Poor surface surface finish milling steel

[s dParticipant @sd79178]

Is it possible to achieve smooth surfaces when cutting with the side of an end mill in stainless steel (316)?

I have been able to get very acceptable smooth finishes on the lathe, but the finish on the mill is very uneven – reticulated might be the right word to describe it, and difficult to sand out. I'm not sure if this is user error, chatter or perfectly normal?

I'm using as little tool stickout as possible in an ER32 collet, one was a 10mm the other a 5mm end mill.

I also tried eliminating the vice but had similar results with the work bolted direct to the table.

The only thing I've noticed is a knocking from the upper part of the spindle with it in neutral and rotating by hand, and some flex in the column of about +/-0.075mm at the collet pushing it by hand. No idea if either is normal or not.

Perhaps my expectations are too high?

Here are some pics

Another piece after a quick sand to see how deep the lines are.Edited By s d on 04/07/2023 12:56:22

Edited By s d on 04/07/2023 13:01:42

Edited By s d on 04/07/2023 13:02:25

[s dParticipant @sd79178]

[JasonBModerator @jasonb]

A few more details would help such as vertical height being cut, amount of sideways depth of cut, spindle speed and feed rate for both cutters as well as hss or carbide and number of flutes and also what mill is it.

Edited By JasonB on 04/07/2023 13:03:38

[s dParticipant @sd79178]

Posted by JasonB on 04/07/2023 13:02:45:

A few more details would help such as vertical height being cut, amount of sideways depth of cut, spindle speed and feed rate for both cutters as well as hss or carbide and number of flutes and also what mill is it.

Edited By JasonB on 04/07/2023 13:03:38

Yes of course…

Chester v30 Mill, similar to Warco WM18 I believe?

4 flute end mills

10mm is 30 degree helix AlCrN coated HSS

5mm (actually it was 6mm) is 30 degree helix TIAIN coated HSS

(I do have some in carbide which I haven't tried yet)

Speed about 2000rpm, but it varied it and it didn't make much difference.

Manually feeding cuts about 8-12mm vertical, depth of cut maybe up to about 0.3mm, again it varied.

[Anonymous]

Of the austenitic stainless steels 303 and 316 machine very well, but for some reason 304 is a pig. It is possible to get a good finish on 316. However I can see a number of potential issues.

First what is the provenance of the cutters, manufacturer and supplier?

For a 10mm HSS cutter 2000rpm is way too fast, should be more like 500rpm, and that's based on recommended speeds for industry.

Work hardening is a real problem with 316. Taking a relatively shallow depth of cut means you need to feed faster than one might expect due to chip thinning.

The play in the column seems excessive to me.

I suspect the mill simply isn't rigid enough to take the cuts especially with conventional milling where the cutter will be rubbing at the start of the cut. Which is death to the cutter and the finish. It helps to climb mill, although I don't know if the smaller mills will be up to that?

Andrew

[s dParticipant @sd79178]

Posted by Andrew Johnston on 04/07/2023 13:51:50:

Of the austenitic stainless steels 303 and 316 machine very well, but for some reason 304 is a pig. It is possible to get a good finish on 316. However I can see a number of potential issues.

First what is the provenance of the cutters, manufacturer and supplier?

For a 10mm HSS cutter 2000rpm is way too fast, should be more like 500rpm, and that's based on recommended speeds for industry.

Work hardening is a real problem with 316. Taking a relatively shallow depth of cut means you need to feed faster than one might expect due to chip thinning.

The play in the column seems excessive to me.

I suspect the mill simply isn't rigid enough to take the cuts especially with conventional milling where the cutter will be rubbing at the start of the cut. Which is death to the cutter and the finish. It helps to climb mill, although I don't know if the smaller mills will be up to that?

Andrew

Great info, thanks Andrew.

I haven't tried anything near 500 rpm, so I'll test that next.

The mill is about 260kg. I was surprised about the amount of flex too. It's not in the spindle or collet or tool (measuring from the head housing to the tool), that all seems very rigid. But measuring off the table, it doesn't take much human effort to flex the column, pushing either the spindle or the top of the column itself.

Experience is in short supply here, so accounting for workhardening is going to be a tricky for me to manage. Need to put in the hours (and days and weeks)!

I tried climb milling and did get slightly more consistent finish, but still the reticulation. Could it be not enough flute engagement? Not taking deep enough cuts to keep a constant pressure causing the tool to bounce?

Milling seems to be much trickier than turning.

Tools are from ARC in the UK, their own branded stuff. Maybe I should look at getting better cutters.

Edited By s d on 04/07/2023 14:05:01

[JasonBModerator @jasonb]

As Andrew says 2000rpm is fast for an HSS cutter, even if it were OK you would have needed to be feeding at a minimum of 200mm/min to avoid the cutter rubbing (0.025mm chip load). Once the cutter starts to rub you can start to loose the edge and also risk work hardening so cutters could now not be at their best.

It would be worth checking that he spindle bearings are not too loose, usually a nut and locknut at the top that will take up any play. Also lock all the other axis except the one you ar eusing to feed with

[Anonymous]

I'm not clear exactly which cutters from Arc are being used? I have not used their HSS cutters, but have tried their premium carbide endmills and was impressed.

The cutting parameters should be fine, but I suspect the mill column isn't stiff enough. Of course HSS cutters are less stiff than carbide so the cutter itself might be flexing as well.

Andrew

[s dParticipant @sd79178]

Posted by JasonB on 04/07/2023 14:04:51:

As Andrew says 2000rpm is fast for an HSS cutter, even if it were OK you would have needed to be feeding at a minimum of 200mm/min to avoid the cutter rubbing (0.025mm chip load). Once the cutter starts to rub you can start to loose the edge and also risk work hardening so cutters could now not be at their best.

It would be worth checking that he spindle bearings are not too loose, usually a nut and locknut at the top that will take up any play. Also lock all the other axis except the one you ar eusing to feed with

I haven't considered rubbing, but can see why it would be a big problem.

Will check the top bearings… I notice that the top is a bit eccentric. Might just be the drawbar though.

[JasonBModerator @jasonb]

No I can't see that coating mentioned, The only 4 flute are the gold coloured ones , if it is those then get the premium ones which are considerably better both HSS and Carbide

[s dParticipant @sd79178]

Posted by Andrew Johnston on 04/07/2023 14:24:04:

I'm not clear exactly which cutters from Arc are being used? I have not used their HSS cutters, but have tried their premium carbide endmills and was impressed.

The cutting parameters should be fine, but I suspect the mill column isn't stiff enough. Of course HSS cutters are less stiff than carbide so the cutter itself might be flexing as well.

Andrew

I believe it's these, which are 3 flute not 4, my mistake… the rougher I bought was 4 flute.

https://www.arceurotrade.co.uk/Catalogue/Cutting-Tools/Milling-Cutters/ARC-Premium-HSS-AL-End-Mills/3-Flute-HSS-AL-End-Mill-Long-Series-TiAlN-Coated

edit – standard length not long

https://www.arceurotrade.co.uk/Catalogue/Cutting-Tools/Milling-Cutters/ARC-Premium-HSS-AL-End-Mills/3-Flute-HSS-AL-End-Mill-Standard-Length-TiAlN-Coated

I tried a carbide 5mm, 3 flute at 500 rpm plus I cranked a bit faster and got better results.. thanks!

I've no doubt wrecked the HSS ones with too high rpm. But the lower speed and faster feed does seem to improve things.

I could sand out the ridges more easily, but I'd like to have none! Will investigate rigidity further.

Edited By s d on 04/07/2023 14:43:57

[JasonBModerator @jasonb]

The 5mm could be run faster than the 10mm approx twice the speed if HSS and if it is carbide then your 2000rpm would be OK.

Out of interest is there any chatter which can often be heard as as squeal while cutting and what is the swarf coming off like? If very fine more dust like then you are not cutting, it should be nice chips.

Although this is just EN3 steel it should give you an idea of how things should sound and the chips produced, towards the end you can see how fast I'm turning the handwheel (2mm pitch screw) . This was a 10mm 4-flute HSS cutter at about 800rpm (25m/min) as it was mild steel

[Martin ConnellyParticipant @martinconnelly55370]

The knocking at the top of the shaft may be clearance play between the male and female splines of the drive.

Martin C

[SillyOldDufferModerator @sillyoldduffer]

I avoid machining Stainless because most of them work-harden. By no means impossible, but expect trouble. Here's what the British Stainless Steel Association say, my bold:

When machining stainless steels it important to ensure that there is no dwell or rubbing caused by machine vibration or tool chatter. Machines must be ‘substantial’ and capable of making the deep cuts needed in machining austenitic stainless steel without slowing down the set feed or surface speeds. Small training or ‘hobbies’ lathes and milling machines intended for machining mild steel, brasses etc. are unlikely to be substantial enough for the successful machining of stainless steels.

By 'successful machining' they mean reliably cutting metal to size and finish commercially without needing a skilled operator to experiment for best results. All will be well using a rigid powerful machine fitted with the right type of cutter, spinning at the correct RPM, with a suitable Depth-of-Cut and steady Feed Rate, suitable lubrication/cooling, and a way keeping swarf out of the cutting area.

Of 316 Alco say:

316 stainless steel has good machinability. Machining can be enhanced using the following rules:

• ‹ Cutting edges must be kept sharp. Dull edges cause excess work hardening.
• ‹ Cuts should be light but deep enough to prevent work hardening by riding on the surface of the material.
• ‹ Chip breakers should be employed to assist in ensuring swarf remains clear of the work
• ‹ Low thermal conductivity of austenitic alloys results in heat concentrating at the cutting edges. This means coolants and lubricants are necessary and must be used in large quantities.

So the odds are stacked against small workshops. My WM18 does what I want, but it's not particularly rigid, or powerful, I only own a limited range of cutters, they're not all in good condition, my experience of stainless is limited, and I'm not a naturally talented machinist. Whilst I and the machine cut machinable alloys reliably well, I'm not surprised when any of the many difficult Alloys turns out to be a challenge. I avoid scrap unless I know what it is.

SD's photos show, I think, the result of work-hardening. Rather than cutting, the cutter is rubbing and bouncing along the surface. Rubbing hardens the surface so effectively that HSS struggles to penetrate and is rapidly blunted, the end.

All is not lost! The finish can be improved by using an inexpensive Belt Sander like this example as a Linisher:

Not sure what others find, but in my workshop milling and lathe cut surfaces often benefit from a mild abrasive touch-up. Depends on the material, but ordinary mild-steel usually gets a licking because it's a bit smeary. Leaded mild-steel, 6082 Ali and Brass are more likely to come clean off the machine.

Dave

[Anonymous]

Don't know why people seem to fight shy of working stainless, just work to your machines limitations. As Andrew says above 303 is a dream to turn or mill, it doesn't particularly work/heat harden easily and polishes easily to mirror, 316 is nearly as good. Never had a problem with either using a WM16 typeish SPG mill and Mini and DB10 lathes. Just avoid 304 as it's only claim to fame is it welds nicely but is a right pig to get a decent machined finish.

[Chris MateParticipant @chrismate31303]

The shiny pattern in picture-?
As you turn the handle of the moving axis, the other axis moves(not locked), or play(gib) in same/moving axis.

-Main culumn locked down-?
-Have you locked the axis you not using-?
-Climb(Against) or conventional milling(pulling cutter)-?

Edited By Chris Mate on 04/07/2023 22:08:16

[s dParticipant @sd79178]

Posted by JasonB on 04/07/2023 14:59:05:

The 5mm could be run faster than the 10mm approx twice the speed if HSS and if it is carbide then your 2000rpm would be OK.

Out of interest is there any chatter which can often be heard as as squeal while cutting and what is the swarf coming off like? If very fine more dust like then you are not cutting, it should be nice chips.

Although this is just EN3 steel it should give you an idea of how things should sound and the chips produced, towards the end you can see how fast I'm turning the handwheel (2mm pitch screw) . This was a 10mm 4-flute HSS cutter at about 800rpm (25m/min) as it was mild steel

That video is very helpful thanks. Not getting anything like that kind of finish, I'd be happy with that. The lower speed helped but I'm still getting this deep grooving imprinted in the work.

Also in brass, though to a much lesser extent. Cold rolled steel is about as bad as the stainless 316.

If I copy your process exactly, the tool is still cutting a not insignificant amount of material on the return (climb milling) pass, it isn't just skimming over it. Then if I repeat the conventional milling pass without changing anything, it cuts even more than the return pass. This should not happen, correct?

The sound is very buzzy and I can feel a lot of vibration. It doesn't sound smooth like in your video.

[s dParticipant @sd79178]

Seeing if this video ebed works… it does…. So this is making three passes without changing any settings. 510rpm. Everything not moving locked. 6mm HSS coated 3F.

Edited By s d on 05/07/2023 09:03:59

Edited By s d on 05/07/2023 09:04:46

[Anonymous]

The plot thickens; it is not an issue with 316 but milling in general.

For a start there is too much stick out on the tool. The holder should be down to the top of the flutes. Given that there is significant cutting on the return pass something is moving that shouldn't be. I suspect the cutter is flexing for starters.

Andrew

Edited By Andrew Johnston on 05/07/2023 10:28:47

[s dParticipant @sd79178]

Posted by Andrew Johnston on 05/07/2023 10:28:29:

The plot thickens; it is not an issue with 316 but milling in general.

For a start there is too much stick out on the tool. The holder should be down to the top of the flutes. Given that there is significant cutting on the return pass something is moving that shouldn't be. I suspect the cutter is flexing for starters.

Andrew

Edited By Andrew Johnston on 05/07/2023 10:28:47

Thanks Andrew. Will bury the tool and try again!

Probably to be expected but face milling produces clean results (well, acceptable enough as a starting point).

—–

EDIT: buried the 6mm to the top of the flutes and got the same result. Cutting on all three passes in 316.

Edited By s d on 05/07/2023 10:50:32

[John Doe 2Participant @johndoe2]

I know almost nothing about machining – so please be gentle – but the OP says they are using the side of an end-mill cutter?

Are they designed for that? I am just wondering if the side flutes of a cutter produced for end milling would be machined to precise tolerances, or if one flute might be fractionally more proud than the others, causing a regular pattern in your work, or chatter?

[Anonymous]

Posted by John Doe 2 on 05/07/2023 10:42:59:

Are they designed for that?

Yes they are; the name endmill is a misnomer. They are intended for cutting using the side flutes.

Andrew

[s dParticipant @sd79178]

So here's the facing vs side milling. I'm happy enough with the face finish, those ridges are fairly even and the surface feels smooth. This is with a 10mm rougher (the side milling was with the 6mm HSS 3F I think).

The rougher doing side milling is better than the other tools, it's much more regular, but still has those vertical dents.

[Martin ConnellyParticipant @martinconnelly55370]

Anything that can be done to stiffen the process will help so if all the none moving axes are locked and the stick out of both the spindle in the head and the tool in the collet is reduced to the minimum then the next question is are you tightening the tool in the collet sufficiently to reduce flex. If you are not using a ball bearing ER nut and suitable wrenches to put high torque on the nut and therefore high pressure on the tool shank then the tool position may flex slightly in the collet holder.

Martin C

[John Doe 2Participant @johndoe2]

Ah, fair enough.

Do we know then, if the milling bit is true and regular ? – is it possible to check each flute "diameter" with a DTI? – perhaps one is slightly proud compared to the others.

In the same vein; does a DTI show any bend in the driving shaft, as measured against the side of the cutter as it is rotated through 360°.

 

.

Edited By John Doe 2 on 05/07/2023 12:33:28

[Author]

Posts