SolidCAM Mach 3 Post

[richiegore]

Hi All,

I have been learning SolidCAM and have posted a number of codes using the Fanuc post processor. The codes are for someone else so I don't run them but I have been told there are some problems. He says the tool shoots up and down and he as to restart it at the beginning of the code, see below:

%
O5000 (SMALLOVALSHEET.TAP)
( MCV-OP ) (26-OCT-2011)
(SUBROUTINES: O5003 .. O0)
G90 G17
G80 G49 G40
G54
G91 G28 Z0
G90
M01
N1 M6 T1
G90 G00 G40 G54
G43 H1 D31 G0 X-96.406 Y-46.626 Z10. S1000 M3
M8
(----------------------)
(3DR-TARGET - 3-D MODEL)
(----------------------)
X-96.406 Y-46.626 Z4.
G1 Z1.6 F2500
X-96.468 Y-48.951
X-96.342 Y-53.751
X-95.994 Y-58.101
X-95.448 Y-62.151


Additionally when the the code goes from roughing to a linear cut (see below) he has to press start in Mach 3 again.


X-84.6 Y-25.049
X-84.45 Y-24.984
X-84.3 Y-24.93
X-84.15 Y-24.891
X-83.85 Y-24.851
X-83.7 Y-24.848
X-83.55 Y-24.86
X-83.25 Y-24.914
X-83.064 Y-24.98
G0 Z4.
G91 G28 Z0
G90
M01
N2 M6 T2
G90 G00 G40 G54
G43 H2 D32 G0 X-14.95 Y16.15 Z10. S1000 M3
M8
(---------------------------)
(HSM-LIN-TARGET - HSM-RASTER)
(---------------------------)
X-14.95 Y16.15 Z13.
Z-0.8
G1 X-14.984 Z-1.059 F4000
X-15.084 Z-1.3
X-15.243 Z-1.507
X-15.45 Z-1.666
X-15.691 Z-1.766
X-15.95 Z-1.8
X-17.508
X-17.663 Y16.


Obviously this is far from ideal. All the forums I have found say stick with the Fanuc post processor so perhaps there are some settings in SolidCAM which I have overlooked? Also I am really bad at reading G-Code as I am mostly self-taught, so please excuse me if it is blindingly obvious!

Thanks,
Richard

[Brakeman Bob]

For the second problem try taking the M01 out. This is Optional Stop and if the operator has the mechine set to stop at M01 and he doesn't know it the machine will stop and require restarting.

[richiegore]

thanks, I'll remove that bit and see if it runs all the way through. I think it must be a setting in SolidCAM which is causing it, I will dig around and see if i can find it....

[richiegore]

Spot on! It was the M01 code, I googled it and found out how to switch off "optional stop" in Mach 3, told him how to do it and now runs fine!

He says at the start the tool shoots up about 100mm before coming back down and starting the cut, is that the G28 command? Could I just remove it and would the code still work OK? He finds it a bit disconcerting the way it shoots up....

Additionally, he said Mach 3 was complaining about "Flood", I assume it is referring to coolant but there is no reference to M08 in the code however, there are references to M8. Wikipedia (obviously not totally trustworthy) says the flood code is M08, is M08 the same as M8? Also can you recommend a good place to learn codes?

Thanks so much for the earlier help

[Brakeman Bob]

Yes, it is the G28 command. The line "G91 G28 Z0." is normally used in Fanuc to take the tool to a safe place in Z but normally it is not required on a 3 axis machine - I have only ever used it on a horizontal with an indexing table. Comment it out in the GPP file and you'll never get it again.

[Brakeman Bob]

Just noticed the second part of your post.

In Fanuc M08 is he same as M8 but whether the machine control will accept both formats depends on the control. Fanuc will but MACH 3 is not known to me.

A good place to learn G & M codes is the machine manuals. The ISO standard for code covers what they do to some extent but does not cover syntax so for example a G83 in Fanuc 16MB will not have the same syntax or even variables as G83 in Mazatrol ISO.

To learn to program long-hand, well there are books and courses available and of course places like CNCZone but it all comes down to getting stuck in with the manuals and standing at the machine thinking "Why on earth won't it do what I want it to...." and trying things out. That's how I learnt.

[richiegore]

Thanks for all the advice, I will look into editing the gpp file to match my needs. I know what you mean about variance in g-code from one machine to another, I will try and get hold of the manuals and start from there. I agree completely by the way, experimentation is the only way!

Thanks a million for yoour help, truely invaluable!!!!