Milling: creating a smooth end finish in a slot

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?

Attachment 19589

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

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

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

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

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.

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.

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...

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

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?

Attachment 19722

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.



Attachment 19723

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.

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.

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.

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

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?

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. :-)

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

Well I say, there are a lot of choices to be made here. I will go look at HSS tools and investigate the possibility of a cooling system along the lines described by @Boyan Silyavski.

Quote:

---

Originally Posted by Rob Meades

Well I say, there are a lot of choices to be made here. I will go look at HSS tools and investigate the possibility of a cooling system along the lines described by @Boyan Silyavski.

---

Have a look at this feed rate calculator:

http://www.daycounter.com/Calculator...lculator.phtml

Free, online and easy to use.

Quote:

---

Originally Posted by Rob Meades

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!


https://youtu.be/NVu4mCFCvmA

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!

Quote:

---

Originally Posted by 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!

---

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/

Well, I'm not having much success here. I don't have my compressor yet so I thought I'd try a HSS/8% cobalt end-mill (4 flute, 7 mm flute length, 6 mm diameter shaft) which requires a lower speed. With the tool sticking out 20 mm to avoid my clamps, I've taken the HSM Advisor recommendations and then backed them off, so 5 mm/second feed rate and 0.5 mm depth of cut, tool running at 14000 RPM as recommended. As a reminder I'm cutting a slot in [343-460 N/mm2 tensile strength] brass plate.

Result: tool snapped off in the middle of the first pass. It looks as though the tips have worn quite quickly and then the tool has become clogged with brass:

Attachment 19958 Attachment 19960 Attachment 19961

Here are my tool details, material details and the HSM advisor screen to match. Where am I going wrong?

Attachment 19951 Attachment 19962 Attachment 19952

FYI, until it snapped, it appeared to be making quite a reasonable cut:

Attachment 19956

Rob

Brass should not be a problem, don't understand why you are having trouble.
Maybe we need a close up of the cut edge, is it square, have you got vibration marks, is it smearing at the top?
Maybe a picture of the machine that is doing the cutting?

Thanks for the swift response and offer of help, here's some more detail. First, the machine (High-Z S-400/T):

Attachment 19967

Then, the material overall:

Attachment 19966

Then the cut; left is early on when some clear-outs are being cut, middle is at the start of the slot-cut (where the right-hand side of the picture is the earliest, the left-hand side is several minutes later) and finally right is the slot-cut just before the bit snapped:

Attachment 19965 Attachment 19964 Attachment 19963

For good measure, here's a video of the slot-cut phase, taken shortly before the right-hand side of the middle picture was cut.

https://youtu.be/buX52aHW8-o

From the third photo it looks like you have issues with rigidity. Your machine has unsupported rails on all three axes, so this is shouldn't come as a surprise. That shouldn't mean you can't make this part though, just makes it more of a challenge.

Is the tool plunging too fast? Ideally it shouldn't much at all.

Have you checked the runout of the spindle? With such a small tool this may have an effect.

The machine purchased was specifically stiffened for cutting brass; at least, that's what they told me, there was an extra stiffening bar, out of sight up-top in the picture of the machine above, for this purpose. I have a feeling that the mess you see on that last picture is because the tool had degraded by that point and hence was rubbing. If the machine were too sloppy, I'd have thought the same mess would appear early on as late on (see right-hand side of middle picture versus left-hand side)? Maybe a better question would be: could lack of machine rigidity somehow cause damage to the cutting edges of the bit?

It is worth noting that I'm cutting a very long continuous slot here as this is a maze that I'm cutting.

Plunge rate is 0.3 mm/sec. Not sure about spindle run-out: how would I go about checking it?

Rob,
Are you using anything to clear chips, cool the tool and possibly lubricate it ? A good blast of air and a squirt of WD40 seems to be the recommendation on other forums. You need to get the chips out of the way to stop them reattaching. Two flute carbide is also a better cutter for brass.

Cheers,

Rob

No, I'm picking up a compressor tomorrow and hope to use Boyan Silyavski's guidance to make myself an air blower. Maybe I'm just asking too much, making such a long slot-cut without cooling/blowing? I moved away from carbide to HSS because I could run at a lower speed (and hence reduce the heating effect) but it doesn't seem to have been a sufficient reduction. I think I'm going to try again with the same settings but reducing the feed rate right down, to 2 mm/second. I'll keep the vacuum handy and give it a suck every so often. I'll also order some more bits, 2 flute this time, and a lot more brass. Gonna get this right eventually...

Thanks Rob,

Rob.

To conclude this thread, I've now managed to cut the brass maze successfully. The secret was, as you probably expect, cooling. With a 1 mm internal diameter copper tube backing 2 bar of air pressure (no water, too messy for my loft) from a Jun Air compressor, cutting for 10 hours caused no damage to the bit whatsoever and the finish in brass is as good as that in perspex. I only applied the cooling during the looong cut around the side of the maze so as not to overheat the compressor but that was enough. Happy milling Christmas everyone!

Attachment 20076 Attachment 20077 Attachment 20078 Attachment 20079

Now you need to rework your G-code so it pierces on a slope rather than a plunge. Thus allowing you to use a conventional end mill, rather than a slot drill, and slick up that maze floor :beer:

Say what with the who now!? There are always wheels within wheels with this hobby. How do I pierce at a slope!?

Your slot drill is bound to chew up the metal directly below it's centre, it is just something they do. A milling cutter has no cut towards the middle so it can leave a fine finish below. They all have their tricks.

However a milling cutter can only plunge vertically so far before it's non-cutting middle bottoms out, so you have to move sideways as you move downwards to remove that middle.

Well, either that or restrict your Z travel to what it can manage :eagerness:

Ah, I always climb into the cut so I should be able to end-mill. But I thought a slot-mill and an end-mill were essentially the same things these days? How would I know I was buying a true end-mill that gave me a smooth bottom. So to speak.

You "pierce at a slope" by using the ramped or spiral lead-in options in your CAM package.

Clods have muddied the water on cutter nomenclature but there are always centre-cutting and non centre-cutting tools, Slot Drill used to refer to a centre-cutting tool capable of plunging (Drilling) and End Mill to a non centre cutting tool,

- Nick

Ah, Ok, so I want a non centre-cutting mill to achieve a good finish on my bottom? The terminology seems a bit weird to me as a thing that cuts a 'slot' I would have assumed to be good at cutting on the side (slots have walls), rather than the end, while the 'end' mill sounds as though it _should_ be good at cutting on the end. But I suppose it is good at 'milling' on the end, rather than 'cutting'? Bugrit, I'll stick with centre-cutting or non centre-cutting, that's at least a single term that can be positive or negative to conjure with.