Offsetting to the Right, Left or Off for Lathe ?s.

[Stampede]

What are reasons for off setting to the Left or Right of the Profile, or tool path?

Thanks.

[bborb]

Offsetting right/left allows you to control finished dimensions on a machined part. For example, your cutting tool may wear or dull to the point where your finished part is no longer in tolerance and you can simply "offset" that tool the amount needed to cut a smaller/bigger dimension to bring the part back into tolerance.
This could be a Cad/Cam question when generating a toolpath from a drawing/model, in which case your software compensates for the radius of the tool's cutting edge.
This could also be a question regarding G41 and G42 commands in the NC program of the control, in which case the powerful math processor inside the CNC control compensates for the cutting tool's radius.
Parts with radii and radial contours can have complicated geometry and gets more complicated trying to cut these profiles with a tool that has a radius. The "offsetting" features of a CNC control and/or your Cad/Cam software tries to ease the burden of you calculating the trigonometry of the cutter toolpath verses the finished part.

[Stampede]

How to chose what side to offset? When doing O.D. machining, I would offset to Left of the Profile? When I.D. machining, I would offset to the Right, depending on what Side of "X" I was on.

Thanks.

[The One]

The purpose of Offsetting to the Left/Right in BobCAD is to determine which side of the Contour you want the reference position of the tool to be programmed to, as well as whether to leave stock for finishing.

If you want to leave stock for finishing it is necessary for you to offset the toolpath, otherwise the system will ignore the Stock allowance and create the toolpath so that the tool nose radius is cutting to the finished dimensions.

Regards,

[Stampede]

When I use offset to the right for a turn profile. Why does it feed -0.01 into the face before rad. the corner or the part, and when I use to the left it's -0.03" into the face of the part. When I use no offset it feeds to the face Z0.0, but does not compensate for the tool nose rad. I'm using a .03" tool nose rad, 0.02" rad for the corner. What I'm I not doing correctly?

Thanks.

[The One]

Stampede,

What you are seeing is what the software was designed to do.

Let's look at this in the case of a simple O.D. turn with a taper with 0.0 for finishing amounts.

Now my images may be off a little, just because I was eyeballing the placement and not using specific coordinates, so do forgive me.

When you choose Off for the Offset type, the system places the theortical cutting edge(shown in ex1.bmp) of the tool on the contour(shown in ex2.bmp). As you can see from the attached image the tool nose does not come in contact with the contour.

When you choose Right for the Offset type, the system drops the theoretical cutting edge below the contour so that the tool nose radius comes in contact with the specified contour(shown in ex3.bmp). You will see that the radius is tangent to the contour that is being cut.

Choosing Left for the Offset type is really only useful when you are cutting, generally, from left to right on the part or doing an I.D. cut. It has the same purpose as Right, but if you use it in the context reviewed above, it makes the radius tangent to the opposite side of the arc(shown in ex4.bmp).

Depending on the radius of the tool nose, you will get a different position when you are using compensation. If you use the Off option, you will get exact coordinates, but the part may not be cut to the proper dimensions.

I hope this helps ellaborate on this question.

Regards