face grooving

[JayMan]

Looking for some help on face grooving with mastercam lathe,,,I have a groove in the face of the part that the od dia is 2.129 the id is 1.379,

the depth from z zero is Z-.657, and there is a full radius in the bottom of the groove.my tool is a face grooving tool that has a .158 dia ball on it and can be plunged into the face at an od dia of 1.89-2.36 and then work in both directions.

 

I'd sure appreciate any help, thanks

[Trevor Bailey]

Try using the groove style CHAIN. More than likely, you will be better off with simply using a rough/finish contour toolpath so that you can side turn and finish in one particular direction.

[pno]

Send me the file by email and I try to help you.

[chris m]

Trevor is on the mark in my opinion. If you chain the groove and pick 'bi-directional' for roughing you will probably be in your '1st plunge' range on the initial move. The bi-directional path takes a little longer than a single-direction path but balances insert wear much better. If you want to take a couple three steps down [i would with that groove depth] you can select 'Depth Cuts' and 'ZigZag between depths' if you want to use a unidirectional cut and still balance out the wear. If, for some reason, the initial move is not in your diameter range you will be forced to create a dummy groove wall to force the tool to plunge at an acceptable X value.

 

Note to the Product Development Guy: a user-definable 1st X value would be a sweet addition to MC Lathe for facegrooving

 

C

[McRae]

Note to the Product Development Guy: a user-definable 1st X value would be a sweet addition to MC Lathe for facegrooving

 

Chris - This is right on,

 

PDG - From a tooling perspective, the trepanning style of a face groover requires a specific diameter to start at to avoid heeling out on the support for the insert. Check out some tooling catalogues to be your guide when making the enhancement.

[EZ3PUTT]

Jay,

check your e-mail.

[JayMan]

Thanks guys, I finally got it, thanks for the support....

[FNU]

Hi Guys,

I am facing the same problem in mastercam. Not able to program for face grooving. I followed the above instructions, but then also it shows the message "ERROR MAKING TOOLPATH"

I have a groove in the face of the part for which the od dia is 3.975 the id is 3.6525,

the depth from z zero is Z-.068, and there is a full radius in the bottom of the groove i.e. .031. My tool is a face grooving tool that has a .125 wide insert on it.

Please help me out with this

100-4000-161.PDF

[Elmer Fudd]

I don't think a .125 tool will fit in that groove.

[FNU]

So what do you recommend using???

[Guest]

6 minutes ago, FNU said:

So what do you recommend using???

Something that does fit?

[crazy^millman]

5 minutes ago, FNU said:

So what do you recommend using???

A tool that will fit. You have a .031R which mean you need to use a tool that is smaller that .031R. Look to Kaiser Thin-Bit or PH-Horn they both have a good selection of smaller tools that will handle this project. Kaiser Thin Bit will even call out the bit and holder you need from that print.

[Elmer Fudd]

Maybe you could profile it with a thread tool type of cutter.

[crazy^millman]

7 minutes ago, Elmer Fudd said:

Maybe you could profile it with a thread tool type of cutter.

You would have to kick the tool at an angle to not hit both faces.

[FNU]

Thanks all for your support.

Can i use a Neutral turning tool with VNMG-331 insert and grind underneath so that the shank doesn't touch the face of the part.

What do you suggest?? 

[crazy^millman]

2 hours ago, FNU said:

Thanks all for your support.

Can i use a Neutral turning tool with VNMG-331 insert and grind underneath so that the shank doesn't touch the face of the part.

What do you suggest?? 

Sure just need to make sure the bottom doesn't rub.

[FNU]

Thanks for your support.