How to Program an Old toolroom Haas Lathe with Mastercam

[BARRY DURLING]

How to use Master cam to program an old Haas CNC tool room Lathe.
There is no turret and it homes to the top right and not left and the
X and Z are opposite new machines with travel directions. Z is the same
but X plus come towards the operator and minus goes towards the back of the machine.

[Colin Gilchrist]

You'll just need a proper Post setup, and to make sure your Geometry in Mastercam is drawn on the proper side.

If you are looking down from the ceiling, is the turret "above or below" the spindle centerline. In other words, when the turret is "home", is it at the back of the machine, as far from the operator as possible, or is it "close to the front" of the machine, near the operator?

The X-Axis is simple to reverse inside the Post. Set 'dia_mult' to -2. (default is 2), if your machine is in Diameter mode. If the machine is in Radius mode, set it to -1 instead of 1.

I'm guessing with no Turret, there is probably no "Work Offset" either? Do you use "G54" for a Work Offset, or is the "zero" just set at the machine, and you want XZ output?

The Posts typically have a switch variable called "home_type", which tells the Post "what kind of Work Offset output are we doing, and how does the tool approach/retract from/to the Tool Change Position. There is an option which would let you use "Home Position" to output an X and Z safe approach/retract position as the start point and last point of your Toolpath.

[O You Know]

I think this is what your asking for. First you need to make sure your tool is set up right go to your lathe tool manager and right click on the tool your using the click edit then you should see this 

Then click setup tool. Change turret to bottom and mounting position to vertical.

 Here is a sample program if you want to take a look. I'm assuming your using the generic Haas TL 2X lathe.

Haas TL Help.mcam

[SasquatchBuffalo]

26 minutes ago, Colin Gilchrist said:

You'll just need a proper Post setup, and to make sure your Geometry in Mastercam is drawn on the proper side.

If you are looking down from the ceiling, is the turret "above or below" the spindle centerline. In other words, when the turret is "home", is it at the back of the machine, as far from the operator as possible, or is it "close to the front" of the machine, near the operator?

The X-Axis is simple to reverse inside the Post. Set 'dia_mult' to -2. (default is 2), if your machine is in Diameter mode. If the machine is in Radius mode, set it to -1 instead of 1.

I'm guessing with no Turret, there is probably no "Work Offset" either? Do you use "G54" for a Work Offset, or is the "zero" just set at the machine, and you want XZ output?

The Posts typically have a switch variable called "home_type", which tells the Post "what kind of Work Offset output are we doing, and how does the tool approach/retract from/to the Tool Change Position. There is an option which would let you use "Home Position" to output an X and Z safe approach/retract position as the start point and last point of your Toolpath.

the guy below you figured it out..........................

[BARRY DURLING]

Thanks for the replies, so these are set in the Post Processor for that machine or in the tool parameters

[BARRY DURLING]

3 minutes ago, BARRY DURLING said:

Thanks for the replies, so these are set in the Post Processor for that machine or in the tool parameters