CNC Lathe ARC types

[mujenpwr]

Are there any videos to go over the Diff use of ARCs for Intercon. I am following the manual and still a bit lost. I did not see anything pop up when I hit the help button either. I would appreciate any insight. Also trying to follow the radius and chamfer options.

[cnckeith]

intro to intercon lathe video.

[mujenpwr]

Thanks Keith I followed most of that. I found the section 8.18 in the lathe manual, not sure why I missed it. I will try it. So no help images pop up with ARCs?

[tblough]

So, what did you notice when you tried each type and graphed them? You can zoom in on the arc area and see the differences. Better yet, actually test them out on some scrap material.

[mujenpwr]

When I went to graph I was getting errors I can’t recall the exact message but something that the operation couldn’t run. I need to retry after I read above. Turning and facing is easy with Intercon but I’m trying to progress to CW and CCW chamfering. I tried to look at the pawn g code and learn from that. I’m not there yet I need more time to understand the logic…. I had some PVC in the machine to try some cuts

[tblough]

Starting on page 88 of the user manual are descriptions of the four different ways to specify an arc. If the numbers you enter are not geometrically correct, you will get an error (for example "arc radius too small") that will prevent Intercon from generating the g-code or graphing until the error is corrected.

[cncsnw]

For what it's worth, the "Chamfer" and "Radius" operation types on the Insert -> Other menu in Intercon are of very limited use in writing programs.

If you want a radius or chamfer in a program, you generally use the various "Connect Type" options to join one line or arc to the next line or arc, with a radius or chamfer.

If you want to radius a corner without moving the cutter along the lines leading into or out of the corner -- so that two line moves with a Connect Type = Radius on the first one is not suitable -- then you would put in a sequence like:
1) Line (rapid) to a point where you can start a lead-in.
2) Line (feedrate) to the start of the arc
3) Arc (usually specified using Endpoint and Radius)
4) Line (rapid) to move away from the part

[tblough]

I agree with Marc that the connect type is easier, but individual arc and linear moves to form chamfers and fillets has a use. I rarely ever use the connect types for the single reason that I tend to use much lower feedrates on corner breaks and arc transitions.

When you are using 0.004" (0.10mm) feed per rev to get proper chip breaking on facing moves and then want a 0.010" (0.25mm) chamfer, the connect type forces that chamfer to be made in 2 revolutions of the spindle. By using the arc features or a standard linear move I can cut the transition feature at ½ to ¼ of my normal feedrate.

To exacerbate matters, when turning and facing, the insert geometry creates a "wiper" feature that improves surface finish. This does not happen when cutting arc or chamfer transitions when you are cutting with a single point on the insert nose radius. The faster feedrates of the connect type results in a distinct helical groove appearance on these small features.

Most of the parts I make are small medical devices with 0.2mm corner breaks and 0.5mm fillets cut with 0.004" nose radius inserts. My need for different feedrates on these features probably does not translate to parts with ¼" fillets and 0.100 chamfers made with 1/16 nose radius inserts.

[mujenpwr]

Thanks for the info guys. I need to get into shop this weekend and work on it. I will report back. I’m new to acorn. The conversational programming is great. I need to apply the above to get it.