What's new
What's new

16mm Wide Thru Pocket/Slot 2.85" Deep in A36; Reconsidering Tooling

SeymourDumore

Diamond
Joined
Aug 2, 2005
Location
CT
I would avoid the drilling also, just ramp down with a through air blast if you have it available.

There is one possible benefit of having a couple of holes.
Since they are through, there is a better chance of chip removal when the pocket gets deep.
IOW if you cannot blow them out, they might just fall through.

But then again, 225IPM for only 1.5" length doesn't give the chips too much of a head start....
 

dandrummerman21

Stainless
Joined
Feb 5, 2008
Location
MI, USA
So I finally got around to trying this yesterday before I left. I will say, it sounded great. It cut great.

BUT it also cut the slot oversize. It also doesn't look too pretty. Not terrible, but not as even as my boss would like and "chattery" near the ends (not actual chatter... kinda looks like a holograph? just a weird finish in general)

The print is old, there's no tolerance given, and I know what it is used for and sure the customer will accept this part. But we are trying for 16mm +/- .010, and the slot is about .645. I had programmed it for .635

To be honest, I'm surprised it cut oversize? I'm climb ramping down, 4000rpm, 120ipm, it was either .015 or .020 per lap around the slot. I would have expected deflection to work away from the walls, not suck them in.

Unless it is deflecting so much that it actually digs into the opposite wall? However I see no evidence of that on the break through, where the slot is still oversize. I may try some positive cutter comp and program it to go a shallower depth to see how it is reacting to it.



So I'm thinking of getting a 1/2" solid carbide feedmill instead. Still have other things to do so this may go on the backburner for another couple weeks.
 

dandrummerman21

Stainless
Joined
Feb 5, 2008
Location
MI, USA
Actually found out after looking at the inserts this morning, that one of the inserts came loose.

That's why it is oversize. Insert edge still looks great though.


Clearly the pocket is too damaged for the insert. I'm gonna try hitting it with a punch to bring the bottom of the seat up a few thou so there' more positive clamping on the insert. Will probably order another one of the same tool if I can verify it will not cut oversize.
 

TeachMePlease

Diamond
Joined
Feb 11, 2014
Location
FL
Actually found out after looking at the inserts this morning, that one of the inserts came loose.

That's why it is oversize. Insert edge still looks great though.


Clearly the pocket is too damaged for the insert. I'm gonna try hitting it with a punch to bring the bottom of the seat up a few thou so there' more positive clamping on the insert. Will probably order another one of the same tool if I can verify it will not cut oversize.

If you have a tooling rep that you do decent business with, you oughta be able to explain your situation and get one in on a Guaranteed Test Order. If it works, you buy it, if it cuts oversize or doesn't perform, the rep takes it back and doesn't charge you anything.
 

dandrummerman21

Stainless
Joined
Feb 5, 2008
Location
MI, USA
Well the 5/8 tool did work pretty well. I got the pocket back into shape, and it was cutting to size. But about 4 parts in the loose insert must have loosened again and blew up. It was cutting to size, purred along very well.

Now I'm at the question of buying the same (but longer) tool I just had, or get a screw on head, or possibly solid shank one.

This job will again hit the backburner now. We've got plenty enough for current orders. But I am pretty determined now to change it to feedmill. Because it was glorious sounding, and cuts about 15-20 minutes of cycle time per part. Totally worth it.

I'll post again when I get something figured out and running.
 

gregormarwick

Diamond
Joined
Feb 7, 2007
Location
Aberdeen, UK
Well the 5/8 tool did work pretty well. I got the pocket back into shape, and it was cutting to size. But about 4 parts in the loose insert must have loosened again and blew up. It was cutting to size, purred along very well.

Now I'm at the question of buying the same (but longer) tool I just had, or get a screw on head, or possibly solid shank one.

This job will again hit the backburner now. We've got plenty enough for current orders. But I am pretty determined now to change it to feedmill. Because it was glorious sounding, and cuts about 15-20 minutes of cycle time per part. Totally worth it.

I'll post again when I get something figured out and running.

Maybe I missed it, what tool did you have?

My favourite small feedmills are Tungaloy dofeed.
 

dandrummerman21

Stainless
Joined
Feb 5, 2008
Location
MI, USA
Maybe I missed it, what tool did you have?

My favourite small feedmills are Tungaloy dofeed.

I had a wounded (previously crashed) 5/8 feedmill from iscar. it was only 2" long but I ground the shank back so i had 2.9" stickout.

After discussing with my boss, we bought another, 3 inch version. https://www.iscar.com/eCatalog/Item.aspx?cat=3105629&fnum=2793&mapp=ML&GFSTYP=I&srch=1

We've had nothing but good results with these tools on larger versions, just trying to dial in this smaller one.


While I'm here, some other suggestions would be appreciated. here is a snippet of the code for this tool:

Code:
 O6003( FEEDMILL SUB 5/8)
 G0 X-.6748 Y.0582 S4000 M3
 G0Z.1
 G1Z0.F50
 G41 G1 X-.6768 F120. D87
 Y-.4699 Z-.0055
 G3 X-.6668 Z-.0057 I.005
 G1 Y.4699 Z-.0155
 G3 X-.6768 Z-.0156 I-.005
 G1 Y.0582 Z-.0199
 Y-.4699 Z-.0254
 G3 X-.6668 Z-.0256 I.005
 G1 Y.4699 Z-.0354
 G3 X-.6768 Z-.0356 I-.005
 G1 Y.0582 Z-.0399
 Y-.4699 Z-.0454
 G3 X-.6668 Z-.0455 I.005
 G1 Y.4699 Z-.0553
 G3 X-.6768 Z-.0555 I-.005
 G1 Y.0582 Z-.0598
 Y-.4699 Z-.0653
 G3 X-.6668 Z-.0655 I.005
 G1 Y.4699 Z-.0753
 G3 X-.6768 Z-.0754 I-.005
 G1 Y.0582 Z-.0797
 Y-.4699 Z-.0852
 G3 X-.6668 Z-.0854 I.005
 G1 Y.4699 Z-.0952
 G3 X-.6768 Z-.0954 I-.005
 G1 Y.0582 Z-.0997
 Y-.4699 Z-.1052
etc..


I have seen the suggestion in this thread about just zig-zagging it back and forth down the center. Would that be better than my current "racetrack" ramp down? And I assume if I did that, I'd be wanting to go down about .010" each way so the cut would be .020" deep by the time it reaches the other end of the slot?

Or should I keep the racetrack path? And should I keep the same depth per pass that I have? While I am going down .020" per lap, it is basically just a .010" depth of cut because the slot is so narrow. So should I double my depth?

For reference, iscar's recommendation is .020-.031" depth of cut and .027-.040 ipt. 400-650sfm


Now that I'm writing that, I realize I've programmed the rpm too high and the chip load too low for the rpm. Maybe I should be running 3000rpm at 162ipm?


Sorry for so many questions. Totally don't wanna crash the good tool when it gets here lol.
 

Rick Finsta

Stainless
Joined
Sep 27, 2017
I will use the "Racetrack" ramp contour method every time if given the choice. I always prefer to have that extra bit of chip clearance.

Are you getting any chip welding on the shank or hole sides? I have that happen if I don't take enough out of the shaft when clearancing back and it can make some awful noise and chatter marks like you describe.

High feed always leaves a chatter-ish side wall finish in my experience, and usually floor finish as well unless you baby it.
 








 
Top