Milling a profile – help with technique please

[Sarah FParticipant @sarahf]

I've just got back to machining a few bits after a break of a few years and I would appreciate a bit of advice from those with more experience than myself.

One of my projects involved CNC Milling the part out which is in the attached photograph. My feeds and speeds were a bit on the industrial side (1.25mm doc, 80mm/min feed rate, 6,000rpm with a 2 flute 3mm slot drill, cutting 5mm deep in aluminium) for my KX1 mill as it did vibrate noticeably. I'll reduce the depth of cut and feed rate a little for the next try.

 

My question related to slot milling, when I cut out in similiar profiles in aluminium, what would an appropriate cutter size be? Also would I be better cutting the slot width in more than one pass, i.e. cutting further out and then an finishing pass to bring the profile to size. The cut finish with cutting the 3mm slot with a 3mm slot drill was very poor.

 

I'd appreciate any advice please, thanks 😊

 

Edited By Sarah on 07/04/2020 18:57:15

[Sarah FParticipant @sarahf]

[JasonBModerator @jasonb]

As you don't really want the slot but the part surrounded by it a cutter with more flutes would be one option to getting a better finish though you could also consider an aluminium specific cutter which would have 2-flutes like a slot drill but with a different helix angle to help clear swarf.

On a contour cut you would be better setting a final shallow finish cut only when full depth has been reached, use climb cutting and some lubrication such as paraffin.

A small cutter will always be more likely to chatter so consider using a larger diameter one and maybe two setups, the first to drill the holes and then a second setup with the work screwed to a block of scrap material then you could do the cut in a series of full height passes working in towards the final contour, this will give more even wear to the cutter rather than just using the end. Your internal fillet where the straight meets the rounded end will be the determining factor here as to how large you can go.

Assuming your cutter is carbide I would have used your max 7000rpm and feed at least 50% faster.

[EmgeeParticipant @emgee]

Hi Sarah

I always use a climb milling program and find it gives a better finish but that is only on 1 side of the slot, it is important to keep the chips clear and if there is any sign of pick-up on the tool a poor finish will result, just a spray of lubricant will help prevent pick-up.
Reducing DOC and feedrate will no doubt improve the finish, best try 1 change at a time to learn what works for your set-up.
Doing a second pass full depth on a different path will of course give an improvement, and as you say look on it as roughing and finishing passes.

Emgee

[BazParticipant @baz89810]

Appropriate cutter size depends on your jobs smallest internal radius, I have a Taig Micromill CNC mill and would do a similar component with depth of cut of perhaps .75mm, feed of 70-75mm min and about the same spindle speed. I would rough out leaving a 0.2mm finishing pass which would be done full depth in one pass. In my opinion you could loose a couple of the tabs, bring the end ones in a bit and loose the middle ones, makes cleaning up a bit quicker.

[Tony Pratt 1Participant @tonypratt1]

Was your cutter sharp as there are a lot of burrs, is it really soft Aluminium? As with all machining you get a better job using roughing cuts then a finish cut with a nice sharp tool/cutter, use lube & climb mill.

Tony

[Anonymous]

I'd agree with Jason. I'd drill the two holes on the manual mill, screw to a fixture on the CNC mill and then profile the outside with a 3-flute 6mm cutter, full depth, 7000rpm, 400mm/min and 3mm width of cut. I normally leave around 0.5mm when roughing and then a full depth finish pass. For roughing I use climb and conventional milling, for finishing mostly climb. If the small concave radii can't be designed out I'd re-machine them after profiling with a smaller cutter. Make the cutter smaller than the radius to be machined or the cutter will chatter.

Generally I avoid slotting where possible. Even with flood coolant it's a PITA to clear the swarf and nothing fudges the cutter and finish quicker than recutting swarf. Another issue with slotting is the use of bridges. When I have to use them I make them 0.5mm high maximum. But they're still a pain to clean up. It can be easier to start with material slightly thicker than needed, profile the part, turn over and face off the unwanted material.

These parts are steel, but show the sort of finish that is possible with a hobby CNC mill:

Andrew

[JasonBModerator @jasonb]

Like Andrew I don't use the method much but this is something I did soon after getting the KX-3, think the mill was still sat on the pallet and code done with Vectric. 6mm dia 3-flute HSS cutter, 3000rpm, 150mm/min feed doing 6 passes 1mm deep for each in teh 6mm material, no finish pass as I did not know any better at the time. Few blasts of air to keep chips out of teh cut and a little paraffin gave a good crisp edge and decent surface ( ignore the hold hole at the top in the scrap material)

And the sort of finish you can get on aluminium, this was roughed and finished at full depth.

[Sarah FParticipant @sarahf]

Thank you for your replies, I do appreciate your advice.

I have ordered some 6mm cutters and I will modify my Cut2D files for a 6mm dia. cutter doing a roughing and a finer finishing pass, using the feed parameters which you have advised.

As I have four identical parts to make for the first part I will slot around the profile, then for the second part I will cut some material nearly to size, screw it to some MDF and then mill from the outside inwards, with again having a final full depth finishing pass. The next two I can vary feeds to see how it effects the finish. I do need the tight 1.5mm radius on two points, so I will do that as a seperate operation after completing the profiling with the 6mm cutter. I am using WD40 as a coolant/lubricant, is that okay to use?

I will also get some specifc grade of aluminium, as the stuff I have is just something I got from ebay and I think it is on the softer side. I'll have a read up on aluminium material specs.

Thanks again for your help.

Regards, Sarah

[EmgeeParticipant @emgee]

Profiling cut with 6mm cutter at the start of this video, max spindle rpm of 2k limits the feedrate, using a slot drill makes it even worse but necessary for this application, material is 7075T6..

**LINK**

Emgee

[Anonymous]

A few more notes:

It helps greatly to use quality cutters – currently I use YG K2 and ALU-POWER cutters from Cutwel (open and shipping) and premium cutters from Arc (closed).

I wouldn't use MDF as a base with, presumably wood screws? If I need a base I always use steel or aluminium; although I do have fairly large offcuts piles for both materials

The most widely available aluminium alloy is 6082 (aka HE30) which machines very well

WD40 is good to prevent the swarf building up on the tool but doesn't do much for cooling. But for aluminium you don't need to worry about cooling. I use flood coolant on my CNC mill – for aluminium it's primarily for washing away swarf rather than cooling. For slotting I wouldn't use squirts of ED40, it'll just cause the swarf to stay in the slot. If the worst comes to the worst I machine dry and follow the cutter with a bendy straw or the vacuum cleaner to remove swarf. If you have a compressor you might be able to setup an airblast. But beware of flying swarf – a trip to A&E to get swarf out of the eye may be a problem at the moment. Of course you wear eye protection?

Andrew

[JasonBModerator @jasonb]

Cutwel have all the YG-1 on offer today, something like these uncoated carbide would be an economical choice.

As Andrew says MDF would be a bit soft for small parts, not so bad if it's a large sheet that you can get plenty of screws into. Best bet would be to tap a couple of holes into a scrap of aluminium and set that in your vice so it is just above the jaw tops then you can try one with the cutter set say 0.25mm below the bottom of the work and do all the roughing and finish passes at that one height.

This is one I have done this morning material is 6082, cutter a carbide 10mm aluminium specific one from ARC running at 4000rpm, feed 300mm/min, 0.5mm depth of cut from just outside the sawn shape and a final 0.25mm finish pass that was run again at thesame setting just incase there was any spring in the tool ( was not needed) Probably a bit boring to watch it all but the reflection of my finger at the end shows what finish you should be able to get. The other advantage of doing it like this is most of the swarf gets thrown clear.

This was the part I posted earlier, profile cut starts about 2 minutes in.

[Sarah FParticipant @sarahf]

I watched the videos and I will be happy if I can get a finish like that.😊

I've made use of the offer at Cutwell (buy 2 get 1 free) and bought three of the 6mm cutters you recommended. I look forward to trying them.

I've got my workshop vacuum cleaner, so I'll use that to clear the swarf. I've got a few chunks of surplus aluminium so I'll mill some flat and use that instead of MDF. I'm very good at using my safety glasses, the last pair were damaged when a Dremel cut wheel broke up and a bit hit the lense!

Many thanks again for your help.

[Author]

Posts