What's new
What's new

Need help with radius grooving.

valterroque

Aluminum
Joined
Nov 13, 2017
Hello, Self learning cnc lathe and I need help/advice on which tool and cycle to use for "grooving" a Radius.
Control Fanuc OiT
Machine Kia SKT 200.
Thanks in advance.
RegardsPolia.JPG
 
I would use a full radius grooving tool. Maybe 3mm wide. You can use G75 to Rough it out.

R

Humm... Thanks, I will look into it.

While i am at it, Can you please confirm that, to setup that type of tool for cutter comp on fanuc control i must use position 8 and specified the radius of of 1.5 for in this example Ø3mm full radius tool?
 
I would use a neutral tool holder with a 35 degree insert for that.
 

Attachments

  • lathetool.jpg
    lathetool.jpg
    10.7 KB · Views: 144
I would use a neutral tool holder with a 35 degree insert for that.

There weak and they suck unless your finishing only.


like bob said in his post or even a toplock full rad insert. plunge to rough then follow it with a finish pass.
 
Interference is not very obvious because the drawing is not to-scale. Actually, it is half circle! Only full-radius tools can be used.
 
Hello Fancuku,
You won't be able to use that tool and insert, as it will interfere with the Start and End area of the radius.

Regards,

Bill
You’re right. I just realized that it’s almost half circle. That tool doesn’t have the clearance to make that radius.
 
Using a full radius tool does not teach him what he wishes to know. Using a smaller radius tool enables him to create any radius groove [larger than the tool] that he wishes to.

Unfortunately I don't speak Fanuc
 
Using a full radius tool does not teach him what he wishes to know. Using a smaller radius tool enables him to create any radius groove [larger than the tool] that he wishes to.

Unfortunately I don't speak Fanuc

bobs 3mm was a full rad insert, I didnt mean a full rad insert the size of the part rad. ie a form tool.
you can get all kinds of sizes of full rad inserts.
 
Using a full radius tool does not teach him what he wishes to know. Using a smaller radius tool enables him to create any radius groove [larger than the tool] that he wishes to.

Unfortunately I don't speak Fanuc

Thanks Gustafson, can you explain wich tool. I am also under the impression that it (the half circle )may only be possible by using a round (full radius) tool.

I have a Sandvik lf123h25-2525bm tool available with parting inserts, however the round inserts for it are to expensive for me to make it a try.
Can anyone recommend a tool that takes cheapo round or other inserts? I was thinking about some MGEHL 2525.
Regards
 
Using a full radius tool does not teach him what he wishes to know. Using a smaller radius tool enables him to create any radius groove [larger than the tool] that he wishes to.

Unfortunately I don't speak Fanuc

As suggested earlier, make a rough shape by calling G75 multiple times, shifted sideways suitably and modifying X value every time. This to be followed by a finish cut with radius compensation. Actually, a tedious method, but can make the part.
 
As suggested earlier, make a rough shape by calling G75 multiple times, shifted sideways suitably and modifying X value every time. This to be followed by a finish cut with radius compensation. Actually, a tedious method, but can make the part.

It is tedious. Were it me, I would just long hand 3 or 5 Rough passes from the OD, then a Finish pass. I wouldn't use G75 for such a small Groove.

R
 
With a cnc one just goes in and profiles it.
A 1/8, 3/16, or 1/4 inch full nose tool works.
You do not show the rad inside dia. but it looks awful close to what a "V" insert can cut in a flat axial rake.
Anyways you want to have a vee bottom or other groover in your collection of toolholders.
If making 5,000 or more I'd just buy a custom tool to plunge and done. None of that cnc dancing around lost time.
 
If making 5,000 or more I'd just buy a custom tool to plunge and done. None of that cnc dancing around lost time.

Hello Bob,
That's a frag over 6mm deep with a 14.16 diameter tool, equating to a bit more than 20mm contact between insert and workpiece. Good luck with that.

Regards,

Bill
 
Lol;, that's not even a inch wide plunge cut.
Bob
Hands up all those that have taken an inch wide plunge cut in other than plastic, on your typical sized Turning Centre found in most machine shops, not built like a Brick Shit House (typical of a Kia SKT 200), and could still hear the radio over the chatter.
 
I have no experience of machining with round inserts. Therefore, i have a question. Can it be used for usual turning operation with, say, 0.5 mm DOC and 0.2 mm/rev feedrate?
If yes, at least for large diameter jobs which can withstand the associated radial thrust, then G71 type 2 or G73 can also be used for making the groove.
 
I have no experience of machining with round inserts. Therefore, i have a question. Can it be used for usual turning operation with, say, 0.5 mm DOC and 0.2 mm/rev feedrate?
If yes, at least for large diameter jobs which can withstand the associated radial thrust, then G71 type 2 or G73 can also be used for making the groove.
Hello Sinha,
Absolutely, but with a whole lot more Feed/Rev. 0.2mm/rev is conservative roughing feed rate with a 0.8 TNR and a much greater DOC.

I took over 30 minutes out of a client's 60 min. cycle time on a large, deep face groove using a 12 diameter button tool, using 0.5 DOC and 3.0mm feed/rev to bi-directional face. Basically, its the same principle as HSM common to Machining Centres, implemented on a Turning Centre. I've also used the same technique in OD turning operations.

The slow feed rate you suggested would result in bird nest swarf.

It would be difficult to use with a Multi-repetitive cycle, as the indeed for the DOC can't be anything near like the feed/rev used in a Turning, or Facing operation (only one Feed Rate can be specified in these Roughing Cycles)

Regards,

Bill
 








 
Back
Top