Using round profile inserts on a lathe

[Petel]

I'm confused as to how to setup and use round circular inserts (RCMT type) on my lathe...first issue really.

I'm trying to make a simple 5mm radius semi-circular groove in a bar. I have a circular RCMT profile tool, radius 3mm. Program is a profile in intercon based on part dimensions.

Tool is setup with tip radius = tool radius at 3mm, nose vector is '0'. I have other nose vectors but without success (not sure that the machine recognizes the inserts ability to cut in z+ and z-?)

I started with cutter comp = right but that did not work at all, the side of the groove towards z+ looks odd. Setting cutter comp off looks much better but then the cut profile seems to be offset towards Z+ (by the tool radius I think?) and does not look like the graphed part in intercon.

I guess my problem is that I'm wanting the tool to cut on multiple edges, or the Z+ side specifically.

I'm struggling with the setup, any pointers for me please? I can post some files but wondered if there were any general tips that I could try first, maybe there are special considerations for these circular profiling inserts?

Thanks all.

[cncsnw]

Comp right should be correct.

Nose vector 8 will probably work best, presuming that you set your Z offset by lining up the tip of the cutter. If you set your Z offset by touching the left side of the cutter, then you will need to use nose vector 3, and the toolpath will look a little unusual, but should cut correctly.

That said, there do appear to be bugs -- at least in v4.14 -- in the lead-in for the final rough pass; retract after final rough pass; and the lead-in for the finish pass. Maybe someone who has a current demo installation handy can try it out and see if those issues are still present in v5.06 or newer.

In the attached program, T4 should be an OD turning tool approaching from the X+ side, with nose vector 8 and a nose radius of 3mm.

[suntravel]

Looks ok for me, but not perfekt.

It needs a rapid move to go to a start position, so the leadout is not chrashing.

Uwe

[Petel]

Thanks for the ideas; managed to get a result today with nose vector = 3 and cutter comp = right as suggested. The tool was set to left and front edges.

I'm still confused with the intercon graphing - on the attached image you can see the finished shape / finish cut lines overlap on the right of the profile. That's also what happens when the machine runs, you can hear the cut on / off on that part of the profile as the tool path graphic suggests. I was expecting two parallel lines and a continuous finish cut. I'm on V4.84. Any ideas?

graphing

10mm R25 tube former.lth

(1.95 KiB) Downloaded 14 times

[cnc_smith]

In Intercon F9 Setup what is the G71/G72 Rough Angle Escape Angle set to? 45 or 90 If set to 45 that may be why you are seeing the angle. Would send a report and the Intercon file so we can see what your setting are and how the program is written. With a pocket like this for the finish pass I have found that at times I had to set Z to zero and just leave material for X. This will allow material for both sides.

[Petel]

Escape angle is 45. Report and intercon file attached.

It's the finish profile graphed shape that I'm unsure about - tried many different combinations of parameters but I can never get 2 parrallel grey lines on the graphing in the radius suggesting the finish shape is not correct (because the tool tip is a full diameter)....or am I thinking about this wrongly?

I tried leaving no material for the finish cut on Z, then on X but that still shows similar issues.

The part is just a tube forming die, so the result is OK for what I'm doing now, but I'd like to understand this better.

[cnc_smith]

Petal,

Sorry for so long getting back to you. After studying the finish pass gray line and semi finish gray line you can see on the right side where the semi finish gray lines is on the right side of the finish pass and the crosses over to the correct side of the finish pass at about 4 o'clock. When you look at the yellow and red in the graph on the right side you can see where the roughing cut is cutting to far to the right. This is a software bug you have found in the G71/G70 cycle.

[Petel]

Thanks,

Am I correct to assume that this is just a graphing error in intercon and that the g-code will be correct? I'm sure I heard the cut change when I was running the job suggesting that the machine was following the graphics, or maybe it was my imagination?

Do you know if this issue is fixed in later versions of the software? I'm on V4.84 at the moment.

[cnc_smith]

This not a graphing error. The graph is running the g-code so this is the path of the tool. As far as I know this has not been fixed.

[suntravel]

It is in 5.08 the same.

Best workaround is not to use cutter comp at the moment in this case.

Uwe