G5 P10000 and Opti-Core

[Sandybar]

Using High Speed code G5 P10000 does not like Helix 3D arcs, I need to be able to use line to line code instead but I don't see a dialog box that allows me to use line to line instead of arcs. Is there a work around for this?

 

Thanks in advance

[Teh Bear without Brains kinda idiot]

iN CONTROL DEFINITION arc definitions ->helix support=>no hellix allowed

[Redfire427]

What do you mean by "doesn't like it"? I have used helix arcs with G5 P10000 on a Fanuc control for years and the machine just eats the code.

 

Carmen

[Sandybar]

I have a older Fanuc 18i control (2001). But it will do helix arcs in regular mode, but not in high speed mode. Am I doing somethign wrong?

[Guest CNC Apps Guy 1]

I've done hundreds of HPCC programs with no issues using helical interpolation...

 

G0G40G49G80G90
N952T95(1/2 FLAT ENDMILL - ROUGHER - LG LOC)
M6
M75
G17
G54.1P21G90B180.(BACK TOOL PLANE)
M8
G0G90X-10.8051Y21.528S15000M3T73
G43H1Z3.3318
G5P10000
M198P2102
Z12.000
M5
G5P0(HPCC OFF)
G91G28Z0.M9
G49
G90
M75
G65P9863Z5.(TOOL BREAKAGE DETECTION)
G91G28Z0.
G49
G90
M1

O2102(STUFF)
X8.2133Y20.6701Z.9086
X8.2129Y20.6805Z.9094
X8.2128Y20.6943Z.9108
G2Y20.7117Z.9122J.0331K-.3048(<<<YZIJK)
X8.2127Y20.729Z.9129J.0307K-.5351(<<<XYZIJK)
G1Y20.7429Z.913
Y20.7568Z.9129
G2X8.2128Y20.7741Z.9122J-.0121K-.5043(<<<XYZIJK)
Y20.795Z.9104J-.0168K-.3272(<<<YZIJK)
G1X8.2129Y20.8054Z.9093
X8.2131Y20.8123Z.9088
X8.2133Y20.8158Z.9086
X8.2135Y20.8262Z.9074
X8.2137Y20.8297Z.9071
X8.2141Y20.8401Z.9058
M99

[Sandybar]

When I use Helix interpolation in HPCC it gives me an planer error. If I go back to line ot line it works. But will do helical arcs when not in HPCC. Control is a Fanuc 18i with CAPS Mori Sieki add on.

[Cannon]

It is an Fanuc option that you have to choose to be able to use 3d helix arcs

We have machine like this and I disabled the arc moves from control definition.

[Mic]

I've done hundreds of HPCC programs with no issues using helical interpolation...

 

G0G40G49G80G90
N952T95(1/2 FLAT ENDMILL - ROUGHER - LG LOC)
M6
M75
G17
G54.1P21G90B180.(BACK TOOL PLANE)
M8
G0G90X-10.8051Y21.528S15000M3T73
G43H1Z3.3318
G5P10000
M198P2102
Z12.000
M5
G5P0(HPCC OFF)
G91G28Z0.M9
G49
G90
M75
G65P9863Z5.(TOOL BREAKAGE DETECTION)
G91G28Z0.
G49
G90
M1

O2102(STUFF)
X8.2133Y20.6701Z.9086
X8.2129Y20.6805Z.9094
X8.2128Y20.6943Z.9108
G2Y20.7117Z.9122J.0331K-.3048(<<<YZIJK)
X8.2127Y20.729Z.9129J.0307K-.5351(<<<XYZIJK)
G1Y20.7429Z.913
Y20.7568Z.9129
G2X8.2128Y20.7741Z.9122J-.0121K-.5043(<<<XYZIJK)
Y20.795Z.9104J-.0168K-.3272(<<<YZIJK)
G1X8.2129Y20.8054Z.9093
X8.2131Y20.8123Z.9088
X8.2133Y20.8158Z.9086
X8.2135Y20.8262Z.9074
X8.2137Y20.8297Z.9071
X8.2141Y20.8401Z.9058
M99

 

I don't see any G19 in your main program nor sub

[Joe788]

It is or was an option. I had a machine with a 16i that wouldn't do helical with G05P10000 active. It's one of the secret Fanuc option parameters. I "bought" the option.

[Mjölnir]

Windows Control Panel -> Mastercam X applet -> Toolpath Support -> HMM Kernel Arc Creation Style -> Linearize All HMM Arcs.

[Tony35]

i never had any problems on our older 18i using G5P10000

i use it all the time

[Mjölnir]

It is or was an option. I had a machine with a 16i that wouldn't do helical with G05P10000 active. It's one of the secret Fanuc option parameters. I "bought" the option.

 

We've got a Roku-Roku with a 16i and "bought" that option too.

 

The Mazatrol Matrix's when using MAZACC /and/ High Smooth don't like arcs at all, hence my prior post about configuring to linearize HMM arcs. It works well.

[Guest CNC Apps Guy 1]

I don't see any G19 in your main program nor sub

 

 

It was a snippet....

 

Did you REALLY want me to post 2,000 lines of code?

[beck250]

Check parameter 8485 bit 2. If it is zero helical interpolation is disabled in hpcc mode. Change it to a 1 to enable it. This is what we had to do to our mori with a fanuc 16i controller.

[Newbeeee™]

I like the older controls where all of the options were 'reasonably priced'

I hate these new fangled locked controls

[Sandybar]

Everybody, thanks for the advice, much appriecated. Must be still alive and kicking, still learning new things.You guys rock!