MC Lathe Threading

[jeff]

Can anyone tell me if MCLathe can machine a profile thread form?

I will be using a 35 degree insert .0313 radius to cut a rope style thread that is approx a 1/2 radius thread.

The thread is used on a crane to hoist 1" round cable up and down.

Please HELP!!!

[roy g. biv]

Jeff,

Do you mean a thread shaped like the grooves on a ballscrew?

I don't think that MC will be able to do that with a .031rad tool. You may need to use a .5rad tool. Or if you have a c-axis with live tooling it could be done using a ballnose endmill.

[jeff]

Yes, that's the type of thread I need to cut.

I would have to make multiple cuts,and the move in for each cut,the tool would actually move on a

small portion of that radius.

 

Hey, roy g biv..... the 7 colors of the spectrum,very cunning.

lol

[Keith Graydon]

10 BIG points to anyone that knows the name of this style of groove!

 

You may be better off milling with C-axis on a lathe or 4th axis on a mill if you've got those capabilities in your shop

 

KLG

 

[ 08-26-2002, 07:33 AM: Message edited by: Keith Graydon ]

[jeff]

Sadly, I only have the standard 2 axis lathes.

I give up Keith,what's the name?

I know it but can't think of it.

[McRae]

Use the cross section of the groove, and break the spline into many pieces. Use finish toolpath and disable arcfitting. If you can write a custom post macro for this then great but if all else fails, manually insert between each end point, moves to generate the thread (ie G32).

 

Watch the pitch though as the acceleration distance is going to give something wonky at the start.

[Keith Graydon]

Lebus groove!

 

anyway, you could define the radius profile and plot points along it.( you would need only 90 degrees of it 'tho)Then,knowing the pitch of the groove, you could chase each point along the drum diameter. Or. if you lathe is REALLY rigid you could use a single form tool or several form tools and blend the sections together.

 

HTH

-KLG

 

I like Andrew's solution too.

 

[ 08-26-2002, 08:36 AM: Message edited by: Keith Graydon ]

[jeff]

Thanks guys,

I'll try that.

UGH!

not looking forward to it though.

[McRae]

It actually is a technique from Glenn, I am massaging it and making it elegant for my own use.

[Guest CNC Apps Guy 1]

gstephens, bring back any memories???????

 

They'd probably have to do it the same way huh?

(sorry folks, inside joke)

[gstephens]

quote:

---

gstephens, bring back any memories???????

---

AAAAAHHHHHHHHHHHH!!!!!!!!!!!!!!!!!!!!

 

quote:

---

They'd probably have to do it the same way huh?

---

Buy a Mazak C-axis lathe (or sub out the job to someone who has one already). They have a REALLY cool function (G1.1) that is used for C-axis threading. X,Z incremental motion through n revolutions of the C-axis (and at 400 RPM no less) too cool. No way to program it in Mastercam though (I wrote a WAY custom post for this one).

[McRae]

What machine and what control?? I am limited with the mazak to 18 rpm C Axis.

[Guest CNC Apps Guy 1]

It was done on an Integrex 45 (I think) with a Mazatrol Tplus Control, but it can be done on any Mazak Lathe that has a C Axis and the G1.1. I'd estimate that this thing would take you about 4 hours to cut at 18 PM.

 

Another option you have is to run it on a mill with a rotary table on it(which would be my personal preferred method for what it's worth), do rotary replacement using a flowline toolpath and turn off ALL the gouge checking. You can't verify it but you can use backplot to check things.

 

JM2C and HTH

 

[ 08-26-2002, 03:34 PM: Message edited by: James Meyette ]