I've done many holes similar to the one you need to do. My mill is will take 16mm cutters but is happier with 10 or 12mm where I can crank the speed up. I work dry, but set up a low pressure air blow to clear the swarf.

I sometimes remove the bulk of material on the drilling machine set with depth stop then transfer to the mill where I would use a relatively large cutter to get near finished size and then finish off with the size needed for the internal corner radii.

Ian P

Your machine is the Warco equivalent of my Clarke mill….

My preference would be to hack out the middle with a 12mm end mill vertically – Like chain drilling – to within 1mm of all edges.

Fit a 6mm end mill and and plunge mill on the 4 corners leaving about 0.2mm on each edge. Machine one end of the pocket to the edge of the plate finished, the same to a perpendicular edge. Then machine the slot to width both ways. This method means that you don't have a problem with backlash. Then clean up the bottom face.

By roughing out vertically it prevents swarf clogging the tool and the machine is more rigid than winding bed handles.

Trevor

Probably more risky breaking through endless drilled holes – you'll get some hairy transient loads on the cutters as they break through, which would be difficult to control and could prove expensive. I'd simply mill it the way Gary suggests, stepping down in stages and conventional milling ie working round clockwise to open it to the final dimensions.

With a bigger machine, you'd be able to climb mill the finish (for a better finish), having roughed it out in one pass. It's also worth using slot drills designed for aluminium cutting (faster helix, better cutting angle etc). Roughing (hogging) cutters allow you to remove material a lot quicker and are worth investing in – in my books at any rate. And I'd use WD40 if using steel cutters.

Murray

Hi Steve ,

I'm curious as to how you are going to hold the piece ?

If you are going to clamp it in a vice then be mind full that as you remove material it will weaken it and it may flex and if you are going to clamp it down to the table check it is not twisted by giving it a rub on some emery cloth or the like on a flat plate – something that has been machined or ground will do like a drill press table , mill table or surface plate , if it is twisted and you clamp it down it will twist again when you release it .

if you can leave it a little long say 20mm each end and clamp it down to the table with 4 clamps and against a fence I would do it this way and trim it to size last .

I would blue it up, mark it out ( height gauge and surface plate if you have&nbsp rough it out to full depth with the biggest slot drill or centre cutting end mill( if you have one ) that you feel comfortable working with leaving .5mm on all inside surfaces except the bottom as it is cut to full depth . Clean up the rest with the 6mm cutter.

I find wd40 not too bad as a cutting fluid on aluminium and tap magic is good as well .

If you don't have a DRO on the mill a couple of cheapie long travel dial indicators could be a good investment as they allow you to move the table around irrespective of how much backlash your machine has , just set one on the y axis and the other on the x axis and you have a poor mans DRO good to a thou or so at least !

That's my slant on things anyhow !

Ian

Edited By XD 351 on 14/11/2014 03:41:22

Steve, I'd drill the corners to depth first, then change to the 12 mm , but use a slot drill here too it gives more clearance for swarfe removal. I'd take 3 x 5 mm deep cuts, check the depth take perhaps a 4 mm deep cut, and finish with a 1 mm cut, maybe a bit faster if possible, or a slower feed.  Finish into the corners either with the 6 mm cutter, or do it by hand with a little chisel.

Ian S C

Edited By Ian S C on 14/11/2014 09:01:02

Steve,

I have to admit, that doesn't leave you much metal at the end, take care it doesn't distort under milling forces when near the end.

I would fit a big slot drill, hitch up my belt and rough out the middle, then finish with a 6mm end mill.

Or buy a suitable box from CPC or RS

Neil

The tolerance of +/- 0.1 mm is asking a lot (for me anyway)

Have you got any stops you can set up on x and y ?

Set them up on a test piece to your sizes and you can do it without looking

> Careful if using ER collet cutter may drop unknowingly or cut a taper, used to cop us out at work.

I've been caught by this a couple of times. Really pays to lubricate the collet (outside) and tighten as much as you can.

But I'm starting to think of getting a clarkson type screw-in cutter holder.

Neil

Maybe I have been lucky but I have never had a cutter move, trouble with the 'tighten as much as you can technique' is that it depends on the users interpretation. Maybe some data exist that gives torque settings for every diameter of collet (and type of nut), but sticking the routine would take up too much time.

I think one has to have a degree of mechanical sympathy here, I tighten my nuts by feel, Its pretty obvious when all the springiness and clearance has been accommodated. After that point the nut just needs a good talking too, whatever happens it not going to rotate very far as all the contacting surfaces are pretty hard.

Ian P

Neil have you tried one of Ketans bearing collet nuts ? You can tighten the nut more with the same effort.I have not had problems with cutters creaping

Thanks – I didn't know that.

I'm an old schooler and would be happy to stick with 'typographic smileys' and no silly pictures at all

neil