Milling: creating a smooth end finish in a slot

[Boyan Silyavski]

For tools smaller than 3mm you really need to find what the manufacturer says about that.

Depends on the bit though, i mean about how long lasting you expect it to be. Instead of using feed wizard, better download the full HSMAdvisor.

Your questions are pointless without knowing the final depth of cut, the shank of the cutter, the LOC and the tool stick out from collet.

Your machine is not on the rigid side, having in mind that it moves on unsupported rails, so maybe have that also in mind.

Depends also what quality bit you use? I have 2mm bits that each one is priced 60 euro and have some that are 5 euro for 10 pieces? Obviously that could be a thing.


Tramming your machine means the head /Z to be perfectly square in X and Y direction to the table. Other wise marks could be deeper. Though i dont see them to be so bad as i would expect from that machine.




Brass must be the easiest material of them all, at least for me. I dont believe you need a rounded cutter for this job. The best bits for the $ i know in this size are the Kyocera micro grain carbide, from drillman1 ebay.

Wanna see them in action? here is a video how i drill brass on my machine. 15 000 holes with a single bit is not a problem. I said bit, not a drill, as i did not have a suitable one at that time. Remember that sound. Thats the sound of a rigid machine, sharp micro carbide bit and perfect for machining brass.






Bellow i did the calc in HSMadviser which i greatly encourage you to test and purchase later as its extremely useful.





Changing the suggested pass depth very actively affects tool life / surprisingly for the better this time, normally for the worse/ so 0.3mm pass depth gives me 219.46 mm/min and double the tool life.


I agree with Merlin, in fact for brass max spindle speed is the right choice for me. with a small tool i mean.

And again, when you calculate, take care for the stick out of tool. Must be as min as possible. Cause if the tool was only 10mm protruding from collet, not 20 as the calc above, then 0.4mm depth of cut instead of 0.1mm and 438mm/min which is roughly 4 times the initial material removal rate



Another thing is that its not right on metal/or even wood/ to dig straight to the end result. offset 0.1mm and make 0.1mm separate finish pass, if need be with brand new tool especially for the finish pass.

[Rob Meades]

That's really useful information, many thanks! The tool I'm using is the 2 mm one of these:

http://www.cutwel.co.uk/milling/mill...e-e5930-series

...so 3 mm shank. and 3 mm length of cut. Which might point to my mistake: I measured what I thought was the length of cut of the bit and it looked like 4 mm (I'm cutting to a depth of 3.8 mm in 0.3 mm increments) but from the manufacturer data it's only 3 mm so the bit would have been getting quite upset towards the end. The stick-out was 20 mm, as you have assumed, which was the best I could do to avoid clamps as I'm cutting quite close to the edge of the material.

Your video shows a rather impressive speed of cut. :-)

I have a spare bit, so I will try reducing the final depth of cut to 3 mm (what I'm doing is purely a test job anyway), increasing the speed to 30000 RPM and have another go with that bit, rather than risk breaking something more expensive just yet. I will also download HSMadvisor.

[Boyan Silyavski]

And if you have not done it till now, do it - compressor, 0.6-0.8mm ID tube blowing air / or air plus cooling liquid/ right where the cut happens. Cooling things down tremendously affects bit life and finish result. later i will show you picture of my setup if you have not done yourself a mist cooler.

[Rob Meades]

Interesting, would very much like to see a video of that.

[Robin Hewitt]

Obviously I know nothing because I have no machine tools that do tens of thousands of rpm, someone will be along to tell me off in a minute, but I would happily cut that in modern brass. When I was a boy, back in the mediaeval period, brass used to snatch but those days are gone.

I think your problem is you are rubbing rather than cutting.

Slavish adherence to achieving feet/minute cutting speeds with tiny tooling makes for ridiculous rpm.

Keeping the tool shank intact with ridiculous rpm leads to tiny DOC.

Trying to get a job done in a credible time frame with tiny DOC leads to high feed rates.

I like my brass to be on the verge of squealing when I cut it and give a nice flake. I would use HSS tooling because a sharp edge is more important than tool wear, there is no tool wear in brass. It cuts like a dream unless you have that mediaeval brass which is a bitch.

I just looked up your router, it has 30 microns of backlash. That is not bad, but does it support a 6 micron tooth loading?

[Rob Meades]

Well, there's another parameter to play with. I'd not looked at HSS versus carbide. Rubbing rather than cutting would explain the look of the damaged tool tip, though I suppose that could also be that once it was damaged it would have been rubbing anyway. Playing with HSMAdvisor I can see that HSS gives me a lower required RPM, but I'm not sure what I gain from that: what can I increase, presumably by upping the RPM again, as a result (DOC, feed rate, etc?), or is it simply a better finish?

Apologies if I'm being dumb here, but I'm still trying to get my head around this. As to your tooth loading question, I'm not sure how I determine the answer...?

And no, I don' t think I have mediaeval brass, just Chinese brass. :-)

[magicniner]

HSS is a sharper edged tool which is less fragile and more forgiving than Tungsten Carbide tooling but will not take the temperatures associated with High Speed Machining so at the cost of reduced RPM you get less chance of the tool chipping.

You may be running the carbide cutter too fast without enough cutting lube/coolant, unless the heat is being removed you can get some smearing of the work material and as soon as that happens it will clog the cutter and give a result exactly as in your photograph, if you get the same problem when running the cutter faster I'd then put money on this being the problem ;-)

- Nick

[Boyan Silyavski]

Interesting, would very much like to see a video of that.

Here is a video overview of what i believe is a correctly build DIY mist fog less cooling system. Hope that helps you and others!

[Rob Meades]

VERY impressive! Especially your worked numbers (2.5 bar, 2 mm inside-diameter feed tubing, 0.8 mm inside-diameter nozzle). I'm working in my loft, so I have nothing like the space that you have, however there are dental compressor rigs that should work well (and quietly) available for around UKP150 on ebay so, using these numbers I should be able to make something similar.

Thanks!

[Boyan Silyavski]

VERY impressive! Especially your worked numbers (2.5 bar, 2 mm inside-diameter feed tubing, 0.8 mm inside-diameter nozzle). I'm working in my loft, so I have nothing like the space that you have, however there are dental compressor rigs that should work well (and quietly) available for around UKP150 on ebay so, using these numbers I should be able to make something similar.

Thanks!

No problem. There are many builds on the net, but when i started making mine i found that they or intentionally skipped explaining the fine details or were just unaware of them. basically almost useless information. So like always i had to start from scratch.

Here are some more details if you have not figured all from the video:

- the brass bar body ideally is >=8x8mm
- fitting holes translate seamlessly to inner bore hole.
- the 2 pneumatic fittings are m5 to 4mm OD tube
- the distance between them should be at least 2cm from center lines
- the way/bore hole/ that connects all is 2mm ID
- the brass tube is 2mmOD and 1mmID. I cramp it at the end with pliers, drill it 0.6-0.8mm, sand it flat, fine sand carefully the edge to chamfer without destroying the flat nozzle face Check correct flow with more output. This is the critical part that defines the blow pattern.
- brass tube is super glued and pushed fit at brass body. Dont overdo it as you will need to exchange tha tube sometimes for some jobs
- for hevy cutting up to 20-25mm cutter 1 tube is ok even blowing heavy chips from working surface, then better 2 tubes positioned from opposite sides
- hose is 4mm OD 2mmID PU hose from China , both air and liquid hose are the same
- quality water filter body will resist even thinners / mine is made in Italy/, a crappy Chinese one will explode if sth else than water, especially using alcohol if you see even one micro crack throw it away.
- 1x baby oil+0.1 x dish washer+ 1x water or kerosine / careful with the container, test it first without pressure and then fill it to the top, full container just breaks, does not explode/