Flat Grooving (Also known as Hale Machining)

[TSmcam]

Anyone encountered this?

Apparently really good for cutting high quality face grooves with a good finish. I'd never heard of it until I saw it as an option on an Okuma mill.

[SuperHoneyBadger]

I would love to see this in action! Always fascinated me, and one of the processes I think about on my days off - sometimes from the perspective of the cutting insert, just touring around the part making a funky gasket groove.

[TSmcam]

I would love to see this in action! Always fascinated me, and one of the processes I think about on my days off - sometimes from the perspective of the cutting insert, just touring around the part making a funky gasket groove.

I have a customer that machines small o-ring grooves with non uniform path (ie not a standard circular face groove). This process would be ideal for that.

I have access to a new Okuma horizontal later in the year that has this function. I'm very keen to try it out.

[SuperHoneyBadger]

I just had an order that needed a relatively tight elliptical groove with rads where the floor met the vertical wall (what is the vernacular for that section anyways? The floor fillet? The baseboards?). Got it licked with a .2MM bullnose since the machine is good, but I thought it would have been a great candidate for this process.

How is it programmed? Just like a contour, but with a lathe tool, and vectors to control spindle orientation during? Is this programmed at the machine?

[TSmcam]

I just had an order that needed a relatively tight elliptical groove with rads where the floor met the vertical wall (what is the vernacular for that section anyways? The floor fillet? The baseboards?). Got it licked with a .2MM bullnose since the machine is good, but I thought it would have been a great candidate for this process.

How is it programmed? Just like a contour, but with a lathe tool, and vectors to control spindle orientation during? Is this programmed at the machine?

In TopSolid it is programmed as a 2D contour, then Multiaxis is switched on, and the Hale Machining Multiaxis method is used.

I'm not sure how the offset is handled at the machine. I am waiting to get ahold of the latest Okuma P500M control to get the coding format.

[CNCAppsJames]

I've done a few projects with this function. First one was back in '98/'99 IIRC. We just called it by it's function; CsContour.

On a Matsuura, we define the tool as a turning tool in the tool manager. In there you define the center to comp edge value.

As far as programming... basically a contour, but I don;t have a post so I have to add in the W's to tell the spindle what angle to use or what angle to go to from point A to point B.

[CNCAppsJames]

...
How is it programmed? Just like a contour, but with a lathe tool, and vectors to control spindle orientation during? Is this programmed at the machine?

Here's a sample section of code;

G91G01X0.Y[-180./#100]Z[-0.5/#100]F[1000./#100]
G91G03X[37./#100]Y[-37./#100]Z0.I[37./#100]J0.F[2000./#100]W-90.
G91G01X[60./#100]Y0.Z0.F[1000./#100]
G91G03X[37./#100]Y[37./#100]Z0.I0.J[37./#100]F[2000./#100]W-90.
G91G01X0.Y[180./#100]Z0.F[1000./#100]
G91G03X[-37./#100]Y[37./#100]Z0.I[-37./#100]J0.F[2000./#100]W-90.
G91G01X[-60./#100]Y0.Z0.F[1000./#100]
G91G03X[-37./#100]Y[-37./#100]Z0.I0.J[-37./#100]F[2000./#100]W-90.

The MACRO ariables were so we could run it in inch or metric and it's incremental. Totally optional to do it this way. Absolute is totally fine too. Can run with G68.2 active.

W is the spindle axis. Every machine builder activates the function differently but basically you orient the spindle, activate the function then go at it.

[MIL-TFP-41]

At my previous gig in NY state we used this function on Okuma's. I believe it was/is called turn cut. We used it for cutting annulus grooves that were buried deep into a manifold. Before this function we had to use expensive (and very slow) carbide form cutters. Something like a 3/4" tool that hung out 7 or 8 inches. With turn-cut, were were able to use a off the shelf Sandvik devibe boring bar. Ran faster and gave a better finish.

[SuperHoneyBadger]

Here's a sample section of code;

When the routine is formatted this way, can it run on any machine? Or will I need options to use the W address for orientation?

Now hearing it has been done for decades, it doesn't sound so exotic!

[CNCAppsJames]

When the routine is formatted this way, can it run on any machine? Or will I need options to use the W address for orientation?

Now hearing it has been done for decades, it doesn't sound so exotic!

At bare minimum on a FANUC controlled machine you need the Cs Contour function (J852), also Spindle Serial Output J850, and an additional axis J802#x+1 and PMC Modifications from the MTB.

Not sure who coined the term "Hale Milling", but yeah, it's an old function that has new life.

Kern Machine made a big to do about the function on an IG post. I pointed out that the function has been around since the 90's on FANUC controlled machines. All some dude could come up with after that was "unfortunately everything about FANUC is stuck in 1990 as well..."

OoooooKaaaay

Tell me you haven't put your hands on a FANUC control since before the 30i Series Control which debuted in 2006.... without telling me you haven't put your hands on a FANUC Control since before the 30i Series Control which debuted in 2006.

[TSmcam]

At my previous gig in NY state we used this function on Okuma's. I believe it was/is called turn cut. We used it for cutting annulus grooves that were buried deep into a manifold. Before this function we had to use expensive (and very slow) carbide form cutters. Something like a 3/4" tool that hung out 7 or 8 inches. With turn-cut, were were able to use a off the shelf Sandvik devibe boring bar. Ran faster and gave a better finish.

This is different to Turn Cut. Turn Cut is effectively programming like a lathe, on a machining centre. Flat Grooving on the Okuma is basically "planing" a groove.

It is an interesting function, and it has some relevance to a couple of products I know of. I am very keen to check it out.

[Zoffen]

Groovy!

[Newbeeee™]

With this process, you can have way "rougher" surface finish but keep good sealing. Lay is important! - which reminds me it's nap time :yawn:

[TSmcam]

According to both TopSolid, and Okuma, it provides high finish. I can only assume they are using specific tools for this process. I'll have to dig a bit deeper

[Newbeeee™]

Yes - great finish because it's scraped/shaved etc - but most importantly for the seal, the surface lay is in the correct direction for optimal sealing. But if the finish wasn't so good (blunt tool etc), chances are it would still seal with no issues because of the direction of lay.