z0.6 machine coordinate, which is above the maximum travel for the H85 tool length offset and will soft limit.

Restarting the same program several times will result in what seems to be random startup in Machine coordinates or using the G57 WCS, sometimes operating as expected for the first tool, and sometimes lifting the Z up and operating it at nearly the max Z height.

CAM is Fusion 360 and post is the generic Fanuc 3 axis post included with Fusion 360. Program is being operated from CF card.
Single block or full bore doesn't seem to make a difference in the way it is seemingly random in choosing the coordinate system.

Any input is appreciated,

O3104 (GPS_OP1)
( MODEL 2414)
(T3 D=0.25 CR=0. - ZMIN=-0.05 - FLAT END MILL)
(T10 D=2. CR=0.03 TAPER=45DEG - ZMIN=-0.05 - FACE MILL)
N10 G90 G94 G17 G49 G40 G80
N20 G20
N30 G28 G91 Z0.
N40 G90

(FACE1 15)
N50 T10 M06
(2 45DEG FACE 24)
N60 S6000 M03
N70 G57
N80 G00 X0.65 Y1.225
N90 G43 Z0.6 H24
N100 G00 Z0.2
N110 G01 Z-0.035 F80.
N120 Y0.625
N130 Y-3.125 F100.
N140 G00 Z0.2
N150 Y1.225
N160 G01 Z-0.05 F80.
N170 Y0.625
N180 Y-3.125 F20.
N190 G00 Z0.6
N200 M05
N210 G28 G91 Z0.
N220 G90
N230 G49

(FACE1 16)
N240 M01
N250 T3 M06
(14 3FL ENDMILL 85)
N260 S7500 M03
N270 G57
N280 M08
N290 G00 X0.65 Y0.625
N300 G43 Z0.6 H85
N310 G00 Z0.2
N320 G01 Z-0.035 F30.
N330 Y-3.125 F40.
N340 G00 Z0.2
N350 Y0.625
N360 G01 Z-0.05 F30.
N370 Y-3.125 F20.
N380 G00 Z0.6

N390 M09
N400 G28 G91 Z0.
N410 G90
N420 G49
N430 G28 G91 X0. Y0.
N440 G90
N450 M30


Cast Iron
Feb 11, 2006
South Carolina
I have the same machine. When the machine does a tool change .
It changes in g91 and it does not change back .
So after every tool change you have to put g90 in the next block.

I went into my toolchange macro and added a g49 and a g90 at the end of it fixed the problem

Rick Finsta

Sep 27, 2017
Exactly that. The toolchange macro is in G91 so just change your post processor if you're not comfortable doing it in your control.

Also, the lookahead options on these machines were sparse and implementation was odd. Make sure to use smoothing liberally for roughing toolpaths as Fusion likes to kick out a ton of lines of code, and I would regularly choke my SV-2412 with 0i-Mate-MB.


Jan 11, 2009
Hillsborough NC
Thanks guys, this wasn't accepted to be posted for a few days and I figured out the g91 / g90 issue and was able to add it to the post itself. That said, I may go into the tool change macro and add it there as Kallam noted so it doesn't need the change in the post.

Rick Finsta I have an OI-MD control (2012) and it seems to handle the code fairly well as far as look ahead. I think the Mate and the B series was quite a bit slower than the "newer" D model. This control does have the "nano smooothing", although I have not yet turned it on or even checked to see if it is a parameter that can be always on, etc.