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  |