Milling – How to get a good finishing cut?

This topic has 17 replies, 9 voices, and was last updated 30 October 2017 at 20:16 by Steve Withnell.

Viewing 18 posts - 1 through 18 (of 18 total)

Author

Posts
26 October 2017 at 22:12 #323783
Steve Withnell
Participant
@stevewithnell34426
I've milled a cavity in some Aluminium plate 22mm wide x 56mm long and 15mm deep. The corner radius is 2mm. I need to take a couple of finishing cuts, whats the best technique to get very best finish? Clue – 22mm is a quarter wavelength

I've obviously got a long series 4mm cutter, which is a standard helix carbide type and the only other cutter I have is a 5mm high helix version (which would obviously leave a bit of cleaning up for the corner radius. The depth of the cavity is the critical dimension.

Steve
Advert

26 October 2017 at 22:12 #8932
Steve Withnell
Participant
@stevewithnell34426
26 October 2017 at 22:23 #323786
Anonymous
A CNC mill, climb mill, and use a 3mm cutter so you don't get chatter in the corners.

Failing that I'd leave about 10 thou or so on width and length and climb mill full depth. The depth can be set accurately using the knee, or quill, depending upon the mill type.

If 22mm is a quarter wavelength why is the 15mm depth the critical dimension?

Andrew
26 October 2017 at 22:25 #323787
Sam Stones
Participant
@samstones42903
Hi Steve,

Sounds like 'Plumber's radio' to me (wave guides and cavities?).

Climb milling; slow feed; plenty of turps.

Regards,

Sam
26 October 2017 at 22:50 #323793
Muzzer
Participant
@muzzer
Perhaps worth trying the high helix cutter? 55 degrees and higher seem to be recommended for best finish in loominum. Also – is it worth looking for a more machining friendly alloy? It wouldn't be cheating but could make the job easier. When you say corner radius, presumably that defines the cutter diameter.

Where are the feeds and speeds coming from? And are you using an adaptive toolpath to control the load on the cutter?

Murray
27 October 2017 at 15:56 #323913
Steve Withnell
Participant
@stevewithnell34426
Posted by Andrew Johnston on 26/10/2017 22:23:18:

A CNC mill, climb mill, and use a 3mm cutter so you don't get chatter in the corners.

Failing that I'd leave about 10 thou or so on width and length and climb mill full depth. The depth can be set accurately using the knee, or quill, depending upon the mill type.

If 22mm is a quarter wavelength why is the 15mm depth the critical dimension?

Andrew

Thanks Andrew.

I keep avoiding sending Ketan a wedge for a KX1, which would be ideal for this application The 22mm is not critical because the resonators are tunable. The depth of the case affects the impedance and bandwidth of the filter (etc). The cleaner the finish the better the overall performance.
27 October 2017 at 16:01 #323914
Steve Withnell
Participant
@stevewithnell34426
Posted by Sam Stones on 26/10/2017 22:25:30:

Hi Steve,

Sounds like 'Plumber's radio' to me (wave guides and cavities?).

Climb milling; slow feed; plenty of turps.

Regards,

Sam

Interdigital Digita Filters – I've made a few at 1.3GHz and this is the first I've attempted for 3.4GHz. I thought with less metal to remove it would be easier, but I've also a lot less 'elbow room' with this one. I shall break out some turps! (I've been working with Parafin and Neatcut, but the Neatcut ends up in sticky mess).
27 October 2017 at 16:34 #323918
JasonB
Moderator
@jasonb
I'd drill out the corners 3.9 then mill out the rest with say a 10mm just under size, clean out the corners then do a full depth climb cut with your 4mm long series cutter assuming it is sharp. Just take a very little off so you keep chatter to a minimum and use a bit of paraffin to help stop swarf sticking to the cutter
27 October 2017 at 16:49 #323923
not done it yet
Participant
@notdoneityet
As i see it, if the depth is crucial, is the ally plate a good constant thickness or has it been faced off? No real problem if youogo slightly too deep – just face again? Another ploy, if the surface finish in the bottom of the cut is needed to be a polished surface, would be to fabricate with a through slot and affix a flat back plate?
27 October 2017 at 16:54 #323928
Neil Wyatt
Moderator
@neilwyatt
FWIW uncoated carbide is supposed to stick to aluminium less than carbide with a fancy coating.
27 October 2017 at 17:56 #323940
JasonB
Moderator
@jasonb
And I should think even less to uncoated HSS as the non sintered material is smoother.
27 October 2017 at 18:27 #323942
Muzzer
Participant
@muzzer
When I worked in microwaves, the duplexers, loads, waveguides etc were made of copper, brass etc that could be silver plated. It was also pretty handy for brazing the bits together. To my understanding, the purpose of the plating is to improve the contact resistance between components which presumably isn't ideal with aluminium. Similarly, when I used aluminium for high current busbars, it was necessary to use special conductive grease (copper bearing, IIRC) to get a good contact. Don't you need a good contact anywhere, or is the cavity free floating electrically?

For (my) reference, I see the skin depth of sliver at 3.4GHz(?) is about 1um and aluminium about 1.5um whereas the layer of aluminium oxide is only 10nm or so, apparently.

Murray
27 October 2017 at 18:52 #323948
Steve Withnell
Participant
@stevewithnell34426
Posted by Muzzer on 27/10/2017 18:27:03:

When I worked in microwaves, the duplexers, loads, waveguides etc were made of copper, brass etc that could be silver plated. It was also pretty handy for brazing the bits together. To my understanding, the purpose of the plating is to improve the contact resistance between components which presumably isn't ideal with aluminium. Similarly, when I used aluminium for high current busbars, it was necessary to use special conductive grease (copper bearing, IIRC) to get a good contact. Don't you need a good contact anywhere, or is the cavity free floating electrically?

For (my) reference, I see the skin depth of sliver at 3.4GHz(?) is about 1um and aluminium about 1.5um whereas the layer of aluminium oxide is only 10nm or so, apparently.

Murray

Hi Murray,

I'm using stainless screws through the case into copper rods. It's all about skin effect so the stainless screw is literally a mechnical fixing and irrelevant to performance. The bottom of the copper rods, I chamfer towards the tapped hole so that the edges bite into the aluminium. Instead of conductive grease, I'm using gold leaf as a gasket to ensure a good seal. This is the other reason for needing a nice flat finish to the walls of the case.
27 October 2017 at 18:56 #323949
Steve Withnell
Participant
@stevewithnell34426
Posted by not done it yet on 27/10/2017 16:49:29:

As i see it, if the depth is crucial, is the ally plate a good constant thickness or has it been faced off? No real problem if youogo slightly too deep – just face again? Another ploy, if the surface finish in the bottom of the cut is needed to be a polished surface, would be to fabricate with a through slot and affix a flat back plate?

My technique is to machine out the cavity a little too deep than skim the top to size, so the bottom of the cavity is parallel to the top of the walls. I could machine a through slot, but I'd still be left with the key issue of getting a nice finish to the side walls and I'd have 16 holes to drill and tap rather than 8 and two lids to make! So all trade offs as ever.

Steve

Edited By Steve Withnell on 27/10/2017 18:58:14
27 October 2017 at 20:46 #323964
MW
Participant
@mw27036
Posted by Neil Wyatt on 27/10/2017 16:54:40:

FWIW uncoated carbide is supposed to stick to aluminium less than carbide with a fancy coating.

That's also why the ones designed for aluminium have their surface polished and buffed, would be great to see a video of how they do that.

Michael W
29 October 2017 at 21:21 #324367
Steve Withnell
Participant
@stevewithnell34426
All done – next step is to see if it performs!. I ended up polishing the sides with the flat of a file, I still had some noticeable ripples in the walls. More practice is probably in order.
29 October 2017 at 23:34 #324383
Marcus Bowman
Participant
@marcusbowman28936
If it was me, I would use a polished, uncoated single-flute carbide cutter with an aggressive geometry designed specifically for machining aluminium. If possible, I would avoid using long small diameter cutters,

Speeds and feeds are pretty important. Spindle speed shold be basded on around 100metres/minute, so a 3mm cutter should be turning at somewhere around 10,000rpm. I'm guessing you are not running your spindle at that speed. A 10mm cutter should spin at around 3000rpm, which is achievable on many small mills, so that's a good go-to size for starters. Won't work for tight corners, of course, but ,as JasonB says, you may be able to deal with those by drilling, or by machining separately.

Rough out, leaving 0.2mm to finish. Climb cut the finishing cut. High speed, but a slower linear feed may help.

I have had decent results with a long series 2 flute cutter on 50mm deep finishing cuts, but it was a 10mm cutter, not a 3mm matchstick. Roughing at 3000rpm, and up to 500mm/min, taking cuts of 15, 15 and 20mm down the face, finisihing with a single climb cut pass at full depth, 3000rpm and 120mm/min. Material was grade 6082 (HE30).

Marcus
30 October 2017 at 20:16 #324517
Steve Withnell
Participant
@stevewithnell34426
Posted by Marcus Bowman on 29/10/2017 23:34:07:

If it was me, I would use a polished, uncoated single-flute carbide cutter with an aggressive geometry designed specifically for machining aluminium. If possible, I would avoid using long small diameter cutters,

Speeds and feeds are pretty important. Spindle speed shold be basded on around 100metres/minute, so a 3mm cutter should be turning at somewhere around 10,000rpm. I'm guessing you are not running your spindle at that speed. A 10mm cutter should spin at around 3000rpm, which is achievable on many small mills, so that's a good go-to size for starters. Won't work for tight corners, of course, but ,as JasonB says, you may be able to deal with those by drilling, or by machining separately.

Rough out, leaving 0.2mm to finish. Climb cut the finishing cut. High speed, but a slower linear feed may help.

I have had decent results with a long series 2 flute cutter on 50mm deep finishing cuts, but it was a 10mm cutter, not a 3mm matchstick. Roughing at 3000rpm, and up to 500mm/min, taking cuts of 15, 15 and 20mm down the face, finisihing with a single climb cut pass at full depth, 3000rpm and 120mm/min. Material was grade 6082 (HE30).

Marcus

Cheers Marcus. I've been asked to make another one of these, so I'll work out the machining as above. I've seen a few single flute cutters around from China, but may stick to a decent slot drill. My mill is flat out at 2,000, so will have to make do at that too!
Author

Posts