Some advice for post-processors for lathe.

[mhatay]

Greetings Masso people.

I have a small mill and lathe with a shared Masso controller. Switching is easy with a designated USB drive for each machine, saving configurations to the USB drive and renaming *.HT1 to *.HTG. A few reboots and Masso in reconfigured. My wiring has common connectors for steppers, limits and spindle control.

I set up the mill first and used a Fanuc 11 post for Solidworks Cam (same product as SolidCam). I am somewhat familiar with CNC mills and it went pretty well and with some edits is up and running.

But I'm having some difficulties understanding what's happening with the lathe. I couldn't find a Mach3 post for SolidWorks Cam so I am using a Fanuc generic lathe post.

I am trying to use logic to understand this but obviously failing. my problem is with the X-axis, Z is behaving.

I have read a lot of posts and checked my setup. My lathe is "tool in front". G00 X positive numbers move the too in towards CL. G00 X negative moves the tool out away from CL.

If in the tool library, the tooltip is set to the centerline. So, G90 G00 X0.000 would put the tooltip on the centerline. This all works. It also works with Masso conversational posts.

If what I stated above is correct then all X dimensions should be positive numbers.

My post is generating negative numbers for the X-axis. I am wondering if this could be that the post is for a "tool behind" machine?

Or did I screw up something else?

This is my test post from Fanuc generic. Of course, I edit out the G50 and fix tool changes to Masso compatible format. I also removed G96 to avoid problems with my speed controller.

Line N5 will give me a "tool error" as it attempts to blow by the center-line.

O0001
N1 G50 S3000
N2 G00 T0303
N3 G96 S1800 M03
N4 G99
N5 G00 X-.9686 Z.1171 M08
N6 X-.5141
N7 G01 X-.3 Z.01 F.0147
N8 X.0314
N9 X.0455 Z.0171
N10 G00 Z.1843
N11 Z.1071
N12 X-.4827
N13 G01 X-.2686 Z0 F.0147
N14 X.0314
N15 X.0455 Z.0071
N16 G00 Z.1071
N17 X-.3141
N18 G01 X-.1 Z0 F.0147
N19 Z-.0105
N20 X-.2678 Z-.4052
N21 G03 X-.27 Z-.4157 R.0507
N22 G01 Z-1.1407
N23 X-.3
N24 X-.3141 Z-1.1336
N25 X-.3441
N26 G00 X-.5141
N27 Z.01
N28 X-.1583
N29 G01 X-.0955
N30 Z0
N31 X-.1 Z-.0105
N32 X-.1168 Z-.0159
N33 G00 Z.0113
N34 X-.0541
N35 G01 X-.0432 Z.0029
N36 X-.2189 Z-.4104
N37 G03 X-.22 Z-.4157 R.0257
N38 G01 Z-1.1657
N39 X-.2686
N40 X-.2827 Z-1.1586
N41 G00 X-.4827
N42 Z.096
N43 X-.2402
N44 G01 X-.0402 Z-.004 F.0147
N45 X-.0293 Z-.0124
N46 X-.1993 Z-.4124
N47 G03 X-.2 Z-.4157 R.0157
N48 G01 Z-1.1668
N49 X-.2141 Z-1.1738
N50 X-.2686
N51 G00 X-.4141
N52 X-.9686 Z.4843 T0300 M09
N53 M05
N54 M30



Thanks in advance,

Mark

 

[evermech]

Hi @mhatay

I am running a haas tool room lathe. It is set up like a conventional manual lathe. When looking at the chuck it turns counter clockwise to go in the forward direction. X axis home is with the tool as far away from the centre as possible. When moving toward the centre of the chuck X is going in a negative direction. When moving towards where the operator stands X is going in a positive direction. X axis can go past the centre point of the chuck it is only limited by the amount of travel it has. Your program should not have any negative X values if you are not going beyond the centre point of the Chuck. When I face a part I usually go about .050" past centre to clean off the bit left in the centre so at that point I would see a X-0.05 in the Gcode.

Mayne this might help

Guy

 

[mhatay]

Guy,

Yup, makes sense, mine is the same.

What post are you using?

Mark

 

[evermech]

I'm using the Haas conversational programming that they provide. Are you able to get your work offsets sorted so you are starting at the correct place? Maybe should set X to outside of shaft, touch off and call it whatever dia. It is

Guy

 

[mhatay]

I think I figured out what's going on.

The Fanuc post is for a "behind tool" machine and if I mount my tool in the back and upside down the code runs just fine.

So is there a way to edit the post to flip to positive numbers:

I'm using CamWorks and will be hitting the books this weekend, but any help would be appreciated,

Thanks

Mark

 

[cncnutz]

Hi Mark

When you set the tool to Front in the tool table it will automatically invert the coordinates in Masso and invert the arcs.

Simply create the Gcode as if the tool is at the rear of the machine and select front mounted tool in Masso the tool table and you should be sorted.

Hope this helps

Cheers

Peter