Milling: creating a smooth end finish in a slot

[Rob Meades]

Newbie question: I purchased a High-Z/S-400T milling machine from CNC Step recently for hobby use. As a test, I'm going to mill a maze into a piece of brass plate. As a prototype step I've cut the same pattern into a piece of perspex. The vertical edges have turned out very well, what I'd also like, though, is to somehow smooth the end of the mill to remove the circular scuffs (see picture below). Can anyone suggest a way of doing that?



Cutting parameters were: 2 mm two-flute end-mill, tool speed 3,500 RPM, feed rate 4 mm/second, plunge rate 0.3 mm/second and pass depth 0.3 mm (so 10 passes to make the 3 mm depth above).

Rob

[Ger21]

Tram the spindle as good as you can.
Use corner rounded end mills.
Get a more rigid machine.

[Rob Meades]

Thanks for the swift response.

Corner rounded end mills sounds good. I'm afraid I need to ask what you meant by "tram the spindle" though...?

That cut was made over a 9 hour period with no return to reference, so I think the registration, which I guess is the derivative of rigidity, is pretty good. Anyway, I'm not forking out more than UKP 5k for a machine!

Rob

[Merlin201314]

You need to use a one flute end mill, the 2 flute leave more trace on the end of tool. Especially on perspex. the rigidity has nothing to do with that, the walls are clean, so no vibrations.... 3500 rpm for a 2mm flute and 4mm feed rate is to low, 8000 rpm and up is 🆗


Sended by my tapatalk

[Rob Meades]

Ah, good information, this is the kind of thing I will learn by experience I expect. I've been searching on the web for something that will tell me the recommended tool-speed/feed-rate/pass-depth for a given material/tool-diameter/number-of-flutes (all in metric please!). Is there such a thing? I end up doing some part of the calculation manually when it seems trivial to create a proper calculator for it.

[Neale]

There are tools like HSMadvisor and G-Wizard, which give you a free trial and then you pay. I think that there might be some free online tools as well, but I haven't used them.

[Rob Meades]

I was originally looking for web-based calculators but if I have to download and/or pay for an app then so be it. I'll go look...

[Neale]

Try this one. I couldn't remember the name just now.

[Rob Meades]

Hi again. I've found myself a 2 mm, 2 flute end-mill with radiused corners (0.2 mm radius) and used the FSWizard web calculator, from which I get a 5 mm/second feed rate and 23,000 RPM for cutting in brass. I've just tried using 20,000 RPM and a 4 mm/second feed rate, running 0.3 mm passes to achieve a 3.8 mm pocket in brass. 10 hours in (it's quite a long pocket), towards the end of the last pass (13 passes), the bit started making screeching noises and eventually snapped. You can see from the picture below that it was fairly badly damaged.

Two questions:

1. Am I expecting too much for a bit to work that hard for that long?
2. Should I try, say, a 3 mm/second feed rate and 26,000 RPM (the next step up on my motor)?
3. ...or something else?

[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.