Spiral internal groove

[Jaani]

An internal groove (Multi start point) with a big pitch is to be done on a turning center. Suppose:
Length = 30 mm
Helix angle = 15 degree
Groove diameter = 100 so Pitch = 84.179
Width = 4
Depth = 2
Number = 10

My knowledge is so weak at appropriate tooling and method to accomplish. So please help me out.
G76 threading cycle or C axis., which one do your recommend? What are the advantages and disadvantages of each one?
What kind of tooling (Holder + insert) do you advise?

 

[lobust]

You're talking about a grease groove in a plain bearing I'm guessing?

G76 doesn't work for this unless you're ok with the groove going all the way through the part or having full round grooves at either end to start and stop in.

You can use G32 with lead in and lead out moves, or you can use the C axis. Using the C axis provides the most control over the toolpath.

I generally use a 45deg lead angle grooving bar - the kind designed for corner undercuts - with a full radius insert. The high lead angle tends to cause the insert to gouge the leading edge of the groove, and this type of bar provides a bit more relief compared to a standard grooving bar, and is easier to grind a bit more if required.

 

[Jaani]

Not a grease groove, something like this picture that the groove goes through.
In this case, G76 is faster or C axis? It seems in G76 spindle may rotate in more RPM, so the time is less.

 

[lobust]

Not a grease groove, something like this picture that the groove goes through.
In this case, G76 is faster or C axis? It seems in G76 spindle may rotate in more RPM, so the time is less.

View attachment 3890

When doing high lead threads, threading cycles (G76, G32 etc) are limited by the max. Z axis feedrate.

On the other hand, C is limited by max. C axis rpm.

Doing multiple grooves like that with a threading cycle means offsetting every groove in Z, which adds up to a lot of air cutting. Using a sub or a macro with CZ interpolation does not have this limitation. To further complicate matters, some controls do not require a Z offset to cut multiple leads, but most do IME.

It's not necessarily the case that the threading cycle will be faster, it depends on how many grooves, how steep the lead angle is, and how fast your machine can run its C axis compared to how fast it can feed its Z axis...

Re. the groove geometry in your picture - those grooves are square and the depth to lead angle ratio means that the cutting edge of the tool will need to be rotated to approximately match the lead angle in order to have sufficient relief on the leading edge.

 

[Jaani]

Re. the groove geometry in your picture - those grooves are square and the depth to lead angle ratio means that the cutting edge of the tool will need to be rotated to approximately match the lead angle in order to have sufficient relief on the leading edge.

Sorry, how to rotate the cutting edge of the tool? After watching the picture, you still recommend the above holder with a square groove insert?

 

[lobust]

Sorry, how to rotate the cutting edge of the tool? After watching the picture, you still recommend the above holder with a square groove insert?

Custom tooling at that point.

Imagine a simple internal groove cut with a grooving bar, then imagine an internal keyway cut with a broach. Your high helix slot is halfway between the groove and the keyway, so the tool you cut it with needs to be halfway between the grooving bar and the broach.

 

[mach ramsey mn]

I’m Not a turning guy by any stretch of the imagination. With the prevalence of all of these multistart threads you would think someone would have the tooling to do this. Am I mistaken? Maybe Horn?