PDA

View Full Version : How to make a very smooth surface on the mill?



beanbag
06-13-2010, 06:42 PM
I need an even smoother surface than a face mill can provide. My face mill can make a mostly shiny surface, but still leaves tiny grooves that you can't feel, but can see. I also noticed a larger groove spacing approx .1" apart, maybe from me turning the hand wheels on the stage in a not perfectly even manner. In the end, I want to wet sand and polish the surface to be mirror shiny. Is there some kind of a buffing or burnishing attachment for the mill?

loose nut
06-13-2010, 07:47 PM
Get a piece of plate glass or a cheap surface plate, put the fine emery paper (250 to 400 grit) on it and rub, change to finer grades as you go. You can get up 4000 grit or better at auto supply houses. Be careful to rotate the work so that it is polished flat and evenly all over.

That's one way, maybe not the best but it works.

Your Old Dog
06-13-2010, 07:48 PM
I'm not aware of any polishing technique on the mill. Many guys use a linisher (fancy name for a belt sander with something like 80 or 120 grit paper. From there you can hand sand and it's a simple matter to buff it up on a wheel.

Mine looks a bit like this only without the 9" diameter wheel on the side. Bought it at a yard sale for $20.00.

http://woodzone.com/Merchant2/tips/g10201.jpg

PixMan
06-13-2010, 07:52 PM
It sounds to me like you have one insert (or tooth?) in your face mill that's below the others. Have you checked that? What kind of face mill are you using?

KiddZimaHater
06-13-2010, 10:18 PM
The best finish is usually made with a fly cutter, with a light finishing pass.

Mcgyver
06-13-2010, 10:30 PM
big sharp slab mill in a horizontal.....best finish you can get next to ground :D

wierdscience
06-13-2010, 10:42 PM
Try inserts with a larger tip radius,or leave a finish allowance of say .005" and switch to a fly cutter with a fairly large radius on the cutting edge.That edge can be ground back on an angle to the spindle axis and canted to the topside of the toolbit.Kinda of like a sandwedge for metal cutting:) Hone that edge with a fine hone and use coolant or something like WD to combat chip welding.

Power feed if you don't have it will help also.

reggie_obe
06-13-2010, 10:50 PM
Try tramming your mill head with a tenths indicator and see if it doesn't improve the finish.

RobbieKnobbie
06-13-2010, 10:52 PM
If you're getting visible finish lines that can't be fealt when you drag your fingernail accross them, you're doing pretty good.

One trick I used to use on a job that called for an 8 finish on one particular machined face was a cratex wheel. I had to change the tool offset between almost every other part, but I never failed a part for finish specs.

The down side is that I had to bring the spindle pretty far up to get the wheel to polish - higher than I could go on a b'port anyways.

lakeside53
06-13-2010, 11:00 PM
It sounds to me like you have one insert (or tooth?) in your face mill that's below the others. Have you checked that? What kind of face mill are you using?

This is very common - inserts are in various grades - but most are only within a couple of thou, and that make a huge difference on a face mill with multiple inserts.

As a test - for a finish pass - remove all the inserts except one.. and adjust the doc/feed rate accordingly. of course... the face mill now behaves like a fly cutter.

darryl
06-13-2010, 11:09 PM
Tramming, yes. Even the smoothest and best cutting tooling will be leaving ridges if the tram is out. Then there's swarf removal- if it gets dragged under a cutting edge it can leave a groove deeper than what you could easily polish out.

Also, how are the table movements- if it's somewhat loose you could be rocking the table a tad when you crank the handwheel. That would give you an 'inconsistency' every 100 thou.

Evan
06-14-2010, 01:10 AM
Your face mill is out. This is the finish from the facemill I made a while ago.

http://ixian.ca/pics6/facemill3.jpg

http://ixian.ca/pics6/finish4.jpg

Jim Shaper
06-14-2010, 01:15 AM
Surface grinder. ;)

Robin R
06-14-2010, 01:16 AM
This is very common - inserts are in various grades - but most are only within a couple of thou, and that make a huge difference on a face mill with multiple inserts.

As a test - for a finish pass - remove all the inserts except one.. and adjust the doc/feed rate accordingly. of course... the face mill now behaves like a fly cutter.

Presumably adjusting the feed rate to what you would use for a single insert, but leaving all the inserts in place, should give the same result.

oldtiffie
06-14-2010, 01:48 AM
I need an even smoother surface than a face mill can provide. My face mill can make a mostly shiny surface, but still leaves tiny grooves that you can't feel, but can see. I also noticed a larger groove spacing approx .1" apart, maybe from me turning the hand wheels on the stage in a not perfectly even manner. In the end, I want to wet sand and polish the surface to be mirror shiny. Is there some kind of a buffing or burnishing attachment for the mill?

BB.

I notice that you didn't say what material/s you plan to cut.

Have a single HSS fly-cutter mounted with a very large "curve" shaped (almost flat) cutting edge.

Run it over the previous cut - slow revs and "backward" - it will act as a burnishing tool - but keep the job very clean of swarf from previous cuts etc. You will need a good amount of cutting (or tapping) oil and a fairly high feed rate - just below where the "swirls" start to show.

Go easy on the "depth of cut" as we want a rubbing action - not a cutting one

The edge on a HSS cutter will stand it where-as a TC may not.

The end of the "cutter" can also be a small part of a very large sphere - might be even better.

In all cases the cutting edge must be very finely honed - and kept that way.

Give it a try anyway.

lakeside53
06-14-2010, 03:07 AM
Presumably adjusting the feed rate to what you would use for a single insert, but leaving all the inserts in place, should give the same result.


In theory, but then the deeper cutting insert is just bludgeoning the already "pre-cut" surface - not really cutting... Carbide inserts have a minimum cutting depth and feed rate for optimal surface finish. Increasing DOC and feed often gives better results than "whisker" cuts. With optimal cuts and feeds using quality inserts on my 2.5 inch face mill, (45 oriented high rake SD) I can get a mirror finish on mild steel (not always!). On my APDK insert face mills, I have one or more inserts maybe 1/2 thou different - and it shows.

Tramming.. well... yes, in theory a perfect tram will allow a perfect overlap on multiple passes of say a 3 inch face mill without a ridge - on a perfect machine. Mine's not prefect. I can tram to within a couple of 10ths in say 6 inches for a vice held part. Mount a big face mill and something is pushed (usually "nod") by the milling forces. I can compensate for this by biasing the nod forward a 1/2 thou.. but don't usually bother as it will just mess up some future cuts. Old iron... but it works;)

Black_Moons
06-14-2010, 03:49 AM
I consider mill toolmarks a fact of life. Its why sandpaper/files/grinders/etc where invented. Faster to just take them out manualy then it is to try and get your mill to leave a perfict finish.

At least, it is after you spend about 1/2 an hour getting your mill to give you a really good, but still not perfict finish.

BadDog
06-14-2010, 04:07 AM
For convenience and cost, it's hard to beat a good fly cutter of sufficient size to complete the surface in one pass. I use a Face Mill when I'm impatient and/or need to remove material at the maximum rate my mill can handle. When I need top finish as machined, I use a fly cutter.

Forrest Addy
06-14-2010, 05:20 AM
Depends on how flat you want it and the material.

Milling Vs flycutting have been pretty well covered. That leaves second op fnishing. Sounds like surface grinding may not be an option for the OP so we are down to some form of abrasive sheet or loose abrasive lapping if we are to secure a mirror reflective surface.

If you want shiny and flat abrasive sheet lap it through a succession of wet or dry grit sheets 'til you get to 2000 and a ghostly reflection in the matte surface. Shinier, continue to 4000 (finest I've seen in abrasive sheets.) After that move on to 3M polishing film. Use a good flat as a substrate for the abrasive sheet and mineral spirits to float away the swarf. It's a lot of work to do the job right. A LOT of work.

If you want merely shiney, dust off the worst of the tool marks with the convex side of a good flat file then buff the surface with a cloth wheel and buffing compound.

Loose abrasive lap it on glass if you wish but it works poorly, slowly, and rounds off the edges unless you are scrupulous in distributing wear. Loose abrasive lap on cast iron if you can but be prepared to re-condition the lap frequently so it stays flat.

I know many declare lapping on glass the apotheosis of lapping technique but glass laps several time faster than the work. In fact, glass is the worst possible choice for a lap in loose abrasive lapping. Here's why: you want to lap the work, not the tool. The lap (tool) need to be softer than the work and of a character to hold the abrasive so it cuts as the work is rubbed over it. Glass is harder than almost every common material and has among the lowest energy of rupture. Glass laps very rapidly compared to steel area for area.

Those who declare success in loose abrasive lapping on glass have never had a serious trial using efficient technique and materials. Yes, it can be made to work but once you compared lapping on cast iron or leaded bronze to glass, you will never go back to glass.

beanbag
06-14-2010, 05:44 AM
Thanks for all the suggestions. I didn't mention a tool or material because I meant for it to be a general question, but in this case, the material is Aluminum, and the tool is a Sandvik 45 deg face mill with Aluminum cutting inserts.

1) I don't have a fly cutter
2) I use a communal mill. I checked the tram before facing, and it was within .001 per 6".
3) The face mill was bought used, so maybe the inserts aren't that even. How would I check?
4) Another option I could try is that I have some slightly less sharp cermet inserts.
5) In terms of burnishing ideas, I also have a "medium roughing" insert that came with the face mill, i.e. it purposely has a rounded edge.

This time, I went with wet sanding with a sanding block (a.k.a. sandpaper wrapped over a piece of glass). It didn't take that long to go thru the grits, but the highest I had was 2000, which still left visible scratches. Then I had to jump to Mother's Aluminum polish. I could get the aluminum shiny, but I could never get it perfectly flat, like it had some tiny uniform texture in it, maybe about .1mm feature size. Is this the grain structure of the aluminum?

Next time, I will try some of the suggestions offered.

PixMan
06-14-2010, 08:32 AM
I don't know about hand finishing being faster or easier than a good face mill. I've got a few face mills, and find that a good-quality name-brand cutter with "G" tolerance inserts will get me a finish as good or better than the fly cutters I have...and a whole lot faster.

I don't have anything big. The nicest one is an old Widia 2-1/2" 45-lead 4-insert mill. It leaves a finish very similar to that shown in Evan's photo. I'm lucky to know have a 6x18 surface grinder to make nice surfaces on most materials, though aluminum doesn't grind well.

It sounds like to OP has a good cutter, and good inserts (because Sandvik Coromant doesn't have too many third-party companies making inserts for their cutters.) I would suspect the machine and possibly the material. Some aluminum plate just won't shine well. "Mic 6" tooling plate comes to mind. It's garbage: Machines like crap and looks like crap.

Seems to me that the OP is getting the best he can get out of what tools he has to work with. Try a fly cutter once just to prove it out, unless you have a dial test indicator to check the cutting inserts as they sit in the spindle.

Evan
06-14-2010, 08:41 AM
No need to get fancy when testing the set of the inserts. Just place the face mill near the edge of a piece of plate so that only one insert can contact the work and start turning the spindle by hand as you lower it very slightly. It is easy to tell the difference of even less that .001" by how much effort it takes to turn the tool through the work by hand, one insert at a time.

small.planes
06-14-2010, 09:05 AM
My face mill can make a mostly shiny surface, but still leaves tiny grooves that you can't feel, but can see.


This is the finish from the facemill I made a while ago.
http://ixian.ca/pics6/finish4.jpg

Which also has lines the I can see quite clearly in the photo...

I have had good finishes look variable because of 'pores' for want of a better word in the base material.
What is the parentage of the workpiece? Al can have quite a bad porosity if the material is not carefully made.
My home cast parts often have areas of (presumably) hydrogen pores, which dont matter for what I use them for.

Dave

Evan
06-14-2010, 09:29 AM
Which also has lines the I can see quite clearly in the photo...


The eye can easily discern lines that are less than .0001" deep. To appear optically smooth the surface must have a variation not more than a wavelength of light. The surface of the piece in the lower photo has a variation of not more than about .0002".

http://ixian.ca/pics6/finish3.jpg

small.planes
06-14-2010, 09:51 AM
Your face mill is out. This is the finish from the facemill I made a while ago.
<Pictures Snipped>

Sorry, I should have quoted all the words you wrote (Emphasis mine), which implied that your face mill gave perfect results, when actually its exactly the same as the OP stated, a smooth surface, but with visible lines.

I assume hes actually trying to make a mirror or similar, and so some indication of how to do this (Im pretty sure youve claimed to be an expert in mirrors, and have reasonably proved you work in this area - telescopes etc) would have been more helpful than a couple of pictures illustrating how the mighty facemill with micron tolerances (I rememeber that thread ;) ) also makes pretty lines in flat surfaces.

Dave

Evan
06-14-2010, 10:04 AM
I assume hes actually trying to make a mirror or similar, and so some indication of how to do this (Im pretty sure youve claimed to be an expert in mirrors, and have reasonably proved you work in this area - telescopes etc) would have been more helpful than a couple of pictures illustrating how the mighty facemill with micron tolerances (I rememeber that thread ) also makes pretty lines in flat surfaces.


The point of my post is that a facemill can produce a finish that is easily polished to a mirror finish. There isn't a lot of visible difference between a visible line that is .001 deep and one that is .0002 deep but the (difference in) effort involved in polishing is tremendous. You spend 10% of the time getting rid of 90% of the lines and 90% of the time getting rid of 10% of the lines. Starting with the best possible finish a tool can produce can save much of that time.

The finish I show above is the number one and most important step in polishing metal.

small.planes
06-14-2010, 10:29 AM
You should have just mentioned that several posts ago, rather than just saying the OP face mill is no good. I think you normally insist on having all the facts :rolleyes:


Dave

psomero
06-14-2010, 12:23 PM
if it was still scratched up looking after you went through the stages of paper you had, you jumped from grit to grit too quickly...

914Wilhelm
06-14-2010, 01:44 PM
Sometimes if I want a smooth appearing, not shiny, finish I'll throw the part in the blast cabinet with some glass beads. This gets rid of the tool marks and leaves a nice matte finish.

Evan
06-14-2010, 02:08 PM
You should have just mentioned that several posts ago, rather than just saying the OP face mill is no good. I think you normally insist on having all the facts

I said it was "out". Fix that and the problem goes away.

Black_Moons
06-14-2010, 02:53 PM
if it was still scratched up looking after you went through the stages of paper you had, you jumped from grit to grit too quickly...

the right time to switch from one grit to another (Afaik..) is when theres no marks from the previous grit (or toolmarks)

Its easyest to see this if you alternate directions for sanding. when all the marks going one way disappear, you know its time to switch to the next grit.

Re: Loose laping on glass
Yea I have no idea who invented that either, I can see it working well with abrasive sheet layed or glued onto the glass, but not loose abrasive.

I wonder if anyone makes a sorta thin PSA sheet for puting onto glass that could be easily charged with loose abrasive. Could be a sorta best of both worlds, wear down the plastic sheet, then throw it out and replace insted of trying to recondition the lap to flatness.

I wonder what materials would be good for such a sheet.. Offhand the first one that comes to mind would be UHMW plastic.. but im no expert.. UHMW would seem nice to me due to its hardness yet likey to embed grit, non afinity for asorbing moisture, low friction to workpeice.

JCHannum
06-14-2010, 03:26 PM
It sounds as though you are hand feeding the mill table. If this is the case, a power feed will provide a smoother finish. Hand feeding will cause the table to rise and fall as the handwheel is turned.

Even if the face mill is "out", a smooth finish can be produced with a slow table feed. Regardless of the type of cutter, face cutter or flycutter, a swirled appearing finish will be the result.

Polishing to a 2000 grit should produce almost a mirror finish if done properly. Back up the abrasive with a hard surface, change direction 90 or 45 degrees with each change of grits and clean thoroughly when changing grits.

small.planes
06-14-2010, 03:50 PM
I said it was "out". Fix that and the problem goes away.

Yes, highly useful advice. 'out' is so quantitative.

Im not sure that the OP actually has a real problem:



My face mill can make a mostly shiny surface, but still leaves tiny grooves that you can't feel, but can see

ISTR that the finger can also determine roughness of well under a thou, but my roughness standards are at work, so I cannot check how rough feels smooth.
Optical flatness is of course 'more flat', but finger smooth finishes are not that far away with a little polishing.

Dave

beanbag
06-14-2010, 04:33 PM
if it was still scratched up looking after you went through the stages of paper you had, you jumped from grit to grit too quickly...

No, it's not scratched looking. The texture is more "grainy", like sand, I guess. If my camera can zoom enough, I'll grab a pic later.

Evan
06-14-2010, 05:51 PM
Yes, highly useful advice. 'out' is so quantitative.


What is obvious is that you are simply trying to pick a fight.

You had better get on Darryl's case too then since he wrote:


Even the smoothest and best cutting tooling will be leaving ridges if the tram is out.

You have also just limited your own use of the term "out" to zero at the risk of appearing petty. Wait. Too late.

small.planes
06-15-2010, 05:06 AM
In for a penny, in for a pound...

In Darryl's case he stated a generalism that is a normallly understood machining term.
Having a tram that is out is indeed not tying it down to microns.
It is however something that even a novice would understand what is wrong (or be able to search for it), and possibly how to take steps to determine by how much, and how to fix it.

Saying:


Your face mill is out.

is not a normal generalised machining statement, and does not give a clue as to which part of the face mill might be 'out'.
I have had a bad finish with my face mill when the retaining bolt was not fully tightened.
It was not sufficiently loose to wobble, but the bolt was not torqued up, and hence allowed the mill to move very slightly.
I have also had mirror finishes with the same face mill that dissappeared partway through a 300mm cut, only to reappear slightly further on.
That time it was not the face mill, or the milling machine, but the base metal.
Or maybe the arbour is slightly bent, or there is one insert at a slightly different angle, or a piece of swarf trapped somewhere. etc...

Its a bit like posting some pictures of a smooth finish with lines in it and not saying that this finish is what you need to aim for before you start polishing.
Useless.

and on that note Evan I will bow out of this discussion between us, but if I can add something USEFUL to the OP thread then I will do so.

Dave

Evan
06-15-2010, 08:04 AM
but if I can add something USEFUL to the OP thread then I will do so.


So far your score on that count is an own goal.

Ian B
06-15-2010, 10:34 AM
The statement has been made that if a mill is "out of tram", it will leave a rough finish.

Let's quantify that a little - say for the sake of argument that a 3" diameter facemill is being used, and the leading edge of the facemill when cutting along the length of the table is 5 thou lower than the trailing edge. If a cut is stopped half way through, it'd probably be just possible to get a 5 thou feeler gauge between the work and the trailing edge cutter tips.

The face mill would only be cutting on the leading edge. This amount of "out of tram" would be measurable by most HSM'ers.

It would produce a surface that is not quite flat, due to the lean of the spindle.

But as long as the tips are still cutting on their radiused portions, why would surface finish be any worse? Does surface finish depend on the trailing edge cutting across the ridges left by the leading edge?

Ian

Evan
06-15-2010, 12:29 PM
Does surface finish depend on the trailing edge cutting across the ridges left by the leading edge?


No. You are quite right. In fact if it is slightly "out" of tram it will produce a better finish without the swirls that it will make if the tram is nearly perfect. The problem then becomes a ridge that will be formed when a parallel pass is made with an overlap.

However, if the insert positions are "out" of alignment with each other then it will produce a series of lines whether or not the tram is in or out.

JCHannum
06-15-2010, 12:43 PM
However, if the insert positions are "out" of alignment with each other then it will produce a series of lines whether or not the tram is in or out.

Not necessarily, if by "out" of alignment you mean one is high (low?) in relation to the others, the face mill will act the same as a fly cutter, the proudest cutter will bear the most of the cutting action. If table feed is reduced sufficiently, a good finish can be obtained all else being equal.

BobWarfield
06-15-2010, 01:24 PM
Lots of dancing around an inherent truth, which is that these cutters leave grooves. You can adjust tram (and yes, many like a little out of tram, see specs on my mill surface finish page:
http://www.cnccookbook.com/MTMillSurfaceFinish.htm) and many other things, but you're going to get those tiny grooves.

If you do everything just right, you can get to where you have "rainbow" grooves as they're so small and close they produce diffraction effects. It takes a well adjusted machine, a good face mill, just the right toolpath, just the right feeds and speeds, just the right coolant, and brand new inserts (not clear how many passes you get before you need more new inserts). Have played with this both on commercial VMC's and hobby mills. The latter or a Bridgeport will get surpisingly close on the rainbow groove front.

But, that's a lot of labor and potentially insert cost. BTW, depending on your circumstances, "wiper" inserts can get closer (they're designed to do the "burnishing" that was mentioned), and PCD with a large radius in a flycutter is great in aluminum too. A lathe will often get closer to a mirror than a mill too.

In the end, if you want a real "mirror" you'll have to polish it. You can decide where the trade off lies between more care milling versus more time and grits in polish, but there's not much avoiding it.

Cheers,

BW

Evan
06-15-2010, 03:05 PM
Not necessarily, if by "out" of alignment you mean one is high (low?) in relation to the others, the face mill will act the same as a fly cutter, the proudest cutter will bear the most of the cutting action. If table feed is reduced sufficiently, a good finish can be obtained all else being equal.


That is true but only, as you say, if the feed is slow enough. At a "normal" feed rate which engages all cutters it will leave visible grooves.

Rich Carlstedt
06-15-2010, 03:53 PM
I think you fellows have strayed way off the point.
First, the poster said he had a finish that he could not feel (only see)
By definition, he has a finish at better than a RMA 32.
( If you can't feel cutter direction with a finger nail when blindfolded, it's less than 32)
THAT is the best a Milling surface can do ( In ordinary milling machines !) (forget the diamond stuff guys)

So the question was how to improve it.
Abrasives or burnishing are the only additional alternatives he has, that I can see.
My experience is only when the part is removed, can it be polished, so I can;t answer, that but What about yours?

PS
Traming has nothing to do with surface finish. He said he had a smooth surface already

Rich

aboard_epsilon
06-15-2010, 04:02 PM
Most of marks produced by cuttings getting dragged across surface by cutters.

So blow air on it in your final pass.,

Final pass should be of little depth ..cutter speed fast .feed slow

Then you should have good results .

all the best.markj

beanbag
06-17-2010, 05:59 AM
Update:

I did a bunch of facing tests on the Tormach CNC machine today. The machine was barely out of tram, and I ended up cutting on the leading edge. I also shimmed my inserts until they were within .0005" of each other. The cutter is a Sandvik 45 degree face mill using aluminum cutting inserts with a little flat right at the cutting edge.

I tried high RPM, low RPM, high feed, low feed, air blast, no air, coolant, oil, using only one insert, etc, and the surface was pretty much the same every time, i.e. I can see lines, but cannot feel them. Here are three pictures of the same piece:

http://i139.photobucket.com/albums/q286/beanbag137/IMG_0315a.jpg

http://i139.photobucket.com/albums/q286/beanbag137/IMG_0314a.jpg

http://i139.photobucket.com/albums/q286/beanbag137/IMG_0317a.jpg

You can't see in the pictures, but I can barely see additional tiny undulations perpendicular to the cutter grooves. I take this to be machine vibrations.

Spinning the cutter backwards, even at zero depth of cut, was a BAD idea.

A Cermet insert didn't seem to work quite as well. There was a tiny bit more shine due to burnishing, I think, but the overall surface roughness seemed worse, and it would occasionally cause a chip to stick to the surface. A blunt roughing insert with a very light cut gave an equally shiny surface, but on closer inspection was actually more lumpy, with microscopic "sand dune" ridges of metal being pushed around.

aboard_epsilon
06-17-2010, 09:47 AM
I see from the pics that you have the cutter centred on the work peice ..

try moving it over so the cutter only overhangs on one side ..and barely (0.5mm -1mm ) overhangs the other.

then you will have half the amount of interupted cuts.......interupted cuts make the whole tool flex with the shock.

thats as well as the air blowing and shallow low feed high speed last cut.
crude sketch illustration that i did some time ago


note the shallow angle of the cutters hitting the workpeice in the second illustration.

me having an older machine ..i notice the amount of noise and vibration cutter makes ..so adjust for the most silent running ..which also gives the best finish.

http://img.photobucket.com/albums/v190/aboard_epsilon/bridgeport/cutterpath2.jpg

all the best.markj

Evan
06-17-2010, 10:56 AM
The machine vibration is clearly visible in the supersamples I have derived from your photo. So is the tip flat of the inserts and it shows that in spite of your efforts to set the inserts to the same height what you are seeing is the difference in insert height.

http://ixian.ca/pics7/machinemarks1.jpg

Tony Ennis
06-17-2010, 11:50 AM
Cool photo Evan. How large are the artifacts we're seeing?

Evan
06-17-2010, 12:00 PM
I could guess approximately but without a ruler in the photo I can't be sure. I didn't keep track of the amount of supersampling I did so I would have to do it again to make any reasonable guess.

beanbag
06-17-2010, 06:14 PM
I see from the pics that you have the cutter centred on the work peice ..

try moving it over so the cutter only overhangs on one side ..and barely (0.5mm -1mm ) overhangs the other.

then you will have half the amount of interupted cuts.......interupted cuts make the whole tool flex with the shock.

thats as well as the air blowing and shallow low feed high speed last cut.
crude sketch illustration that i did some time ago


note the shallow angle of the cutters hitting the workpeice in the second illustration.

me having an older machine ..i notice the amount of noise and vibration cutter makes ..so adjust for the most silent running ..which also gives the best finish.


all the best.markj

Thanks for pointing this out. Normally I go for a 70% cut, but here I had multiple blocks mounted on the vice, so I couldn't offset the cutter by much.

However, I think the advice you gave is opposite to what you are supposed to do. In this case, you are supposed to position the cutter such that there is a glancing EXIT, not entry. The reason being that carbide is better in compression than tension, so if you have a thick chip on exit, that sudden release of force is bad for the insert. I was told this by an Iscar rep, and it is also explained in the Sandvik milling catalog.

beanbag
06-17-2010, 06:23 PM
The machine vibration is clearly visible in the supersamples I have derived from your photo. So is the tip flat of the inserts and it shows that in spite of your efforts to set the inserts to the same height what you are seeing is the difference in insert height.


Nice detective work. How did you create your image?

I think I can set the insert heights a little better if I actually use real shim material, and not pieces of paper laying around. But how much would that really help? Even my tests with the single cutter looked about the same.

As for the scale of the images, you can check the third image for the presence of lined paper and human writing ;)

aboard_epsilon
06-17-2010, 06:26 PM
Thanks for pointing this out. Normally I go for a 70% cut, but here I had multiple blocks mounted on the vice, so I couldn't offset the cutter by much.

However, I think the advice you gave is opposite to what you are supposed to do. In this case, you are supposed to position the cutter such that there is a glancing EXIT, not entry. The reason being that carbide is better in compression than tension, so if you have a thick chip on exit, that sudden release of force is bad for the insert. I was told this by an Iscar rep, and it is also explained in the Sandvik milling catalog.

well as Evan has said further up

vibrations ..

probably caused by the cutter hitting the work at angle in my first illustration ..

my bridgeport is old ..and any vibrations are magnified ..the spine shafts are worn ..and i move the cutter over to the best place that makes the least amount of racket...........which also gives the best finish ..

I've done a lot of work with stainless which is hard on cutters (inserts) .......and in an endevour to achieve the best finish results, so i have miniumum of polishing to do ...what i do is, as described.

anyway ...thats as much info as i can relay to you ..

others will comment

all the best.markj

beanbag
06-17-2010, 06:30 PM
I can try it your way too.

aboard_epsilon
06-17-2010, 06:38 PM
also

my machine finishes better climb milling .........so it may help to do your finishing cut on the way back.

all the best.markj

Evan
06-17-2010, 06:57 PM
Nice detective work. How did you create your image?


I would have to write a fairly lengthy tutorial to describe that. It isn't a one or even 10 step process. The most important part of the process is to select the sharpest portion of the image and then begin up sampling it a stage at a time. During that process I apply various manipulations such as sharpening, despeckling, blurring, unsharp masking, noise reduction and contrast enhancement. I also work in layers so that I can make a series of similar images using different sequences and then combine them to make the final image. It is a sort of synthetic image stacking process. It extracts information that is not visible to the eye but is contained in the image by the way the Jpeg algorithm encodes image data, especially at edges. The final image I work with is around 100 megabytes which is then downsampled for display.

It takes much longer to tell than it does for me to do but I have been fiddling graphics and optical systems for decades.

Robin R
06-17-2010, 11:38 PM
This may be a day late and a dolar short, but Black Moons in post #31 was musing as to whether anyone made a PSA backed plastic sheet, for sticking to glass. As it happens there is a Lee Valley product for just this use, not cheap though. http://www.leevalley.com/en/wood/page.aspx?p=33017&cat=1,43072

rowbare
06-18-2010, 12:42 PM
However, I think the advice you gave is opposite to what you are supposed to do. In this case, you are supposed to position the cutter such that there is a glancing EXIT, not entry. The reason being that carbide is better in compression than tension, so if you have a thick chip on exit, that sudden release of force is bad for the insert. I was told this by an Iscar rep, and it is also explained in the Sandvik milling catalog.

Bob Warfield had a blog post on this a short time ago. Look for "Rolling Into a Cut" dated 5/15/10 on http://www.cnccookbook.com/

bob

Wirecutter
06-18-2010, 01:02 PM
One trick I used to use on a job that called for an 8 finish on one particular machined face was a cratex wheel.

Totally agree! I got my hands on these cool abrasive wheels at work a while back, and I loved them. Took me a bit of searching and head-scratching to find out what they were called and buy some, but I like 'em. I've used them in the Dremel with a part turning in the lathe, but never in a rigid, steady-feeding machine such as a power-fed mill.

You should see the finish I can get in my humble little setup on 304 stainless.

-Mark

John Stevenson
06-18-2010, 06:59 PM
Had a couple of minutes tonight between jobs and dug my finishing flycutter out to try.

Now these pics are not good, I used macro but the lighting was all over.

http://www.stevenson-engineers.co.uk/files/finecut2.jpg

This is a piece of general quality alloy scrapbinium [ TM ] 10 thou cut 2,500 rpm and a dab of knacker lacquer on the top.

Looks rough with the tool marks but the vertical lines and swirls [ not the arcs ] are from me rubbing it with a bit of clean rag so you get an idea of the arc marks.

http://www.stevenson-engineers.co.uk/files/finecut1.jpg

This is cold rolled, 15 thou cut and again 2,500 rpm, no coolant.

The marks you can see but not feel, I could probably get better with a new insert and play with the speeds and feeds, perhaps 2,500 is a bit fast in steel ?

This is the cutter.

http://www.stevenson-engineers.co.uk/files/finecut3.jpg

You get a new life out the insert every 30 degrees and it's double sided.
No good for you Tiffie, it's been used.......

.

BobWarfield
06-18-2010, 09:07 PM
Those are nice flycutters for finish, John. You gotta love the round inserts--nice big radius and as you point out, you can rotate them to expose more surface. I love the round inserts on the lathe too.

You can definitely get a better finish than that beanbag, but it will still have grooves. Not that it isn't worth it to do better, but when you've gotten to diminishing returns, you have to decide whether to accept the grooves or get on with polishing.

Cheers,

BW

Doc Nickel
06-19-2010, 01:12 AM
I could guess approximately but without a ruler in the photo I can't be sure.

-If that's 60Hz vibration from the single-phase motor, if you knew the RPM and cutter diameter, the spacing and therefore scale could be extrapolated.

Doc.

PixMan
06-19-2010, 01:13 AM
Wrong insert for aluminum. I see built-up edge, a common failure when the insert isn't dead sharp in a soft material.

For future jobs in Al, see if you can get an uncoated one. Even if you can't, either way be sure to use some kind of cutting fluid.

Paul Alciatore
06-19-2010, 01:46 AM
if it was still scratched up looking after you went through the stages of paper you had, you jumped from grit to grit too quickly...


Or you didn't clean it scrupulously between grades. Just one grain of a coarser grit will ruin the work you do with a finer one.

Another thing, do use some oil or cutting fluid with the sandpaper. It improves the finish by several grades of grit at each level. This works with both power and hand lapping or grinding. You can get an almost optical finish with 2000 grit this way.

BobWarfield
06-20-2010, 04:02 PM
Here's some little cubes I did up yesterday.

Here is their actual size (0.600"):

http://www.cnccookbook.com/img/TurnersCubes/Jewelry/ActualSizeCube.jpg

That's not a very flattering angle, but I wanted to make the grooves visible. Take the photo as oblique as possible to maximize shiny. Even asphalt has a "mirror" finish at the right angle if you've seen the highway mirages.

The grooves are reasonably hard to see, and the cubes look very shiny in person. There are little diffraction rainbows that catch in the light. Hard to see, but there a little bit of one on the cube that is diagonally left of the bottom most one.

These were done at 20 IPM with a Glacern 3" 45 degree facemill. My spindle only goes 1600 rpm, which is awfully slow for this 6061. Depth of cut for the finish was 10 thousandths, and I had sharp "aluminum" inserts in it, but they were not new.

Here they are magnified:

http://www.cnccookbook.com/img/TurnersCubes/Jewelry/P1011928.JPG

Lots of ways to do better. It would've helped to use brand new inserts, run at 10 IPM, run flood coolant (this just had an air blast), and have a spindle that would run a little faster.

But, these guys are ready for the vibratory polisher and emerge from there with a mirror finish. There's a bit more machining to be done on them first, though.

Cheers,

BW