using vmc as a lathe

[ddwinn]

anyone out there done this b4? i have a cincinnatti 1250 c w/acramatic 2100 ctl.

[HuFlungDung]

Well, there was this one time when I put a drill in the chuck in my mill and drilled a hole in a stationary workpiece, kind of reverse to how you'd do it in a lathe, but ya, I've done lathe work in my VMC

[ddwinn]

i probably need to change my control setting to g18? i read an article in mms sometime ago but can find it.

[pmurray]

ddwinn,

All the time on a Haas.

plm

[ddwinn]

thats cool pmurray, i'm going to be cutting durabar, i have a pretty good spindle at 10hp. i figured taking .05 thou cuts to finish a 3 in sphere should be fine. i'm using teksoft as a cam program system. can you helpwith an explanation of the g17/18 coding to facilitate this process? thanks, ddwinn.

[pmurray]

ddwinn,

I will answer your question about G17 & G18 in a moment but, first a little background on what I do.

When I said that I use a mill for cutting as a lathe, I guess what I meant is that I use the mill for making parts that are round in nature, and would lend themselves to be made on a lathe or, a combination of a lathe and mill. To save time on making parts that have features that would require the use of both a lathe and mill, I have found that I can usually do all the operations on the mill.

Take for an example a steam engine flywheel with an elaborate set of internal spokes. I would take some round or square stock, fixture it on the milling table, and, on the XY plane in 2-1/2D, cut the round profile for the OD of the flywheel, drill the bore for the axle and cut the slot patterns for the spokes. I would then turn it over and face to the desired width for the flywheel. With the exception of the cutting of the slots, all of these operations can be done on a lathe but, I find it easier to do it all on the mill. Note: in my CAM software, I set it up for a 2-1/2D mill operation.

Now for G17, G18 & G19: They are used for selecting the Arc Plane that the G02 & G03 circular interpolation commands will work in. To summarize:

G17 – XY plane (typically a mill)
G18 – XZ plane (typically a lathe)
G19 – YZ plane (a machine I probably can’t afford)

All three commands are modal, i.e. one command remains in effect until another in the set is used.

In the G02 & G03 commands, the I, J and K parameters represent the relative X, Y and Z distances, respectively, from the starting point of the arc to the center point of the arc. So if you are cutting in the XY plane, you would set G17 and use the I & J parameters in G02 & G03; cutting in the XZ plane, you would set G18 and use the I & K parameters in G02 & G03; and, cutting in the YZ plane, you would set G19 and use the J & K parameters in G02 & G03.

Now for some examples: In my above description for making the flywheel on a mill, when I cut the OD circle, I am doing it in the XY plane and use the I (X) and J(Y) parameters in the G02 or G03 command and make sure that I invoke a G17 prior to executing a G02 or G03.

Now, let’s take a lathe where you are cutting an arc along the length of a rod (Z axis) – something like you might see on a chair leg. Looking down from the top of the lathe, the profile of the arc is lying in the XZ plane. In this case you would first invoke the G18 command to set the XZ plane. Then use a G03 (counter clockwise cut) using the I (X) and K (Z) parameters. In reality this would be done with multiple G03 commands to limit the DOC but, a CAD system will take care of this automatically to give you the desired final depth and length of arc along the Z axis.

I’m not sure about how you would go about cutting a sphere on a mill – perhaps 3D – but, I still see problems for the undercut on the bottom half without a second setup and alignment with the top cut would be difficult. If the sphere is small enough, you might be able to use a rounding tool for the top half in 2-1/2D but, you will still have the indexing problem when you turn it over to cut the other side. I have not thought about it that much, just thinking off the top of my head right now.

Good Luck,

plm

[ddwinn]

thanks for the info. i realise that g18 is the xz plane. now, if you mount that short leg (4-5" x 3dia) in the spindle and you set up a gang-type lathe bits you might be able to have the part manuever about the xz plane at the different lathe tools. if you cock your head and look at the machine sideways, it is a lathe.
theoretically, a machine with helical interpolation, you can cut threads.
i have a job that i'm running 200 pcs. if i use ten cat40 blanks and mounted my part to them, i could have an automatic loading lathe. ddwinn.

[DareBee]

I have used as a lathe ddwinn style.
Stock goes in the toolholder, cutter is clamped in the vise, start turning!
PS I would never consider turning anything 12"OD though ;-)