Do I need tool with 0 nose radius to do that?

M Code · Aug 3, 2021

Hi

I have a job the required doing an OD groove, the above two edges of the groove require to have R0.005 on both edges as attached. Do I need a 0 nose radius insert to do that?

TeachMePlease · Aug 3, 2021

An OD groove can be programmed with any nose radius tool that will fit into your groove...

thedude31 · Aug 3, 2021

I would cut groove first before finish pass on OD then on finish pass create geometry to have the rads included on od pass. Still learning lathe programming but that would be how I would approach it.

M Code · Aug 3, 2021

TeachMePlease said:
An OD groove can be programmed with any nose radius tool that will fit into your groove...

Thank your for your reply

In fact I am not talking about the R value inside the groove I am referring to the above two edges of the groove need to be 0.005R just to break the sharp edges. How that can be done?

David Ferguson · Aug 3, 2021

By programming a toolpath that takes into account the nose radius of your tool. You might even be able to do it with your grooving tool.

Mike1974 · Aug 3, 2021

In cam, no. Free hand i don't know

M Code · Aug 3, 2021

David Ferguson said:
By programming a toolpath that takes into account the nose radius of your tool. You might even be able to do it with your grooving tool.

OK using Cam software. For example I will use 0.03 nose radius.. Can that do the 0.005R?

David Ferguson · Aug 3, 2021

sure, you draw your profile with the 0.005 R included, and tell it to take a finish pass with a tool defined to have a 0.03 nose radius. Now the tool needs to fit in the slot (which was why I suggested using the grooving tool if it can cut on the sides), Otherwise you might need to use both left and right hand tools for the appropriate corner.

TeachMePlease · Aug 3, 2021

M Code said:
Thank your for your reply

In fact I am not talking about the R value inside the groove I am referring to the above two edges of the groove need to be 0.005R just to break the sharp edges. How that can be done?

Trust me, I'm not the one who didn't understand the question.

Edit: That was rude.

Any OD radius can be created by any OD radius tool by programming a radius that incorporates the radius of your turning tool as well as the radius you wish to create on the part.

angelw · Aug 3, 2021

M Code said:
Thank your for your reply

In fact I am not talking about the R value inside the groove I am referring to the above two edges of the groove need to be 0.005R just to break the sharp edges. How that can be done?

Hello M Code,
They are external radii, therefore, as TeachMe suggests, they can be cut with a any tool nose radius of a tool that will fit inside the groove. It's very common to rough the groove and then finish the profile of the groove, including external corner radii with each side of the grooving tool, taking into account the corner radius of the grooving insert.

When actually executing the finish pass you have to be mindful of the feed rate being used in the area of the corner radii. It needs to be less than the corner radius, otherwise it could be missed in one revolution of the part. The feed rate has to be substantially less than the radius feature being cut so as to cut that feature accurately.

Following is example code to cut a 0.25" wide by 0.25" deep groove 1.0" from the end of a 2.0" diameter shaft, using a grooving tool with 0.03" corner radii. The groove has 0.005 external corner radii.

When using each side of a grooving tool to finish a groove and particularly if the sides of the groove have tolerances, its good practice to use a tool offset for each side of the insert. Doing so allows for the position of each side of the groove to be controlled.

G00 X2.0400 Z0.5000 T0101 (TOOL OFFSET FOR FRONT SIDE OF INSERT - TOOL STYLE 3)
G01 X2.0400 Z-1.2300 F0.50
G01 X1.5100 F0.005
G04 X0.25 (DWELL 1/4 SEC)
G00 X2.0400
G00 Z-1.2850
G01 X2.0000
G02 X1.9300 Z-1.2500 I-0.0350 K0.0000 F0.002
G01 X1.5000 F0.005
G01 Z-1.2400
G00 X2.0400
G00 Z-0.9650 T0121 (TOOL OFFSET FOR BACK SIDE OF INSERT - TOOL STYLE 4)
G01 X2.0000 F0.010
G03 X1.9300 Z-1.0000 I-0.0350 K0.0000 F0.002
G01 X1.5000 F0.005
G01 Z-1.0100
G00 X2.0400

Regards,

Bill

SeymourDumore · Aug 3, 2021

OK, so my way of doing this ( multiple times a day even ) is to pick up your grooving tool with 2 separate offsets.
Offset #1 is Direction 3, which will be doing the back side of the groove.
Offset #2 is Direction 4, and will be working on the front wall of the groove.

As far as the Radius of the grooving tool, any size R will do the external radius on the edge of the groove, but in order to program it accurately and without overcut
your limiting factor here is the inside radii of the groove for the tool Rad.

Nerdlinger · Aug 3, 2021

You would only need a small radius corner tool (.005” or smaller) if that .005” dimension was an INTERNAL corner. Since it is an EXTERNAL corner you can do it with any radius tool….think about facing and chamfering/radiusing the front of a part with a turning tool….any nose radius can produce any chamfer/radius on the front edge of the part. Your CAM software really should allow you to enter in the corner rad of your grooving tool as well as apply the .005” edge break with no problem. Good luck!

wheelieking71 · Aug 4, 2021

The controlling factor here is how the code is generated.
Are you programming with CAM software? Or are you manually writing code?

angelw · Aug 4, 2021

wheelieking71 said:
The controlling factor here is how the code is generated.
Are you programming with CAM software? Or are you manually writing code?

Why so? An external corner radius is an external corner radius and a tool nose radius is a tool nose radius, with neither of them changing irrespective of the method used to create the program.

alphonso · Aug 4, 2021

My Cam program puts out tool path like this. Red dot is the reference point of tool.

CarbideBob · Aug 4, 2021

On caveat when programing this small of an entrance rad.
If the OD was not cut by the same tool and that OD is say .002 oversize or undersized you end with rather poopy blend be it a notch in the OD lots or rad missing.
A workaround is to only program 80 to 87 degrees of rad swing,
A form tool made to cut this as a second op will have at least 2 and as much as 8 degrees outwards on this rad for this reason dependent on expected OD tolerance.
Life is so much easier if the same tool did the OD work.

Other as Bill has said is feedrate. You have to go way slow around this corner or it will not be there. This is not a machine response thing but a sort of threading action of the cutting tool.
If feeding .004 per rev using a 0 rad tool... that .005 rad is not there. Or is sort of there. Rotate the part, check it again and many confusing things.

These small rads are a pain. Note also that this the remove burr idea so programming in the plunge cut may not do what is asked for.
This dance best done after the groove to size.

There is no zero rad cutting tool once it sees a cut.
Bob

wheelieking71 · Aug 4, 2021

angelw said:
Why so? An external corner radius is an external corner radius and a tool nose radius is a tool nose radius, with neither of them changing irrespective of the method used to create the program.

I guess my wording could have been better.
Maybe I should have said: "the controlling factor of the answer to your question" treating the question more of a how-to, than a yes/no.
My bad for being vague (very, LOL).
The simple answer to his question we all know is "NO".

Fancuku · Aug 4, 2021

There is no tool with zero nose radius.
When you program the finish move you need to add the .005 radius value plus the radius of the groove tool. Lets say the tool has a .007 nose radius so your R value will be R0.012.

CarbideBob · Aug 4, 2021

Fancuku said:
There is no tool with zero nose radius.
When you program the finish move you need to add the .005 radius value plus the radius of the groove tool. Lets say the tool has a .007 nose radius so your R value will be R0.012.

One may need to tweak be it called out .007 or .03125 rad on the cutting tool when making a .005 resultant.
I make cutting tools and insets. Lots of true to form and location things happening here.
It works in the CAD and on paper. Not so much real world let alone checking that .005 rad and lead/end smear or tangent.
I know it is corner break but if needed to hold or will be checked........
Option two is a tool ground to do it in a single plunge and no fancy G-code. In/out done. But at .005 corner I would not quote this.
.006 sort of the bottom in carbide and it will wear to a .007. In PCD one can go smaller.
Bob

elbowgrese · Aug 6, 2021

Can you really measure that 0.005 after you machine it? Probably someone is making fun of you.

Do I need tool with 0 nose radius to do that?

Aluminum

Diamond

Plastic

Aluminum

Cast Iron

Diamond

Aluminum

Cast Iron

Diamond

Diamond

Diamond

Stainless

Diamond

Diamond

Titanium

Diamond

Diamond

Cast Iron

Diamond

Plastic

Similar threads