How do you handle internal sharp corners?

[bhayden10]

I have a 1" thick piece of 6061 tooling plate with a 6"x8" window with .125 internal corner radiuses. I usually would pocket this out but read here where some of you contour the slug out and would like to try that. (is countour ramp good?) What methods do you guys use when pocketing or contouring aluminum when the internal corner radius is .125? I run into this all the time, some parts are boxes with 3" walls, with them I usually rough with a carbide 3/8 3 flute and finish with a carbide 2 flute 1/4 but have problems with chatter in corners trying to run a decent feedrate on the flats but the sudden direction change is obviously not good. I have been leaving about .03 on the walls, then restmill to within .01 stepping down .125 and finishing with a slow feedrate (2000 @20) steping down about .75 The change at point feedrates don't seem to work because there is only a point there for it to change. Sorry for the long post, but I know there are some great machinist on here and would like to see if there are other options for this.

Thanks.

[Guest]

Brian,

 

Absolutely, drop some screw holes in where the slug will be and like you said use contour ramp to clear it out.

 

Sometimes on deep small internal radius callouts you might conventeional milling the corners.

[jeff]

quote:

---

drop some screw holes in where the slug will be and like you said use contour ramp to clear it out.

---

+1 to John,

2 tie down holes are needed.

I remember the first time that I only put in 1 bolt hole....hahaha the endmill broke rather quickly

[bhayden10]

Thanks for the info, what angle, speeds and feeds would you use on that? (3/8 3 flute alumimill) It defaults to 3 degree's is this good? I would guess I won't be able to go as fast as normal since there is the corners to deal with but i've never used the contour ramp process, it looks good though.

[Guest]

3 degrees is generally a good number that I use, most hi helix cutters are designed to cut on a 3° ramp. Some even greater, I've seen 11°

[Thad]

quote:

---

The change at point feedrates don't seem to work because there is only a point there for it to change.

---

You could always create a radius.

 

Thad

[Surface]

Turn it into chips....The time saved by ramping that type of pocket is outweighed by other factors.

A 1/2 inch endmill will pocket all the material in a conservative 3 minutes. Compare that with drilling two holes, screwing in two bolts, ramping and then removing two bolts. Add additional programming and setup and you have spent more time per part. Additionally, it was necessary to stand at the machine resulting in further downtime.

For the small radius, try to plunge the corner first with a low rpm, say 400rpm, will eliminate any chatter.

[Jerosu]

Or you could drill out the corners first. Then use the endmill to clean up the "cusps" that are left.

[mowens]

I would finish with the 3/8, then finish each corner with the 1/4".

[Fig sign]

You could always create a radius.

~~~~~~~~~~~~~~~~

+1000

iT IS ALWAUS A GOOD IDEA TO CREATE radius a bit bigger .

Thus the tool will not stand still in walls always

stay in move

Very important for deep roughing

If you use rough mill 12 mm diameter rad 7 is good enough

Now if you drill entarance hole start your toolpath from it not a big deal ,but saves lot`s of pain

You can drill the corners too ,but I see no need in it

Two bolts holding the part is a big timesaver and

I use it all the time when possible

You can hide bolts head inside the part with ctrsnk .

This is very trivial stuff and it`s up to you to decide

If you made a eough contour and finish mill chatters no matter what you do step aside 0.2 mm

and drill the corners out with mill before finishing

Do not be afrais to go down with rpm

For long nonrigid mills reduce of speed can be up to 200-300 percents and more

I usually drop feed radically ,reduce speed on the nachine till chatter goes out and add feed

let `s say that I mill with end mill 6 mm 7000 rpm and 1200 mm/min (very usual speed /feed )

When milling with long mill like 70 mm length

I can go down to s2000 f300

Or will mill in conventional direction

In any case I will provide the small but possible radius

Everything has tollerance ,so rad 3.1 instead of

r3 will dounrate chatter a couple of times even without feed drop

Also you can use highfeed and slow down your feedrate in corners

[mcpgmr]

quote:

---

Turn it into chips

---

I agree. Also in this case I would drill the corners leaving .01 to.02 and use a e.m. to plunge them to fin size or create special geometry for contouring the corners in a step down fasion with a radial lead in and out. Use the largest dia e.m. you can fit in the pocket for finishing the walls but not too large that you will have a lump of material on either side of the corners to deal with when finishing the corners. I do this all the time. the majority of the parts we make have real deep blind pockets with .06 to .12 corner radius's. Wire EDM is always an option if the pockets are thru and the customer allows it. HTH!

[Fig sign]

Turn it into chips....The time saved by ramping that type of pocket is outweighed by other factors.

~~~~~~~~~~~~

It depends

Sometimes it is a great thing

I milled monel part with Hanita varimill constant

RAMPING INSTEAD OF DRILLING THE PART LOOKED

like a big ring with holes on outer diameter

We did it in 4 axis

The spindel load when drilling was HuUUUge

The drill used to break any time

Varimill worked great

[jeff]

quote:

---

Varimill worked great

---

I love these endmills!!!!

[bhayden10]

There are always several ways to skin a cat. Thanks for all the input, I really enjoy reading threads about how guys go about making parts. I have learned a ton from this forum, I would be lost without it.

[specv]

I would turn it to chips and finish with a 6MM(.236) DIA EM then you are actually creating the rad with the code not the tool. When a small EM hits a full corner it will chatter. its much easier to contour it. I would also drill the corners out beforehand.

[Guest]

quote:

---

There are always several ways to skin a cat.

---

Hey, hey, hey, there is a lot of skinning the cat talk going on around here.

 

A puddy tat "might" get the impression these ain't safe waters to be swimmin' in.

 

[bhayden10]

You better play nice John or you could end up looking like this...