Milling a pocket

[stragenmitsuko]

I seem to have a minor problem when milling a pocket , or better a corner .

This is a pretty deep pocket, 58mm ( 2 1/4 ") and I'm using a very long 10mm
endmill . I need to use that small diam endmill , cause later on the part will be reversed and the rounded corner removed .

I make a U shaped cut , conventional milling . After each pass , the cutter is lowered or better the table is raised 5mm for a next pass .
This is a casting so I'm only cleaning up the edges . Abt 3 mm (1/8" ) to remove from the sides . It varies cause my casting isn't perfect .
In the corner the cutter seems to flex , an instead of having a nicely chamefered corner I'm getting something that looks overcut .
The part is good and fuctional , but I just don't like the look of it .

If this was solid material being carved out , I would drill the corners first 0.5 mm from the edge and then mill it . Then I don't have this problem .
But as this is a casting that won't work .

Any tips or tricks to avoid this .

Pat

 

[Nick Hulme]

You can peck plunge cut your corners with a centre cutting end mill.
Direction of cut changes how the cutter pulls at the corners and reduced contact, i.e. shallower cuts, will reduce cutter deviation.
You can use a cutter with much shorter flutes if you reduce the shank by a few thou from the end of the flutes to the cut depth.
If you're not already using carbide it might be worth trying for it's increased rigidity and single flute end mills are great for profile cuts in aluminium.
If you're not already use air or flood to clear chips.

- Nick

 

[Jasonb]

I'd take less of a cut say 2.5mm deep per pass so the cutter will not be removing as much material and therefore won't deflect as much.

Also cut the pocket say 0.2mm under size then go back and cut to finished size which could be done in 5mm steps.

This one is also 10mm cutter, 52mm deep. I bored out first then just went round and round teh edges size of cuts as above. Dab of parafin and a sharp cutter

Boring

Milling

And what the inside finish came up like

 

[purpleknif]

Drill the corners 1st staying perhaps .010" away from your finish dim and staying off the bottom. use a flat bottom drill (easily ground) to finish the bottom.
Rough the pocket, Then plunge corners to finish with the end mill. then finish the pocket with the end mill.

 

[kwoodhands]

Is your endmill center cutting? I had similar problems til I realized the long cutter I had was not center cutting.
Mill with a regular length cutter ,switch to the long one. Make sure the long cutter reaches the bottom of the slot in one pass. Looking at the pic the cutter may not be center cutting. Not positive from the pics.
mike

 

[ShopShoe]

Perhaps a roughing cutter first, then clean it up.

--ShopShoe

 

[gbritnell]

While coventional milling has it's place cutting into a corner isn't one of them. As has been mentioned I would plunge the corners out, staying away from the finished number and working my way in. Once you have the corners where you want them climb cut the walls going into the corner. This way the cutter will want to climb away from the corner rather than pulling itself into it.
gbritnell