What Insert to use for Partial Radius Groove ?

RocknRonF · Jan 14, 2019

Hi Guys, Beginner here. I have to cut this .040-.041"Radius Groove in a part, .056" deep into the part. What Size Full Nose Radius Insert do I need to accomplish this? I assume I use a standard .047" Full Nose Radius insert and by going only .056" deep, should leave me with the .040-.041" Radius but I'm not sure. There must be a formula for this. Any suggestions? This will be done on a manual lathe.

MattiJ · Jan 14, 2019

0.041 radius insert, fed to 0.056 depth

aerodark · Jan 14, 2019

That 4 microfinish call-out will be impossible on a lathe.

Finegrain · Jan 14, 2019

The tolerance for the groove radius is a bit precious. You will be at the mercy of the insert manufacturer, and I bet they will not guarantee +/-.0005" on the radius.

You would be less sensitive to tool radius if you interpolated with a .031" or even smaller radius insert. Maybe even a 331 V insert instead of a grooving insert. The 331 should have a .016" radius, and may have a sufficiently acute angle to make your groove.

Regards.

Mike

Finegrain · Jan 14, 2019

Finegrain said:
The tolerance for the groove radius is a bit precious. You will be at the mercy of the insert manufacturer, and I bet they will not guarantee +/-.0005" on the radius.

You would be less sensitive to tool radius if you interpolated with a .031" or even smaller radius insert. Maybe even a 331 V insert instead of a grooving insert. The 331 should have a .016" radius, and may have a sufficiently acute angle to make your groove.

Regards.

Mike

Whoops, never mind on interpolating the groove, I just saw "manual lathe". Good luck

.

Regards.

Mike

Limy Sami · Jan 14, 2019

Can't help with an insert (I'd grind a tool from HSS) …...but here's (IMHO a good) circle calc Circle Calculator

guest · Jan 14, 2019

RocknRonF said:
...I assume I use a standard .047" Full Nose Radius insert and by going only .056" deep, should leave me with the .040-.041" Radius but I'm not sure.

If your tool is .047" rad, the groove is going to be .047" rad no matter how deep you cut it.

The width is not called out- as mentioned previously, you need a .040"/.041" radius grooving tool, plunge .056" deep. The width of the groove will be the same as the grooving tool (.080"/.082"), since the depth is greater than the radius.

Finegrain · Jan 14, 2019

guest said:
If your tool is .047" rad, the groove is going to be .047" rad no matter how deep you cut it.

The width is not called out- as mentioned previously, you need a .040"/.041" radius grooving tool, plunge .056" deep. The width of the groove will be the same as the grooving tool (.080"/.082"), since the depth is greater than the radius.

Oops, you are correct! The drawing makes it look like the groove depth is well short of the radius, but the numbers tell a different story.

Regards.

Mike

Finegrain · Jan 14, 2019

Limy Sami said:
Can't help with an insert (I'd grind a tool from HSS) …...but here's (IMHO a good) circle calc Circle Calculator

Ah, you are pretty good at the grinder if you can hand-grind a radius +/-.0005" :eek:

.

Regards.

Mike

WizardOfBoz · Jan 14, 2019

In looking at this drawing, I see what others have pointed out: a 0.056 depth for a 0.04005 radius. If so, you need a flat-sided tool (like a parting tool) that is 0.082" wide, and has the 0.041 radius at the end. This will result in a groove with straight sides for 0.0155", with the bottom radiused.

I'm skeptical that this is what was intended. Could be. But the drawing has a little ripple in the dimensioning line, so could the 0.056 dimension be the edge radius/chamfer dimension? Then, the depth for the groove could be 0.041. Or anything.

Point is, I'd ask the customer to clarify this before buying the wrong tool for the job they need.

Limy Sami · Jan 14, 2019

Finegrain said:
Ah, you are pretty good at the grinder if you can hand-grind a radius +/-.0005" .

Regards.

Mike

T&C grinder ……..and only if I try VERY VERY HARD I might be lucky.

N54 · Jan 14, 2019

EDIT for correct link

This isn't a job for an insert in a manual lathe. You need to make a tool that has the exact radius you need....

The OP doesn't mention material, so let's assume 6061

I'd grind one of these M2 drill blanks to a full round end. McMaster-Carr Then set up in the surface grinder to grind 1/2 the diameter away- looks like spade drill at this point. Hand grind in relief. Feed it .055 depth (.110 on the dial).

The last .005 would be fed with a 50 RPM or less spindle speed to minimize chatter- lots of heavy oil. Polish the final .001 out with oiled emery @600+ RPM.

CarbideBob · Jan 15, 2019

I doubt the ability of a manual lathe with the best in the world, well seasoned machinist to make this part to print without an enormous amount of time and effort.
I will second that with that I see it hard to do on a cnc.

First lets work with that you can grind this radius into a a tool with a swing on a T/C.
If there is any top rake the cut radius won't be right due to height vs dia. and the changing tool contact from up/down centerline.
One could go zero but there is that 4 RMS. Even with a elliptical tool end (to comp for as ground verses actual cut) holding that is going to be a bitch in a plunge.

Maybe a overly specked part but if matching the print is needed ......
With a rad this tight and the finish spec very nice inspection equipment enters the equation.
Opposite side of that is can the customer check it.
Bob

Search

Largest Manufacturing Technology Community on the Web

Search

What Insert to use for Partial Radius Groove ?

RocknRonF

Plastic

MattiJ

Titanium

aerodark

Titanium

Finegrain

Diamond

Finegrain

Diamond

Limy Sami

Diamond

guest

Guest

Finegrain

Diamond

Finegrain

Diamond

WizardOfBoz

Diamond

Limy Sami

Diamond

N54

Plastic

CarbideBob

Diamond

Similar threads