Best way to mill a pocket in Al on a manual mill

I have a piece of Aluminium 100mm long x 80mm wide by 25mm thick and I need to cut a substantial pocket in it using my round column Warco Minor (RF25/Chester Eagle variant) mill. It's happy with 12mm cutters, but much bigger gets to be an issue.

What is the most effective way of milling a pocket 95mm x 75mm x 20mm deep?

No corner must have a radius greater than 3mm and the tolerance on all dimensions must be better than +/- 0.1mm. The material is just off the shelf plate, nothing exotic.

It seems a simple task, but I haven't done this before and I suspect there is a best method.

Whats the expert view?

TIA

Steve

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

First thing, be careful about milling aluminium - some grades are very "sticky" and tend to build up on the cutting edges of tools. The usual advice is high speeds, but I've found just the opposite. I reckon the ali welds itself to the tool edge and higher speeds mean higher temperatures. I use slow speeds and paraffin or WD40 as a lubricant. Stop immediately if/when resistance is felt, and clear the ali buildup on the cutting edges before continuing.

To cut the pocket, I'd rough it out with a 10mm endmill, about 5mm deep at each pass. Then do the corners with a 6mm cutter (3mm radius), and then do a finishing pass all over.

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

Looks like the consensus is to chain drill out the pocket then tidy up!

Thanks

Steve

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

Don't use an end mill, they won't plunge cut. Use a slot drill. Anyway 4 flute cutters seem unhappy dealing with Ali on my Novamill, 2 flute slot mills seem much happier. I run them fast, lubricate wth mixture of cutting oil and paraffin, and quite fast feed. I think the solution to the Ali sticking to the cutter is to get it hot enough and fast enough it doesn't get a chance to stick!

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  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

Why does this web page add smiley faces to my post and then log you out so you can't edit them out ?

please ignore the little yellow mongrel winky thing as I didn't put it there and surely there has to be a way of turning these off permanently?

it would make a good target for sighting in my .303 though !

Ian

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

Hi XD,

It's the combination of some characters and a bracket - a pain, but it's built into the editor so the web designers can't take it out

Neil

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

I do similar all the time, as XD said rough it out with a two flute maybe 10mm dia cutter - 12mm pushing it a bit much with that machine though would take 19.4mm cutters, used to have one.

Use uncoated cutters and continually blow out the debris. Plus point very little coolant will be needed and will be contained within. Careful if using ER collet cutter may drop unknowingly or cut a taper, used to cop us out at work. General rule for aluminiums is you cannot have too much speed, people use 30000 rpm routers! As mentioned before get a feel for whats happening, you will know if the cutters doing its job, don't force it.

Once roughed near to size slap in a 4 flute long 6mm, check cutter flutes are at least 20mm. Downside is the cutter will flex so minor cuts to finish off to size climb milling (working anti clockwise) with bed locks nipped up will leave a good finish. Alternatively can use a long fluted 6mm with say flutes 10mm, shank will rub below that so keep plenty of coolant on.

Holding in a 4" vice will be more than adequate. Gripping force initially over the length to start with and will end up gripping on each ends 2.5mm = fine. Granted if using a 3" vice, around 5mm wall using 6082 aluminium it will start to collapse. If it moves then you tighten job back up, it will cut a taper.

Depth of cut passes you will have to suck it and see, key is get a feel for whats happening. ie if its tough going ease depth of cut off. You will hear the cutting change note when it starts to pick up and bind to the tool, this can be straight away or after several passes going down in depth. Aluminiums can be a right swine for binding up especially threads.

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

I'd stick it in the 4-jaw and turn a 74mm hole almost to depth as thats the quickest way to get most of the material out, then onto the mill 12mm cutter to take it out to 94x74, finally finish with a 6mm cutter.

Did a 40x 50 x 45 deep pocket a few months ago which would have been a long job on the mill but drilling 25mm followed by boring out on the lathe was quick and just finished with a long reach 10mm cutter on the mill

Edited By JasonB on 14/11/2014 16:30:56

> 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

"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."

Jon and Neil,

Are you suggesting the ER collet loosens during the work?

Why do you think this happens? I have a set and even though I have not noticed it happening I am glad to be forewarned about the possibility.

John

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

Every time it's happened to me, my impression is that it's either I haven't tightened it properly (see Andrew J's article in the current ME) or been with a screwed shank cutter where part of the screwed section is held by the collet.

Probably on 4 or 5 occasions.

Neil

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