Fusion Turn Fanuc Post FPR/G95

[bensbenz]

 I have tried using Feed per rev mode, but the generic FANUC post output never adds any G95 commands. This is the output I  get from a simple face with that option enabled:

%
O1001
N10 G98 G18
N11 G20
N12 G50 S1600
N13 G28 U0.

(FACE1)
N14 T0101
N15 G54
N16 G99
N17 G97 S1400 M3
N18 G0 X3.04 Z2.
N19 G0 Z0.8296
N20 G1 X3.1131 F0.04
N21 X3. Z0.773
N22 X1.0375
N23 X1.1506 Z0.8296
N24 G0 X3.04

N25 G28 U0. W0.
N26 M30
%

 I also tried with another post that was modified for G32 which I have attached, and I get the same result. If I had one that did both that would be great.

[HughesTooling]

I had a scan through the post and it looks like you need to set the Property type to B or C not sure what else that does but give it a try.

Mark

[bensbenz]

When I change that to B or C I get the following if I post the OP with FPR enabled:

%
O1001
N10 G90 G95 G18
N11 G20
N12 G92 S1600
N13 G28 U0.

(FACE1)
N14 T0101
N15 G54
N16 G94
N17 G97 S1400 M3
N18 G0 X3.04 Z2.
N19 G0 Z0.8296
N20 G1 X3.1131 F0.04
N21 X3. Z0.773
N22 X1.0375
N23 X1.1506 Z0.8296
N24 G0 X3.04

N25 G28 U0. W0.
N26 M30
%

I havent tried it on the machine yet, and I dont know a lot when it comes to this stuff so please excuse my ignorance. I see the G95 at the top, does it get canceled by the G94 called in the OP itself, or is that for roughing (just looking at a G-Code reference online)?

[HughesTooling]

I don't get the same as you, have you set feed per rev in the OP you're using. This is with the FANUC post that comes with Fusion.

Mark

[bensbenz]

I was using the Post that I attached. When I change to the generic post and use type B I get this, which looks correct, right?

But using that post, I dont get the G32 threading that I need for my machine.

[HughesTooling]

Give this a try, I copied over the code that made the G32 in your post. It looks like it should work but probably best to test cutting air a few times.

Mark.

[bensbenz]

Awesome! I will try it out in a bit and let you know how it goes, thanks!

[bensbenz]

I finally got out and tested the code and I get an error before I even start. Mach3 says the line N12 G92 S1600 is wrong, something about all axes missing in G92:

O1001
N10 G90 G95 G18
N11 G20
N12 G92 S1600
N13 G28 U0.

(FACE1)
N14 T0101
N15 G54
N16 G95
N17 G97 S1400 M3
N18 G0 X3.04 Z2.
N19 G0 Z0.8296
N20 G1 X3.1131 F0.04
N21 X3. Z0.773
N22 X1.0375
N23 X1.1506 Z0.8296
N24 G0 X3.04

I think thats coming about from changing to Type B in the post settings.

[AchimN]

So what is the problem? Do you need G95 for FPR instead of G99?

Fanuc TYPE A is usually G99 for FPR and G98 for FPM.

Type B and C is G95 for FPR and G94 for FPM.

If you use TYPE A into the post you will get G98/99.

[bensbenz]

Yes it seems mach3 is a strange beast on the lathe. It needs G95/94 for FPR but is doesnt seem to like the G92 S command that gets output when I use either type B or C. I think I will switch my machine over to Mach4 and give the modified post a try with it and post back my results.

[Anonymous]

Looks like the problem is the G92 that Mach3 expects to be a coordinate offset, not max spindle speed.  Don't think that one is supported by Mach.

You probably want to get rid of the code that outputs either a G50 or G92 for that:

    var maximumSpindleSpeed = (tool.maximumSpindleSpeed > 0) ? Math.min(tool.maximumSpindleSpeed, properties.maximumSpindleSpeed) : properties.maximumSpindleSpeed;
    if (properties.type == "A") {
      writeBlock(gFormat.format(50), sOutput.format(maximumSpindleSpeed));
    } else {
      writeBlock(gFormat.format(92), sOutput.format(maximumSpindleSpeed));
    }

[bensbenz]

G50 seems to work ok, maybe I should just change the 92 to a 50 so it always outputs that?

[HughesTooling]

Just a bit of info for anyone trying to figure out the different g code, here a nice site with a lot of information.

g-code lists

Mark

Edit Mach3 here

[Anonymous]

According to the Mach4 manual G50 is supported there.

There is a G50 in Mach3 turn, but it doesn't appear to befor Max spindle speed.  It's to reset the G51 scale factors.

I don't see a way to set a maximum spindle speed so I would just remove that part of the post.  Comment it out by putting "//" in front of the lines so you can bring it back if needed.

Dave

[bensbenz · Accepted solution]

I had to dig further in the post and comment out another set of lines to completely remove the G92 for max spindle speed. I also had to switch some imperial\metric conversion code in the G32 that somehow was copied over from the original modififed post. It was causing the G32 feed calculation to be incorrect. Reference to that change can be found here:

https://camforum.autodesk.com/index.php?topic=6242.msg25149#msg25149

So attached is a post that if you use it, with Type B selected in the options, should spit out compatible code for Mach3 that includes Feed per rev and G32 threading. I have only tried it on one air cut, I will try it on an actual part tomorrow and post back what happens.

Thanks everyone for the help, maybe it will help others as well.

[fonsecr]

FYI We will get a generic Mach turning post included as soon as possible.

[bensbenz]

Great to hear, thanks.

[peteymidd]

Hi, is there a generic mach 3 post yet?
cheers

[bensbenz]

No, but the post above works for mach3 turning.

[peteymidd]

Ok, thanks benz - will try it today. Have you tried it with metric and imperial. I'm metric

cheers