Feeds, speeds, and other topics for the home machinst

[David]

So I don't clog up my B class mogul build thread with a litany of woes about CNC I've started this thread.

A summary of the current state of play: I bought a Tormach PCNC1100, I use cheap SWT HSS 4 flute cutters from ebay (HSS AI, whatever that is, I can't find anything via google about it. It's AI, not AL), no flood coolant, so far mostly 1.6mm or 2mm profiling and pocketing.

The mill isn't leveled or trammed. I know the spindle isn't quite perpendicular to the table because of the result when flycutting, but I don't know if that due to bed twist or spindle tram.

I use Fusion360 and Cut2D. Cut2D is quicker and easier to use for profiling and basic pocketing.

I'd like to use 2 or 3 flute cutters assuming they can center cut as I assume that would be better for this type of work but I can't spend the money right now.

To begin with I've taken Roger's advice and for the two little triangular cylinder drain shaft brackets in this post I slowed things down considerably.

The cut details: Brand new 3.5mm 4fl endmill, assume plain HSS. Spindle speed 1500rpm, feed rate 60 mm/min, doc 0.25mm. A straight ramp down over 20mm to avoid plunging the 4fl cutter.

It took 30mins to cut them, and you can see the 2mm material is flexing by the fact that there is a sliver of material on the lower left, and on the right the material was cut right through on the pass that was meant to still be 0.25mm above the bottom! I stopped it a pass early. You can also see the difference in the size of the spotted holes which were meant to be 0.5mm deep.

There were meant to be tabs on each straight side to hold the parts in place but the variable cut depth did away with them.

The tool was happier and the cut cleaner, although the total amount of cutting was much less than for the brake pull rods.

I still had to stand there and blow the chips away and brush cutting oil on once each time around a triangle, and still hear the occasional 'ping' which made me think the cutter was about to break.

Questions:

With chips this small and a 4fl cutter is it safe to just leave the chips in place? They'd basically fill up the channel being cut pretty quickly.

Could I have cut this dry? The oil makes the chips stick to and near the cutter so they sort of form a blob around it.

What feed/speed would you use assuming no flood coolant.

How would you have held the 2mm stock?

If you don't use flood coolant, what do you do? How do you keep the cut clean and stop the tool overheating?

What diameter, flute, and material are your favourite cutters?

[Doug]

Hi to answer some of your questions,
The with of the cut should never be the same as the cutter so always make it at least 0.5mm wider that will sort your chips problem and the cutter won’t break
Coolant should always be used unless your cutting cast iron
Dabs of coolant are fine for low fees and light cuts (I tend to stay below 1mm)
My fave cutter is 6mm carbide 4 flute end mill
Think you have overdone the hold down on the material the clamps you used look more than capable
I also use wood backing usually laminated board cos it’s flat but would use mdf at a push but it expands with oil and water so one use only.

[David]

Thanks dug.

There are so many screws only to try and hold the plate flat - the clamps do nothing in that regard. The screws were something of a failure too which surprised me!

I have a 6mm 4fl carbide cutter and didn't get much joy from it. I was running dry but blowing air on it as I read carbide doesn't like intermittent cooling.

What rpm, mm/min, doc would you use for the carbide cutting mild steel?

[Doug]

Oct 29, 2018 21:46:18 GMT David said:

Thanks dug.

There are so many screws only to try and hold the plate flat - the clamps do nothing in that regard. The screws were something of a failure too which surprised me!

I have a 6mm 4fl carbide cutter and didn't get much joy from it. I was running dry but blowing air on it as I read carbide doesn't like intermittent cooling.

What rpm, mm/min, doc would you use for the carbide cutting mild steel?

I usually go by “ear” as the condition of the cutter greatly alters the amount of material it will remove cleanly but I would start around 4-600 rpm and 15-25mm/min and usually <1.5mm depth but that will all depend on how rigid and powerful your mill is if it is chattering then I slow the feed down, I would never cut mild steel without coolant as it blunts the cutter. I have had no issues with dabbing with a paint brush so your ok doing that.
All the best
Doug

[Roger]

Hi David,

Here are my thoughts...

Holding sheet metal is always going to be troublesome, it will always move so you have to factor that in for any nibs you're intending to leave. The nibs need to be fairly high else they will not exist in some places. I may be wrong, but the nibs on that part look like they have vertical plunges? That's not going to end well. Nibs have to use sloping sides just like normal entry moves. This is why I couldn't use nibs on Alibre CAM because originally they didn't support sloping sides.

I think you would benefit from making some low profile clamps like mine that allow you to clamp very close to the work. Those chunky clamps don't let you get close unless you have the tool hanging out a long way. You can cut a piece of stock that's only 10mm bigger than the final part size and clamp it close to the edges. I also clean it all off with meths and use strong packing tape to hold the edges down sometimes.

Personally, I think you're using too big a cutter for that thickness of material, I wouldn't go above 3mm for that. In fact, I'd probably use 2.5mm and go say 0.5mm deep at no more than 30mm/min. I judge the spindle speed for how it sounds. If you're welding chips to the work, you're going way too fast. You should be able to leave it and walk away. I've just machined 1.2mm Stainless Steel Sheet with a 2mm cutter, 0.4mm deep at 20mm/min 1900RPM and it's cut out five parts unattended. There was plenty of cutting oil still in the groove when it was finished. Sure, it's thrown up some big burrs, but that's par for the course. If you're having to watch it, you're not getting as much benefit from CNC as you could. For me, exchanging run time for zero attendance is a no brainer, I've got better things to do than watch the machine!

My gut feeling is that your RPM is still too high, as are your feeds, but you can go deeper.

In my experience, there's no reason why you can't go at least the depth of cut being equal to the diameter of the cutter before you have to consider adding extra clearance. In fact, I don't usually consider it an issue until you're going to 2 x the diameter deep or more. I can't remember the last time I had to do it.

I have no issue with chips remaining everywhere, it's going to happen unless you have flood coolant or compressed air blowing the chips away, so I just accept it's going to happen. That doesn't mean I won't hoover up the swarf from time to time if I'm there.

I always both rough and finish every part, regardless of what it is. Usually I use the same tool for both, but for fine work I'd change to a sharper cutter for the finishing cut. I group the cuts together for convenience so I don't have to keep going to the machine to start a new part of the program.

For roughing, I leave no more than 0.3mm stock for finishing, and often I use 0.2mm. It depends on how big the cutter is and how hard the machine has to work. If it's a big part with big cutters and heavy loads, I'll use 0.3mm. If it's a very delicate part with small cutters I may even leave 0.1mm for cleaning up. The key thing to take away is that even with chips in the way, a finishing pass usually gives a good finish. For the best work, getting rid of the chips will help a little, but usually I'll finish them with draw filing, so it's not that important.

I use a 3 degree slope into the work for the roughing passes, and the same for the nibs. This really matters when you're machining difficult materials like Stainless Steel sheet. For the finishing cut, I always plunge precisely into the gap made by the rouging cut and then do a 2D approach from the side. It's easy to do because the entry arc radius is the same as whatever stock you've left from the roughing cut. There is no linear extension for this, the cutter drops straight into the groove and then describes a tiny arc to start the finishing cut. Sloping entries for finishing passes can lead to long ugly lines on the finished piece, particularly if you're machining plastics.

The reason for the above method of entry is that it can be universally applied to any situation. You never have to consider what stock is outside of the part, something you have to be aware of when using a 2D side entry.

Personally I think you should ditch HSS cutters, they're not much good for CNC in my opinion, especially when much of it is running nearly dry. Carbide is cheaper than you seem to indicate. I've used this supplier and I've just ordered some even cheaper ones from here. I keep a bottle of cutting oil that I apply to the cut from time to time so it's not completely dry. I find it cuts smoother and sounds generally happier when there's a bit of lube on it. I'd love to use flood coolant, but it's just not practical in the space I have available.

[92220]

I use a lab wash bottle (£2.36, and free post, on Ebay) for coolant now. Although I have integral coolant systems on both the lathe and the mill, I haven't used them for a couple of years now! I have 3 x 250mls wash bottles of coolant so I always have a full one. The machines stay cleaner too! The coolant gets squirted exactly where needed and not over everything else.

Bob.

[David]

Thanks Bob. It certainly sounds like a good idea for the manual machines but the point on the CNC machine would be just as much to wash away the chips as the cooling, so a constant stream would be necessary, preferably without me standing there providing it! Air is probably as good for clearing chips, and I assume MDF backing pieces would be useless with a constant stream of cutting fluid on them.

We're in a spending freeze here as we reorganise finances after a hopelessly expensive few years so no misting systems or carbide cutters are on the immediate horizon. I'll just have to get by with what I have for a few months while we clear the decks and come up with something more sustainable.

If I was really keen you'd imagine I could rig up an air tube from the compressor with what's laying around. I don't seem to be that desperate yet! It's stupid but I just loathe working on the tools themselves even when it would then improve my working conditions and productivity for years to come.

[Roger]

Hi David,
MDF isn't very good even when you apply coolant by hand because it softens and you lose the clamping force. I use a coated version that's really thin and that works pretty well.

In my opinion, spending time on tools and tooling saves not only time but stops me from scrapping jobs that aren't held well enough so they move while being machined. I treat them as another project, and when it comes to the time to use them I get a lot of pleasure from them. I suppose we all get our pleasure from different aspects of Engineering.

[David]

I am wondering if I am using the wrong type of toolpath for my parts. Doing an F360 adaptive clearing op, going down 0.5mm at a time is a joke and does not seem to be effective use of the cutter.

I've looked at the 3D toolpaths and can't find anything that suits, I end up with big plunges and lots of stock left around the outside.

So I'm simulating cutting the full depth stepping in from the outside. I've made the round stock as small as I dare but there are two things I don't like:

1. It isn't until the 10th time around that the stock at the 'top' and 'bottom' of the part start to get cut - it would save a ton of time if the toolpath just zipped straight across if it saw no stock was in the way.
2. Converse of 1, the first cut along the sides of the part is more than 50% of the cutter width which I assume will just snap it. I'd need to add 10+ passes to avoid this.

If I solve 2 by adding 'padding' passes so the first cuts are not too wide it makes 1 worse.

I'm using a stepover of 0.5mm which is more than I'd do on a manual mill, I'd go 0.25 there. Is this too much? Too little?

How would you guys cut this part? Is there some strategy I could use to clear those side bits first?

The toolpath parameters:





The big gap at 'top' and 'bottom' on the outer cuts:



The big cut at the sides on the initial cut:

[atgordon]

Looking at your problem made me realize that I have never used anything thinner than 1/4" on my mill! Workholding for a small part is critical, and it looks like you have got the part well clamped ... I'm guessing that T-bolt clamps are as close as you get to the work and not hitting the chuck. F360 does allow you to build in fixturing and you can force the machine to avoid clamps, etc. (a little fiddly too do)

In terms of cut, I try never to ramp down into a slot. It is tough to do well, and with black iron (which often has a hard skin), it can kill the end of the cutter quickly. If you are forced to ramp, then use 2 flute cutters and reduce the feed rate for the entry phase (why are they not called slot drills anymore?).

In this case, I would have elected to drill en entry hole (I try and make the entry holes a little larger than the cutter dia) so that you could come down to full depth of cut, and then used adaptive clearing to work around the slot part (it is one of the few toolpaths that give constant cutter load). I would be tempted to try a slightly wider slot to improve the surface finish ... but then I would have looked at the extra cutting time, and probably gone for a single slot cut.
What coolant are you using (you're mention of the "oil" sticking made me wonder if you're using cutting oil =- not a good idea since it is pretty goopy. I'd use a good synthetic GP coolant (they have excellent bio degradation resistance). I would use flood coolant for a job like this.

I ran the numbers though the FS package I use for my starting point and came up with RPM 1450, Feed 0.5" (was 0.05" typo!) in/min, fz=0.0002" ... I usually run slightly slower on a fist cut (say 1200), and at 50% feed on the pendent until the cut is underway and then move towards 100% once I hear and see that the cutter is happy.

FS stuff is more of an art for stuff that is difficult to hold and thin! Plus the smallest cutter I've ever used in my CNC life is 0.25" so I have no experience with smaller and thinner stuff. The folks who have built locos using CNC are better at this stuff than me!

If you are hearing "ping" sounds, something is seriously wrong! The CNC gods are telling you to stop!

[Neale]

Here's a completely different take on the problem. I'm building the Don Young Black 5, working on the tender at the moment. The front and rear drag boxes are a jigsaw of 3mm steel pieces to build up fairly complex structures. I've redesigned the individual components to use a tab-and-slot self-jigging structure which can be assembled, clamped, and then MIG welded. To cut the pieces in any meaningful timescale I needed CNC, so looked to my CNC router to do the job. Fortunately, I seem to have built it strongly enough. The problem was the minimum router spindle speed of around 6K RPM. I have been successfully using 3fl carbide cutters (I have been buying these from Cutwel at about £5-6 each). I run 3.5mm at 5500RPM (a bit under the min for the spindle which means not very much torque which limits rate/depth of cut). I'm using about 0.8mm DOC at 160mm/min. I cut a slot the width of the cutter (F360 profile cutting path) with a "stock to leave" of 0.2mm, then a full-depth finish pass to bring to size. Finish is acceptable for the purpose if not brilliant. For the slots and small features, I'm using a 2mm 3fl cutter at 8500RPM and 110mm/min, 0.5mm DOC. DOC and rate of cut are lower than Cutwel recommend on their web site but I can slow the spindle if I go much heavier than that - loss of torque issue from a spindle that runs up to 24K! However, rotational speed is as per supplier's recommendation, and I cut dry (as per supplier's recommendation). That's cutting hot-rolled MS, ramping in (usually). Ramping-in speed is about half the usual cutting speed. I also use triangular tabs to avoid plunging at the trailing edge of rectangular tabs although they are steeper than the ramping-in angle. The cutters are supposed to cut to the centre so theoretically capable of plunge cutting but I try not to plunge to be kinder to the cutter. I follow the cut with the shop vacuum cleaner to keep it clear of chips - and I do get real chips, not dust, although obviously the chips are pretty fine. I've now just finished the second drag box, plus a couple of fabricated frame stays in 2.0mm steel cut the same way, and I'm still on my original cutters.

In reality, it's laser-cutting job but this is both a lot cheaper (hot-rolled strip from my local supplier is really not that costly) and means that everything is completely under my control. I'm surprised that it works so well but the secret was finding those small cutters than run faster than I would have expected and without coolant.

[David]

Thanks Neale. What you're doing I have tried to do a number of times without the success you're having. I'll need to do it again at some point but wanted to do some parts that were not thin flat stock given it wasn't working out for me.

How do you hold the stock down? I find it bows and flaps and carries on with clamps or screws.

I'm about to look for posts by you in the hope of seeing pictures.

I'm too cheap to buy name brand cutters until I think I won't break or dull them within minutes, but I'm glad to hear you can get ones that are happy to cut dry. Do you know what coating they have? I've read a number of times that carbide would prefer to cut dry, but with an airstream, than intermittently wet.

I've bought a couple of cheap misting nozzles on the recommendation of a friend who uses them in the hope they will free me up from standing in front of the machine blowing the chips away.

I've used the last of my 'workshop' money this month to get a couple of 6mm no-name altin coated endmills too. I hope that's what I ordered - there are a lot of coatings and I'm not hugely confident the ebay sellers get them right, and in a non-serif font i and l look a lot the same. Perhaps I'll end up with something that only cuts cheese!

atgordon has warned me carbide should always be used close to the recommended rpm, whatever the feed rate. Anyone else agree with that? Even on a toy machine like mine?

[Neale]

As it happens, I'm putting together a talk on the whole process I use, from initial design in F360, then CAM, to cutting. I was taking some photographs last night to illustrate it so I'll try to post some later when I've downloaded them from my camera and worked out how to upload them here. I'll try to describe my hold-down methods as well and some gotchas in that area.

This is the range of cutters that I'm using at the moment, although I think they had a special offer on when I bought them.

Please don't think I'm an expert - I'm just a bloke who's been playing about a bit and struck lucky. The sight of a tiny 2mm cutter in my CNC router is still frightening but sometimes you have to trust the figures and the machine! 

[David]

The relevant words from that link are "The new X coating offers higher performance machining compared to TiALN". I've ordered TiALN as I thought that was the best coating for cutting steel. We'll see what happens.

[David]

I've been looking for info about carbide coatings and dry cutting etc and found an interesting page.

The things that stand out are:

"The heat is dissipated so well into the chips with the AlTiN coating that dry machining is mostly recommended, except when slotting where the chips need to be expelled out of the channel. The aluminum in the coating helps form a gaseous aluminum oxide layer at the cutting edge where temperatures can reach more than 1800°F. This helps protect the carbide substrate from the damaging effects of heat. That's what makes this coating ideal for high-speed and hard milling, especially in dry cutting."

and

"Forms a thin surface layer of Al2O3 that is hard, low in friction and oxidation resistant. As this layer wears, it is constantly rebuilt from the Al in the coating.
Performs best in high temperature applications. Requires high temperatures to form the Al2O3 surface layer."

So apparently if you don't run it hot enough the coating doesn't work. What do you think?

I know I can't run industrial feeds and speeds but I went to a site that had detailed figures and calculations and came up with:

Mild steel, Surface ft/min = 500, Surface metres/min = SFM * .3048 = 152.4 m/min.
Feed per tooth = MMPT = 0.043mm/tooth
Chip load factor at 10% radial cut depth (0.6mm) = 1.8
RPM = SMM x 318.06 / 6 = 152.4 * 318.06 / 6 = ~8000!
Feed = RPM * 4 * 1.8 * 0.043 = 1.3m/min!

Clearly not practical. But does it mean I'm wasting money buying this coating?

[simplyloco]

Jan 8, 2019 10:58:07 GMT David said:

I've been looking for info about carbide coatings and dry cutting etc and found an interesting page.

SNIP

Clearly not practical. But does it mean I'm wasting money buying this coating?

In my not so humble opinion, the answer is yes!
John

[Roger]

Hi David,
Why are you concerned about removing all of the material outside of the part? It wastes time and wears out cutters when there's no need for it.
For a part like yours, I'd use a 6mm cutter and say 1mm deep rouging cuts, sloping in from the top at 3 degrees starting at 0.2mm clear of the surface. I'd leave 0.3mm stock and completely clear the profile first. It doesn't look deep enough to need making the width of the cut bigger than the tool diameter.
Don't worry that the outside will have stock sticking up.

I'd then create a pocket operation to rough the face using the same parameters but with 50% step over.

The finishing cut for the profile would plunge using a 0.3mm radius entry move and no straight portion so the cutter drops into the channel you've roughed out. NB:- This is why the 0.3mm stock was left and it must match the radius of the entry move.
ie it's a 3D entry when roughing and a 2D entry when finishing.
You can finish the full depth in one cut. Plunge slowly in case the tool setting length is slightly long since you're having difficulty setting these accurately.

I disagree about not sloping into a slot or anything else, in my opinion it's not a problem if you use a shallow slope of 2 or 3 degrees and lubricant. I slope into all my roughing cuts because it makes life easier when stock is going to be left outside of the profile. Using this strategy you can slope in with 4 flute cutters without difficulty. 3-flute cutters are the most universal in my opinion, making sloping entry easy while still giving enough cutting edges and clearance to get good swarf removal.

The finishing cut for the face uses the same strategy as the roughing of the face but uses a smaller diameter cutter and does the full depth in one cut.

Bear in mind that my comments only reflect amateur practice, commercial shops would certainly use different strategies where time is of the essence.

With regard to Coated Carbide cutters, you'll find that pretty much all of them come coated as standard, even on the cheapest of cutters sourced through eBay

[David]

At this point having both come down from the top in layers and in from the sides at full depth I prefer the latter - at least for the shorter part. It took less cuts so I assume didn't wear the cutter as much.

Having said that you're clearly having great success with the shallow cuts going down a step at a time so I don't claim one is objectively better.

The reason I like coming in from outside the stock and clearing it away is that it gives more room for the chips to fall away. Even though I have ordered the air/mister nozzle (only $18 AUD, but recommended by a friend) to blow the chips away I know I won't bother to fit it for who knows how long. The 'quiet' compressor I bought is just as noisy as my rattly old original so that both ended up being a waste of money and puts me off having it in use continuously. I reckon it will fire up every few minutes or so with even a small amount of air being used - it's the same as the one sold by Tormach with a different label, but it's useless.

[Roger]

I wouldn't worry about clearing chips, at least for roughing cuts, it really doesn't matter.

[David]

I drilled all the rivet holes in the tank plates of a tender today. It's the same as mine, but mine was done about 7 years ago so I had to draw up the model first. I did that about a month ago and it took about 10 hours of fiddling. I modeled the internal angles etc so the lower rivets fit better on this set than mine did.

Anyway, the front and back were simple enough, and I milled out the coal opening on the front plate.

The sides are too long for the machine to do in one hit so I had to square off the right side and use the lower-right corner as the origin. I could drill most of the holes in that setup. Then I had to slide it across and use the bottom-leftmost hole just drilled as the origin for the second setup. It went better than expected, I thought I'd have a lot of trouble with moving the stock.

For alignment I put two parallels in the bottom slot of the table and pushed the stock hard against it. The parallels are not a good fit in the slots but I figured given they're the same they should tilt the same amount and it would work. That made it easy to keep the stock aligned on the X axis and keep the Y reference during the move. I knew the reference hole Y dimension for the second setup so knowing both the current Y and the required Y I only had to fiddle for a few seconds to line the drill up on the hole in the X direction.

The 1.6m drill was at 5000rpm, 65mm/min feed. The 1.2mm drill was 5000rpm and 30mm/min feed. Hundreds of 1.6mm holes on the one drill!