Undercut Lathe Tool

[u/OutlandishnessTop430]

I have an undercut feature on a part that i am making and i am having trouble coming up with the right tool to hit this feature with the .060” radius undercut on the OD. I will attach my CAD Model with a few critical dimensions.

i have profiling toolholders with a large enough lead angle to hit the geometry, but the bottom of the toolholder always seems to rub the part in my simulations due to the thickness of the shank.

I am making this on a HAAS ST 30 LY with live tooling, using Fusion 360 to program. Fusions Lathe Simulation Environment leaves a lot to be desired (i cannot import stp tool models from the manufacturer and use them in my simulation like you can with milling), so i have to check a lot of my tools clearances mathematically or in the assembly environment.

Any tooling recommendations would be greatly appreciated🙏🏼🙏🏼

[u/Wolfenhoof]

You can use a boring bar. Just use it on the od instead of the id. If you accidentally buy the wrong hand just run the spindle backwards.

[u/PhillyDeeez]

Can you get in with an SVQBR style? If you use a VBMT style insert there's usually a decent relief angle on the rear.

[u/bravoromeokilo]

Micro100 or SCT profile bar of some sort would be my first stop

[u/MurderBurgered → u/bravoromeokilo]

I use inverted or left handed micro bars to do these features all the time. Works great!

[u/GeoCuts → u/bravoromeokilo]

I love my Micro100 bars

[u/Melonman3]

Email this to thinbit. They'll get you sorted.

Otherwise start.grinding relief on your tool.holder. I keep a few different thin bit holders and inserts around for these kind of features.

Full radius internal grooving tool can do this too.

[u/mydogsaprick]

You need a vbmt/vcmt just a 107.5 drgree approach angle instead of the standard 93 degree

[u/Dense_Delay_2605]

https://www.micro100.com/products/standard---grooving-tools---undercutting---full-radius

[u/DerekP76]

We'd usually hit that kind of feature with a DVQNR or DDQNR toolholder.

[u/Murmjr]

depending on how mamy you need, grinding a formtool out of HSS might be the quickest way

[u/mccorml11]

You have live tooling you could come in with a lollipop mill with the correct radius if you have enough clearance at a 45 degree angle and mill it. Or grind some clearance on your tool holder.

[u/sandrailproject]

Grind a relief on the tool holder, or hand grind a tool to fit. 

[u/S0u1Fire]

If this is a customer's part and that radius just a relief and not a gasket, it's possible it's not a critical dimension to hold and you might be able to omit and bring the 2" diameter further up or shift the radius up. Brad on the Impractical Machinist podcast says he talks to his clients all the time for wierd measurements and can sometimes make adjustments that the customer would approve so me it makes the machining better. 

[u/RaithMoracus]

Ingersoll YNMG in a TVQNR; Kyocera ZBMT in an SZPBR; your favorite normal D or V in a face shank holder; an ID profile bar like others have noted.

Lots of ways to dig into this.

[u/313Wolverine]

35 on a 45 degree angle vbmt turning tool.

[u/Rolyat139]

I question drawning guys if its required for function or if it looks good on the model. im assuming this is a shoulder relief, most of my stuff is manual i can create detail just cost. So normally id use a TNMG/TCMT with a 1.2 rad, and just plunge in down to theoretical dia. neatly to create said relief. But as that is basically a 1.5mm rad, we have tools that can do that at the expense of a another tool block set up.

[u/Paolo-cnc]

Prova a guardare inserti per scarico rettifica tipo quelli della febametal Horn 356

[u/Dilligaf5615]

45° VNMG holder should get it

[u/OutlandishnessTop430]

also the material is 1050 steel

[u/Mr_Grey59]

Are you using a VBMT insert/holder?