PDA

View Full Version : How to improve turning accuracy?



form_change
07-20-2011, 05:40 PM
Most of the turning that I do is general purpose stuff (say +/- 4 thou) and has no need for great precision. However, lately I've been trying to turn shafts and bore holes to within a thou and am finding that a challenge. Typically I turn down to 5 or so thou over, measure with a micrometer, adjust and ... overshoot.

The cross slide has some backlash but as I'm not changing direction I wouldn't have thought that would have a great influence. The dial is graduated to 1 thou increments on diameter, so I'm thinking that I shouldn't need to be putting the compound on odd angles, and the lathe is a big solid thing (12x30), so flex while possible shouldn't be a major consideration. This happens with carbide as well as (freshly sharpened) HSS.

From those who regularly do this sort of thing, what are the rules/ tricks for this operation. Is it just practice? Should I be locking the cross slide once adjusted even if it is a light cut? Taking more than one spring cut before measuring? I could rough down closer to the desired dimension but suspect the radius on the cutter tip will start to come into play.

Michael

PixMan
07-20-2011, 05:57 PM
Always make sure backlash is out, and for a one-off part (as opposed to high-production) take TWO final cuts of the same depth-of-cut. Try to have your final cuts at least equal-to or greater-than any radius on the tip of the tool.

By taking two final cuts you can make the first cut, measure deviation from target size, then adjust the infeed for the second cut accordingly.

jdunmyer
07-20-2011, 06:05 PM
Michael,
You need to practice a bit more, and play with parameters: DOC and feed rate.

If you're turning something down, taking a .030" cut, measure it after every pass to see if it's actually being reduced by .060". When you change to a .005" DOC, the part will almost certainly be reduced by more than .010", due to the spring in your setup. Lighter DOC -> less spring -> more DOC than planned.

When you want to hit a given dimension, the best thing is to back off on your DOC well before the final pass. IE: go from a .030" cut to a .005", when still maybe .020" from final dimension.

If you change your feed rate, say to get a smoother final finish, you'll also tend to overshoot and make your part undersize. Same reason as above.

Again, experiment and you'll be able to do much better. That said, I'll sometimes take the last .001" off with a file. It doesn't take long, and you can hit the dimension right on the nose. Plus, if your lathe is cutting a slight taper, you can usually correct it at that time.

taydin
07-20-2011, 06:11 PM
I'm not in a position to give advice, but just wanted to share my experience while turning a shaft to be fitted into a bearing. I did a first pass, measured the diameter and then did a second pass. The result was 20.00mm, as measured with a micrometer. But when I tried the shaft after a half hour, it was loose. I didn't take into account the heat expansion, which made the part appear thicker than it really is.

rohart
07-20-2011, 06:16 PM
It's always worth remembering that when you measure the diameter, you measure the tops of the peaks of the rough turned surface.

If you're after .500 say, amd you measure .503 after a rough cut, the troughs are probably already below .499.

If I want to know how I'm going, I'll take a finish cut at .520 to see what it really is. Then I'll rely on the dial to get to within a gnat's, even going for another rough cut and a finish cut afterwards.

gwilson
07-20-2011, 06:19 PM
Yes,spring back and heat can hurt. Depending upon several factors,like how long is the work,is it supported at the tailstock, how sharp is the cutting tool,etc. can cause the metal to spring back. Generally speaking,if you take another pass at the same setting,you will see the cutting tool removing a bit more metal. On a close fit,heat will swell the diameter enough to mess up a fit when it cools.

Arcane
07-20-2011, 06:35 PM
The cross slide has some backlash but as I'm not changing direction I wouldn't have thought that would have a great influence. The dial is graduated to 1 thou increments on diameter, so I'm thinking that I shouldn't need to be putting the compound on odd angles, and the lathe is a big solid thing (12x30), so flex while possible shouldn't be a major consideration. This happens with carbide as well as (freshly sharpened) HSS.

You might be getting a little "sticktion" on your cross slide that shows up as non uniform advances as you wind it in in small increments. Setting the compound over to do the last few thousands greatly helps over come this. FYI, the angle that seems most preferred is 5.7391704 degrees. This gives a ratio of 10 to 1 which makes the distance conversion a simple matter of moving the decimal point one over, nice and simple and darn near fool proof.

macona
07-20-2011, 06:51 PM
Dont sneak up on a cut. Almost guaranteed to cut undersized.

Davidhcnc
07-20-2011, 06:55 PM
I would

1. take all cuts the same depth and feedrate...then load induced deflections are similar for each hit.

2. Aim for plus 2 thou.

3. Sort out the surface finish and size with a smooth diamond hone and/or smooth emery roll.

Black_Moons
07-20-2011, 07:04 PM
Thermal is a good point, Cutting heats up work, your final cuts should be done after it returns to room tempature, especialy if you have hoged off a lot (really heats the work)

Spring back is another good point, in the work (Causes taper) and the lathe itself (Causes overshoot)

What i'll usally do is take 2, 3, sometimes even 4 passes at the exact same depth setting, untill the tool isent even shaving off dust.

Then measure it, adjust the dials for the next pass, finish diamiter + 0.004" or so.
Do that pass 2 or 3 times, measure again, and do another 2 or 3 passes at the final setting of finish diamiter (Sometimes a half thou off the +0.004 it should be from the last pass)

Watch out for taper when measuring it. If its work spring, it will be smallest at the chuck (And tailstock support if used and properly aligned)

Taking the final 0.001" or so off with sandpaper/files is supriseingly accurate and easy. Just measure along and where its big you mark with a felt pen, then just file the marks off, repeat. the trick is getting a decent lathe file, idealy with safe edges, and puting it down on the work flat without the edges touching first and leaving scratchs. (I am tempted to grind the edges of my lathe file to make it smoother on the corners, but then I can't make square shoulders with it.. Need another lathe file I guess)

And yea, it will *remove* taper if care is taken. thats right, some poor sob with a micrometer and a file can be MORE accurate then your 1000lb+ $3000+ lathe, easily.

Just realise the poor sob with a file sure won't beat you on material removal rates! its all about using the right tool for the job/task at hand! And yes doubters (I used to be one!) a file is often the right tool!

lynnl
07-20-2011, 07:12 PM
Dont sneak up on a cut. Almost guaranteed to cut undersized.

I'm certainly not qualified to mentor on this issue, but that's been my experience too Macona.

I try to never find myself needing to take off less than 10-20 thou on the last pass. And as others have suggested, jot down the deviations from "dialed" cut increments for those last several preceding cuts, so I can sort of project how that final one is going to turn out.

Carld
07-20-2011, 08:15 PM
I am going to assume it's a worn lathe since you state there's slop in the cross slide.

When using a lathe with worn cross feed screw/nut you have to use a dial indicator on the cross feed. I use two mag bases. One with a dial indicator on it and another with a flat bar for the plunger to run against. That is the only way you will know how much your feeding into the work. You can't trust the dials on a worn or sloppy lathe.

Your just wasting time trying to use the dials on a worn lathe or any other machine that uses feed screws.

Sometimes you have to screw the compound all the way forward to remove any slop that can't be adjusted out.

I spent most my career in shops with worn out machines and had to learn how to make very accurate work using worn out machines and it wasn't easy.

I'll go set up what I used to do and post a photo.

Here's a photo of the setup I used. Of course I put the indicator on the right side when I was using it. The reason I put it on the left side here is because I didn't want to move the compound for the demonstration. You can use almost any mag base and indicator as long as you can put the plunger on a solid spot on the compound. The combinations are endless for sure.

http://i82.photobucket.com/albums/j276/yeathatshim/P7200001.jpg

Here's a photo of my collection of Mighty mag bases that I used a lot and sometimes needed several on a machine to do the job.

http://i82.photobucket.com/albums/j276/yeathatshim/P7200004.jpg

Scottike
07-20-2011, 08:30 PM
There could be several things happening that could cause that, are the gibs on your crossfeed and crosslide properly adjusted? Better too be a hair tight than too loose. The depth of cut on your finish pass should be influenced by the alloy your working, some finish well to light passes of a couple thou and others do better with a cut of 10 thou or more. The setup of your cutting tool can have an impact too. Especially if your tool is below center. And experence and practice is always a plus. When I first started, my mentor had me turn stepped rounds of varying diameters and step heights until I could get them to within +/- .0005 of the spec set for them. It was great for experence in turning to a shoulder and cutting to a dimension and can be used to get familar with how different materials behave.
Typically, for straight turning, I use my crosslide for setting the depth of cut for my roughing cuts and only use my compound for the finish pass-es. If I'm not sure how the material will finish I'll take some practice finish passes with the compound while I'm while I'm still roughing, that let's me play with the speeds and feeds and check how my depth of cut compares to what's actually happening. That way I know how to achieve the finish I need before I'm ready for the last couple of passes. My finishing speed is almost always faster than my roughing cuts. If I've been taking heavy roughing cuts on a piece, as I start getting close to my dimension I make a couple passes with lighter cuts before my finishing pass.
I always leave my compound angle set at 30 deg. for threading unless I have to change it to cut a specific angle and there's no other way to easily make that cut. If I'm not threading my compound is always set be at the end of it's travel towards my work minus 1 full turn. That leaves me enough travel for finishing and gives me the most rigid cutting platform. I have the gib on my compound set tight enough so that it takes more effort to turn than my crosslide and has a slightly stiff feel to a turn of the handle. I set my tool post up so that my tool holders (qctp) are parallel to the face of my chuck for turning and parallel to my work piece when boring. I set my tools into the holders at a slight angle - about 3 deg. - to give me a little extra clearance when coming up to a shoulder. Remember that with your compound set at 30 deg. a 10 thou indicated turn of the of the handle will be a cut of less than ten thou. For precision I'll setup a dial indicator to show me the exact depth of cut on the compound.
I have a 10x jewelers loupe that I use to examine the cutting edges of my HSS and carbide when I'm sharpening them. It will let you see defects in the edges that you might miss otherwise. Especially if your freshening up a tool you've already used or your like me and your eyes arn't what they used to be.
This is just my opinion and I'm sure others here their own way that's just as good or better, so I'll be following this thread along with you to see what I can learn.

Carld
07-20-2011, 08:45 PM
The problem with a worn lathe is the feed screw and nut on the cross feed and compound are not worn evenly the length of the screw. That makes you get different DOC with the dials.

You really can't trust the dials on worn lathes. You have to use a dial indicator to know exactly how much you moved the cross feed or compound.

On some lathes I had to use a dial indicator on the cross feed and the compound when cutting a thread because the dials would lie to me.

john b
07-20-2011, 08:55 PM
Just do like the Pix man say's. Keep it simple. john b.

vpt
07-20-2011, 09:00 PM
You have to learn your machine and what it does. Like mentioned when I start getting close to the number I am shooting for I take at least two spring cuts before moving anything.

KEJR
07-20-2011, 09:14 PM
I agree with Carld. Although I'm not an expert here by any means I've had the luxury of using pristine machines at work with DROs on them. With that setup you can see the DRO moving if your setup isn't right.

I quickly learned at home with the machines within my budget that I couldn't get away with the same kind of neglegence I had been using on well kept machines with DROs at work. As Carld says a cheap indicator can account for almost the same thing as the DRO if you are careful.

I'd do what others have said and make a couple finish passes at 0.020" over and make sure you are getting consistent finishes with the correct amount removed every time. Using your indicator here will help isolate if something is moving, the dial is off, or if your tool is not cutting properly. If this is all set get to within a few thou and start taking just a half thou or so off until you are at your final dimension. Once you learn your cutting tools and machine better you can refine this a bit more so you can cut out a step or two.

I'm contemplating making a crosslide lock for real precise work in conjunction with my indicator. If you indicate the thing in perfect and it moves while you are cutting you are kind of stuck in this scenario where you need to lock something.

I'm learning as I go and am just passing on my experience. Good luck.

KEJR

383 240z
07-20-2011, 10:03 PM
I have been following this thread with great intrest as I am trying to make a test stand for Rochester carbs. It is a 0.500" thick plate of 6061 AL. It has 4 pins going thru it that a 0.625" in diameter. They are going to be a press fit (they dont have to be I'm using it as a training exersize) they have a step turned on them that steps down to 0.3125". I have been toying with the idea of drilling a 0.500" hole and using my new boring head to take them to spec. then pressing the pins in. (also thinking about opening them to 0.600" and turning some 5/8" 6061 to 0.600" and pressing them in. Any way I was just out in the shop (dang its hot out there) and have been having trouble getting it to spec +/- 0.001"

What does DOC mean in this context?

Anythoughts on what I am doing right/wrong?? Also what is the correct interfernce for a press fit in this material? a 0.601" pin in a 0.600" hole??? Keith

justanengineer
07-20-2011, 10:13 PM
I think the best advice by far on here is Scottike's. The biggest problems I see whenever I see somebody inexperienced on a lathe are the basics. As already stated...

1. You cant be too rigid. Make sure the tool is as close to the tool post as humanly possible. Just an FYI, unless you have a Monarch or other HEAVY (not large) lathe, your average 1000 lb 12x36 is considered very flexible.

2. Lock every axis solid except for the one youre using for the same reason, to improve rigidity.

3. Make sure the gibs are adjusted properly. They should be adjusted so you can just begin to feel a slight drag when you spin the handle. This also improves rigidity.

4. Angle the compound and use it as a fine feed for finishing cuts.

5. Make sure youre using the correct speed and feed. If you cant produce a high quality finish, or if the tool is overheating/not heating enough then you should adjust accordingly. This is where I love mechanical variable speed adjustments and DROs for dialing in exactly the right speed.

6. Make sure your tool is sharp, ground properly, and stop to look at it every couple of passes. Ive seen too many people not pay attention and overfeed/lose the tip of the tool and not notice.

Just an opinion as well, so feel free to ignore, but I would put away the carbide until you have a bit more skill. Many view carbide as a replacement for HSS, which it definitely is not. There are many very good reasons why usually week 1 of many machine trades courses involves nothing but a grinder and HSS bit.

Keith - DOC = depth of cut or the amount of material taken off in a single pass. If you need to find info about press fits, refer to Machinery's Handbook. If you dont have a copy yet, its about the one required text to have on hand in the shop IMHO.

NzOldun
07-20-2011, 10:24 PM
Most of the turning that I do is general purpose stuff (say +/- 4 thou) and has no need for great precision. However, lately I've been trying to turn shafts and bore holes to within a thou and am finding that a challenge. Typically I turn down to 5 or so thou over, measure with a micrometer, adjust and ... overshoot.

The cross slide has some backlash but as I'm not changing direction I wouldn't have thought that would have a great influence. The dial is graduated to 1 thou increments on diameter, so I'm thinking that I shouldn't need to be putting the compound on odd angles, and the lathe is a big solid thing (12x30), so flex while possible shouldn't be a major consideration. This happens with carbide as well as (freshly sharpened) HSS.

From those who regularly do this sort of thing, what are the rules/ tricks for this operation. Is it just practice? Should I be locking the cross slide once adjusted even if it is a light cut? Taking more than one spring cut before measuring? I could rough down closer to the desired dimension but suspect the radius on the cutter tip will start to come into play.

Michael
Michael,

You will ALWAYS get some 'spring' in your system, particularly when using boring bars. When you have roughed down to within 0.010-0.005, back off you cutting tool slightly, start the lathe and then feed the tool slo-oowly back until it just touches. You can mark the area beforehand with a felt tip to show the touch, if you wish. Note the reading on the dial and proceed from there. Take about half of the remaining calculated depth on the first cut and then take a second cut without altering the tool. You may be surprised at how much the second cut takes off. Proceed in this manner until you reach your desired size. With GREAT care and using a little bit of polishing with emery cloth, you should be able to get within thou', assuming you have a 'tenths' micrometer. (only 'click' the micrometer three times, every time you use it!;)

NzOLdun

Carld
07-20-2011, 11:09 PM
DOC is how far the cutter is fed into the work. On some lathes if you turn the dial in .100" you will remove .200" off diameter and on some lathes if you feed the dial in .100" you will take .100" off the diameter. It depends on how the manufacture set up the dial.

If you use a dial indicator against the cross feed you will take off double what the indicator moves so be very careful when taking cuts.

I don't care how tight you make the gibs on the lathe cross feed and compound, if the screws and nuts are worn you will NOT get what you move the dial. It could be anywhere from a half a thousandth to .010" or more depending on the wear on the screws and nuts.

becksmachine
07-20-2011, 11:11 PM
I have been toying with the idea of drilling a 0.500" hole and using my new boring head to take them to spec. then pressing the pins in. (also thinking about opening them to 0.600" and turning some 5/8" 6061 to 0.600" and pressing them in. Any way I was just out in the shop (dang its hot out there) and have been having trouble getting it to spec +/- 0.001"

What does DOC mean in this context?

Anythoughts on what I am doing right/wrong?? Also what is the correct interfernce for a press fit in this material? a 0.601" pin in a 0.600" hole??? Keith

Thoughts on 2 points here;

#1, trying to press soft aluminum into soft aluminum is just begging for pain & heartache. Even a small amount of interference could easilly translate into galling and other bad words. ;)

#2, "DOC" translates to "depth of cut" or material removed on the radius, not diameter. A .050" DOC would reduce the diameter by .100".

Dave

form_change
07-20-2011, 11:12 PM
Thanks guys - there's some good stuff in there. I hadn't for example considered feedrate as having potential to change DOC but it is something to think about. I also bump up the speed and drop the DOC for finish cuts, so I'll have to consider that too.

These days I try to use HSS for fine work and save the carbide for less precise stuff, as it tends to push the work away rather than cut. I usually hone with a diamond stick every so often (not between critical cuts obviously). Having said that, I hit 0.500" spot on the other day with a carbide tool but with a high DOC and high speed - I was expecting it to end up 0.502 or something. Sometimes moving that QCTP lever a 1/6th of a turn is just too much effort...

I think I can rule out lathe rigidity as a major contributor. It's a 12x30 lathe but weighs in at around 1500kg (3300lb). My gibs are adjusted so that a slight but definite effort is required to turn the handles. A machine handle that can 'spin' is an invitation for something to change.

Michael

EVguru
07-21-2011, 05:21 AM
You might like to consider a skiving tool;

http://www.productionmachining.com/articles/the-forgotten-art-of-skiving

.RC.
07-21-2011, 05:55 AM
Using a DRO makes the job much easier or other direct measuring device..

Are you using carbide or HSS?

form_change
07-21-2011, 06:53 AM
I use both RC - usually I use carbide for bulk material removal and HHS for lighter cuts. Typically for a shaft with a shoulder on it I'll use HSS as I can get a sharp corner. Boring I usually use one of two carbide (insert) boring bars I have.

The DRO plan is nice, but there are two issues I need to sort out first. One is finding the money but the second is fitting it to the lathe. Along the bed is fine, but fitting to the cross slide is not straight forward. One of the things I want to do when I have the time is make up a dummy scale and try it for position so that I can check it won't be mashing the scale with the tail stock or interfering with the taper turning attachment

Michael

airsmith282
07-21-2011, 08:08 AM
Most of the turning that I do is general purpose stuff (say +/- 4 thou) and has no need for great precision. However, lately I've been trying to turn shafts and bore holes to within a thou and am finding that a challenge. Typically I turn down to 5 or so thou over, measure with a micrometer, adjust and ... overshoot.

The cross slide has some backlash but as I'm not changing direction I wouldn't have thought that would have a great influence. The dial is graduated to 1 thou increments on diameter, so I'm thinking that I shouldn't need to be putting the compound on odd angles, and the lathe is a big solid thing (12x30), so flex while possible shouldn't be a major consideration. This happens with carbide as well as (freshly sharpened) HSS.

From those who regularly do this sort of thing, what are the rules/ tricks for this operation. Is it just practice? Should I be locking the cross slide once adjusted even if it is a light cut? Taking more than one spring cut before measuring? I could rough down closer to the desired dimension but suspect the radius on the cutter tip will start to come into play.

Michael

you should always lock the compound slide when doing any turning operations this will help prevent taper turnning alot, and help make better cuts either way,the dials on these lathes are pretty much a joke there not as accurate as you might think you have to compensat for the stuff.

but once you know where 1 thou is or 5 thou really is then its a snap,
taking lighter cuts also improves accuracy and alot it will reduce tool flex prolong the life of your cutters and increase the life of your machine and the bearings alot..

if your turnning ss or other steels try and keep it in the 300 rpm range with HSS cutters and 500 to 550 with carbid unless your set up for coolent in which case the carbide can be turrned higher then 500 at that point and hss cutters can hit the 500's with ease..

luthor
07-21-2011, 09:23 AM
if your turnning ss or other steels try and keep it in the 300 rpm range with HSS cutters and 500 to 550 with carbid unless your set up for coolent in which case the carbide can be turrned higher then 500 at that point and hss cutters can hit the 500's with ease..


Airsmith, have you ever heard about Surface Speed, your statement above is misleading and totally incorrect.

GadgetBuilder
07-21-2011, 10:37 AM
My approach is to ensure the slides aren't too tight, they need to move smoothly without slop but must be loose enough that they don't stick and then jump. A worn leadscrew doesn't have much effect when the movement I'm after is only a thou or two - wear doesn't have much effect on small incremental moves so the dial is close enough.

I've found that normal lathe bits don't cut predictably on shallow cuts of 5 thou or less. When target diameter and/or finish is critical I use a vertical shear bit:
http://www.gadgetbuilder.com/VerticalShearBit.html

This bit can't cut more than about 3 thou but it leaves a good finish and allows sneaking up on the target diameter with small cuts. Still needs spring cuts. And movement of the cross slide must be predictable (no stiction).

Once I get within 2-3 thou of the desired diameter I use a shop made lap. These are easy to make for modest diameters. My lap holder is steel and the laps are slices of 1.25" aluminum bored to size and slit to allow adjustment.

Laps work fairly rapidly when reducing the OD by 2 thou or less because mostly they're taking the tops off the machining marks. I use 300 grit aluminum oxide but valve grinding compound (silicon carbide) will work too. I prefer alox because it breaks down more rapidly.

One nice thing about laps is that they make the shaft more round - turned items aren't often perfectly round. Also, diameter of turned shafts can vary a tenth or two over the length and you can feel this and concentrate on the larger diameter areas. If you don't refresh the lapping compound it breaks down in the process and the finish gets finer and finer. Finally, lapping is slow compared to turning so it is fairly easy to work to a tenth.

Note that laps slow way down when all the machining marks are gone so it pays to turn as close as possible to final diameter.

My shop made lap holder and two laps, nothing fancy but it works well:
http://img507.imageshack.us/img507/9823/shopmadelaps.th.jpg (http://imageshack.us/photo/my-images/507/shopmadelaps.jpg/)
The setscrew keeps the lap from spinning in the holder and allows adjusting the size as you go along.

Bottom line is it takes me a lot longer when I'm fussy about getting the size exact.

John

brian Rupnow
07-21-2011, 10:37 AM
Something that I have noticed with turning, is how much the sharpness of the cutting tool plays into final cuts. I have seen situations where I "sneak up" on a final diameter, and get to within.004" of final finished size. I advance the cutting tool 1 "marked increment" on the crossfeed dial, (which amounts to .002" on the diameter) and take a pass---and the tool doesn't remove any material!!! So---I advance the tool one more increment---take a pass, --and it still doesn't seem to remove very much material. Okay, damn it, the piece is still oversize---so I advance the crossfeed 1 MORE increment.---and then the friggiin' tool digs in and takes of .006", leaving the part undersized. This happens more than I really want to admit. I must remember to keep the cutting tool sharper, for final turning!!!----Brian

steverice
07-21-2011, 01:56 PM
Take the time to get acquainted with how the machine cuts, take your measurements the same every time and always keep it loaded against the backlash and use an indicator if necessary, but the dial should be good after you get comfortable with its readings.

Horst
07-21-2011, 02:43 PM
Use the 1/3 cut method. When you get to within say 0.060 of the target dial in 1/3 (.020). Then mike and divide by two (say after the first pass you miked .041, then you dial in .0205). make second pass. Mike again and remove final amount. This works for boring as well. Usually hit nuts on. If on a production run make a note if dial readings. Should be repeatable.

Tony Pratt
07-21-2011, 02:53 PM
Something that I have noticed with turning, is how much the sharpness of the cutting tool plays into final cuts. I have seen situations where I "sneak up" on a final diameter, and get to within.004" of final finished size. I advance the cutting tool 1 "marked increment" on the crossfeed dial, (which amounts to .002" on the diameter) and take a pass---and the tool doesn't remove any material!!! So---I advance the tool one more increment---take a pass, --and it still doesn't seem to remove very much material. Okay, damn it, the piece is still oversize---so I advance the crossfeed 1 MORE increment.---and then the friggiin' tool digs in and takes of .006", leaving the part undersized. This happens more than I really want to admit. I must remember to keep the cutting tool sharper, for final turning!!!----Brian
Use two tools, keep one for roughing and one to say take the last 10/20 thou off. The finishing knife tool needs to be nice and sharp with a small radius stoned on the leading corner. This business of the lathe not taking a .001" cut is badly adjusted slides,a blunt tool or both.
Tony

RussZHC
07-21-2011, 05:42 PM
Don't think this is a "hijacking"...at what point in the series of events does one re-sharpen/touch up a ground bit?
As already posted, just use judgment as to what the edge of the tool should look like (or what it looked like "new") and what it looks like "now"?

Logically there must be some wear happening each pass or for that matter each turn.
Is a change in the chip (shape, color) viable? Or does that have too many variables involved?
Can one get clues by how the machine or cutting action changes sound? Or is that more a function of DOC as opposed to the tool edge being the way it should be?

EVguru
07-21-2011, 05:55 PM
I usually give the tool a stroke with a diamond lap after every couple of roughing passes and certainly before a finishing pass. Unless I have a tool crash, or hit a weld, or try to mahine some exotic 'mystery metal' I almost never have to regrind my tools.

Carld
07-21-2011, 08:24 PM
Quote from Brian, "Okay, damn it, the piece is still oversize---so I advance the crossfeed 1 MORE increment.---and then the friggiin' tool digs in and takes of .006", leaving the part undersized."

When that happens it's a sign the crossfeed screw has worn spots and is not moving the crossfeed when the handwheel it turned. The only way to know what the crossfeed is moving is to use a dial indicator or a DRO on it if it has a worn screw. It could also be that the gib is too tight.

EVguru, if you look at the top surface of your cutter with a high power magnifier you will see the top is worn down even after you have dressed the side to sharpen the edge. The cutting pressure wears the top off the cutter more than on the side because the metal is rubbing across the top of the cutter not on the side of the cutter. To keep the cutter sharp you have to grind the side far enough to remove the rolled edge on the top of the cutter. It won't show as easily on carbide as it will on HSS but it's there.

If you really want a fine machined surface with a constant diameter then use a shear cutting tool. You can take less than .0005" with it and the compound set at the correct angle to take .0005" per .001" of feed.

Black_Moons
07-21-2011, 08:34 PM
When to sharpen tools.. Well, You'll want to sharpen them at least 2 passes before the final pass if its super critical (or swap tools) because you need to leave enough metal to dial the tool in and figure out its 'length', then make your finishing cut.

As for when to sharpen them... I find surface finish a good indication of when to sharpen a finishing tool. Though you might wanna sharpen it every now and then or before any critical jobs even if the finish is still good. Only takes a few seconds to hone it if its still very sharp, It takes minutes to hours if you dull it badly (or regrinding) or chip it.

Also, Once it gets dull, it dulls badly even faster due to the massive incress in force needed to cut. You do NOT save time by sharpening less often, You waste a lot more time by spending that much longer to resharpen it, and having to remove that much more material. Sharpen often enough to keep it sharp. More often is wasted, Less often makes sharpening take excessively longer.

For roughing... Hmmm. I guess I would do that opticaly, with a jewlers lupe (Look for the specular reflection off the edge, If wide and visable under diffrent viewing angles, its dull), or just after X inchs of metal turned. I often use carbide to rough, And the same tool to finish with if its not critical I get a good finish. (though I often do get a great finish with normal carbide in aluminum. Steel I never get a good finish so why bother trying unless its critical, then use emery paper anyway. Again, I Usally will change inserts when I find it gives a poor finish in aluminum and/or it looks dull with my lupe)

Woods and plastics love my HSS custom grinds however for a good finish.

If you find its not cutting when you advance it 0.001" (not taking off dust), thats a good sign its dull.

When using carbide and roughing, beware you might not notice the tip cracking off, because even a jaggid peice of carbide will cut if pushed hard enough. I learned the hard way: if you start seeing sparks, Its probley something horrabley wrong :) (Unless its a weird alloy or super high SFM with CBN or some other exotic cutting tool)

Amount of force you need while turning is a good indication of sharpness too, Or if its well above center (rubbing on the relief) You'll quickly notice by how hard it is to cut with, Or how it cuts only once the pressure is very high and then stops cutting. (Also can be caused by very springy work however)

brian Rupnow
07-21-2011, 08:35 PM
Quote from Brian, "Okay, damn it, the piece is still oversize---so I advance the crossfeed 1 MORE increment.---and then the friggiin' tool digs in and takes of .006", leaving the part undersized."

When that happens it's a sign the crossfeed screw has worn spots and is not moving the crossfeed when the handwheel it turned. The only way to know what the crossfeed is moving is to use a dial indicator or a DRO on it if it has a worn screw.

One of the things I have learned over the last 3 years, is to NOT measure the piece being turned with a Vernier caliper. When I get down into the "close" range, I use a micrometer. I know that in theory, each "increment" on my crossfeed dial will take .002" off of the diameter. Sadly, theory and practice don't always play by the same rules when I am machining a part.:eek: :eek:

383 240z
07-21-2011, 08:45 PM
Quote:




Originally Posted by 383 240z

I have been toying with the idea of drilling a 0.500" hole and using my new boring head to take them to spec. then pressing the pins in. (also thinking about opening them to 0.600" and turning some 5/8" 6061 to 0.600" and pressing them in. Any way I was just out in the shop (dang its hot out there) and have been having trouble getting it to spec +/- 0.001"

What does DOC mean in this context?

Anythoughts on what I am doing right/wrong?? Also what is the correct interfernce for a press fit in this material? a 0.601" pin in a 0.600" hole??? Keith


Thoughts on 2 points here;

#1, trying to press soft aluminum into soft aluminum is just begging for pain & heartache. Even a small amount of interference could easilly translate into galling and other bad words.

#2, "DOC" translates to "depth of cut" or material removed on the radius, not diameter. A .050" DOC would reduce the diameter by .100".

Dave

Dave not really worrying about galling, in fact it will tend to help me, as once the locating pins are in place they will stay there.

Carld. I feel your pain that was my problem last night, then I start second guessing myself (was I at .020" or at 0.025"??) I then was resetting my dial indicator to 0.000" after every cut. I also was making the mistake of using a vernier caliper to measure, I was having better luck with my micrometer this morning.

An a related note, If I post some pics of my lathe, could somebody show me where my gib adjustment screws are?? and maybe tell me how to adjust them? They are where they were when I drug this machine home. Keith

darryl
07-21-2011, 08:51 PM
Lots of good advice so far. You really need to 'characterize' your lathe and cutting tools. Find out what happens to the position of the tool as you go through the routines of dialing in, moving the carriage back and forth, moving the crosslide and compound back and forth. You need to know every area where you must account for unwanted movement. If you miss something, there will always be a mystery.

Sometimes there will be flex where the tool would either be drawn into the workpiece, or pushed away from it, and this is different than having play in the various slides. Much of this has to do with the tool, the angles ground on it, the type of material you're working with, and the sharpness. Some of it has to do with the toolpost flexing, and this could be because of an imperfect fit, a poor clamping bolt, debris, or simply a crappy toolpost. If it can rock at all on the compound, nothing lower down will fix that.

As others have said, you must account for play in the slides, and you need to know if the slides move without you dialing. What can happen is you make a cut, then make a spring pass. It should cut again, slightly, then settle down. A third spring pass should not remove any material to speak of. But, let's say this seems to work as it should- now make another test cut, then a spring pass, then wait a few minutes before making the last spring pass. You might find that now that last spring pass takes off more material- even though you did nothing different, the tool has advanced a tad further into the workpiece. This would be from the slides 'relaxing' a bit when given a few moments or minutes without the back pressure from the cutting action.

Think about the procedure you use to account for the total of the plays, and how consistently you apply that procedure. If you do something differently during your test cuts, then you should expect that there could be an effect from that.

Someone mentioned about the freshly machined surface having high spots. You need to know how high to leave them so when you have done what you might have in the way of smoothing the final result from the turning operation, you'll know on a fairly consistent basis how much your 'cleanup' is narrowing the workpiece. I like to use a file to knock off high spots, and there is certainly a technique to being consistent with that. You should probably not put more than a few seconds of filing on the machined surface, otherwise you could taper it or make hollow spots, etc. One thing I sometimes do is file right after turning, then reverse the spindle and the file and touch down again for a couple seconds, then maybe a second or so in the forward direction again. Most of the micro slivers that would give an indicator a false reading of the actual diameter would be removed by this process.

Using the 1/3 method that Horst brought up, you can integrate the filing procedure with it.

The worst thing that you can find now is that if you have accommodated all the sources of errors, the result could still be inconsistent. You might have to start looking at the spindle bearings, or variations in the positional accuracy of the chuck as mounted on the spindle. You might spend considerable time characterizing your machine in these ways, but the end result should be that you can fairly consistently turn to within a thou or less when you need to.

383 240z
07-21-2011, 08:55 PM
Again pardon my ignorance, but what is a spring cut? Keith

form_change
07-21-2011, 09:09 PM
It's when you do another pass (or several) without changing the tool position, on the basis that the cut you've just made (as you haven't got absolute rigidity) has 'sprung' away from the work, leaving it slightly over size (undersize when boring), even if the dial says it's right. Especially important when boring as boring bars will deflect much more than other tools.

Michael

KEJR
07-21-2011, 09:20 PM
This is mostly on topic, so I hope I'm not getting off track:

Last couple of projects I've been using a conventional right hand HSS tool bit with a real sharp and pointy tip on it to finish a diameter and then take a finish pass on a shoulder in the same setup. I do get some fine lines in steel even though my tool is pretty sharp. Some classic books I've read show big honking radii on the cutting tool for finishing. Obviously you can't have a big radius on the tool if you turn and face a shoulder and want a decently sharp corner on the part.

Should one compromise and just slightly round the tool tip, or are these old books overstating it?

KEJR

Toolguy
07-21-2011, 09:31 PM
Slightly rounding the tip will usually help the surface finish. I use a diamond file for HSS and carbide. It only takes a minute or less.

airsmith282
07-21-2011, 09:35 PM
Airsmith, have you ever heard about Surface Speed, your statement above is misleading and totally incorrect.

iam sorry its not my fault you cant understand me i laid out the post rather clear and very accurate,, and its in no way misleading ,..

Black_Moons
07-21-2011, 09:37 PM
This is mostly on topic, so I hope I'm not getting off track:

Last couple of projects I've been using a conventional right hand HSS tool bit with a real sharp and pointy tip on it to finish a diameter and then take a finish pass on a shoulder in the same setup. I do get some fine lines in steel even though my tool is pretty sharp. Some classic books I've read show big honking radii on the cutting tool for finishing. Obviously you can't have a big radius on the tool if you turn and face a shoulder and want a decently sharp corner on the part.

Should one compromise and just slightly round the tool tip, or are these old books overstating it?

KEJR

You can kinda cheat. First off, you could swap tools to make the inside corner sharp.

And, you can cheat while grinding your tool, while its true a huge radius can produce a better finish (till it chatters..), realise that only the very tip of the tool is in contact, So you really only need a very small section of the huge radius.

Think of huge nose radius, as in the entire tool is a 180 degree ball
Now chop it in half, except the half left is a little more then half.
That tool can get very close to shoulders and still have a huge nose radius. (Would be 91 degrees of radius)

Even that, you don't have to grind the whole 91, you really only need a couple degrees of radius, its just important that where the tool enters and leaves the work is radiused.

That said, Note that rounded 'fillets' on shoulders are MUCH stronger then sharp corners, and the more rounded the stronger it is (Stress raiser, etc)

Carld
07-22-2011, 12:01 AM
What airsmith posted for speeds will work. In fact it's best to use what gives the best finish and it may not always be what is in the chart. A surface speed chart is only guide line. I seldom use what is on a surface speed chart because I experiment with it and in fact I don't even use one anymore. I machine by the seat of the pants method.

There's a lot that affects the surface speed and a few are, type of material, shape of the cutter, HSS or carbide, type of carbide, size and rigidity of the lathe, rigidity of the cutter, holder and tool post and the feed rate. You can't just look at a chart and use what is there as gospel because what works one time may not work the next.

Machining is not a science, it's a skill and there are few constants and many variables.

When your roughing it down to size the cutter doesn't have to be sharp but when your taking finish cuts it better be as sharp as you can get it and keep it sharp. If the finish cutter is dull it will push off the work. For finish cuts it's best to have a radius on the nose. The radius has to be more than the feed rate of the cutter so it will not leave a thread like finish on the work and a shear cutting tool leaves the best finish of all.

darryl
07-22-2011, 12:02 AM
I use HSS a lot. I grind to a sharp corner, making sure I have front relief and side relief. Then I hold the face of a diamond stick against the side relief and round over the nose, keeping the stick in contact with the front and side surfaces. That makes the diamond touch up the edges without changing the relief angle. It works because the grind leaves a bit of a hollow, and the diamond doesn't have to remove much material to sizzle up the cutting edges. The round over probably has a radius of about 10 thou on an average- I just go with what works for me. Where I want to leave a larger transition in a corner for strength, I'll make the radius larger.

Setting the cutting edge nearly parallel to the workpiece often leads to a situation where you can remove material with the nose mostly, then reverse the feed for a clean-up pass.

Carld
07-22-2011, 12:07 AM
For finishing a shaft with a shoulder use a 60 deg cutter with a radius on the nose and set the cutter at about 45 deg to the shaft. Then take .010" or less cuts on the shaft and shoulder until finished to size. It works every time.

EVguru
07-22-2011, 05:04 AM
EVguru, if you look at the top surface of your cutter with a high power magnifier you will see the top is worn down even after you have dressed the side to sharpen the edge.

Which is why it's usually the top edge that I do first. I then give all the angles a stroke with the diamond lap. It only takes seconds.

luthor
07-22-2011, 05:59 AM
It is obvious that some people on here do not understand the concept of surface speed, a 1/4'' diameter shaft at 500 rpm has a surface speed of 392.7 inches per minute, a 2.0" diameter shaft at the same rpm has a surface speed of 3141.6 ipm, nothing to do with a chart just simple maths.

383 240z
07-22-2011, 06:29 AM
Luthor. Instead of condeming those who do not understand the concept, why don't you enlighten us neandertals by posting the fourmula? And if I understand your post correctly, if there are only 2 variables (diameter and rpm) a chart could be made very simply. RPM on one scale, diameter on complementary scale and conclusion where they cross. Keith

willmac
07-22-2011, 07:00 AM
Surface speed does depend on diameter and rpm. That is why it it is inappropriate to quote a rpm figure without reference to diameter. However the most useful question is 'What is a reasonable rpm to choose for this cut?'. That depends on more than the diameter; other factors are critical including:
Tool type and material (i.e. HSS, carbide, coatings etc)
Tool design (i.e. tip shape etc - chip breaking capability)
How long you want your tools to hold their edge.
Work material (i.e Aluminium, Brass, Leaded Steel, Cast Iron, Stainless Steel require vastly different surface speeds)
Machine capability (What rpm and feeds can your lathe deliver)
Work shape and holding (out of balance faceplate work needs vastly different speeds to collet held bar stock)

Carld
07-22-2011, 09:21 AM
For surface speed charts or formulas all you have to do is google for them. As willmac said, the diameter and rpm are part of it and then the feed rate and DOC. When you start doing lathe work it may be confusing but after you have turned a lot of metal you get a feel for how fast, deep and feed you want for different materials. There's really no need to refer to a chart after some experience turning.

If your turning a large diameter to a small diameter you will have to change rpm at some point to keep things right. That is, large diameter, lower rpm, smaller diameter higher rpm. Once you have figured out what works best with your lathe and tooling it's easy to just use your experience of past work to get a starting point.

On the other hand, many love to read charts and do math so they prefer doing it that way for each job. Manual lathes are much more forgiving than CNC in that with CNC your trying to get the most optimal performance from machine and tooling within a certain time frame. With a manual lathe your mostly concerned with just getting the job done the way you want it.

It's as I said in an earlier post and willmac said above, there are a lot of variables to consider along with rpm, diameter, feed, cutter and material among other things.

It's not a science, it's a learned skill.

vpt
07-22-2011, 09:35 AM
I was trying out different grinds and angles for different finish results last year.

A 45 degree knife edge gave me the best finish.

http://img197.imageshack.us/img197/3491/lathewood024.jpg

Carld
07-22-2011, 09:48 AM
That cutter is what is called a shear cutter.

KEJR
07-22-2011, 09:55 PM
Slightly rounding the tip will usually help the surface finish. I use a diamond file for HSS and carbide. It only takes a minute or less.

Thanks toolguy. I'm also finding those diamond files pretty handy, althought I just bought some fine stones to hone HSS cutters. I did some practice tonight with a slightly rounded HSS cutter honed smooth with a stone and it gave me the best finish so far even on C1018 which I find always wants to leave gummy lines on my work. I think I am at the point now with these tools that I get accurate removal and good looks, but a touch of oily 600 grit will polish it up even more.

Thanks,
KEJR

loose nut
07-23-2011, 10:45 AM
Luthor. Instead of condeming those who do not understand the concept, why don't you enlighten us neandertals by posting the fourmula? And if I understand your post correctly, if there are only 2 variables (diameter and rpm) a chart could be made very simply. RPM on one scale, diameter on complementary scale and conclusion where they cross. Keith

RPM's = (SFM X 4) / DIA.

That's the basic formula reduced down to its simplest form for HSS tooling, carbide (or other type of inserts) will be increased by a factor or two or more depending on the type of carbide and the type of lathe you are using. It is intended for production turning were time is money and you aren't paying for the insert's so it is a really good idea to use the bottom end SFM range in the formula to reduce the RPM's somewhat on a smaller less ridged machine. This doesn't take DOC into account, I was taught .050"/HP but again that depends on the power and rigidity of your equipment. Use it as a starting point until you get the feel for your lathe.

On a drill press I usually divide the the result in half and use a little more pressure to get a higher chip load. The tool stays cooler (not smok'in and burned to a crisp) and the job still gets done about as fast.

form_change
07-23-2011, 06:14 PM
The metric version I use is RPM= (surface speed x 30)/diameter,
where surface speed is in metres and diameter is in mm.
Usually I simplify in use by saying RPM=9000/diameter - this is for normal steel & HSS and then multiply/ divide by factors for different materials (tool or work such as 3x for Aluminium, 1/2 for cast iron, 3x if using carbide and so on.)

Michael