PDA

View Full Version : Really basic questions about sliding fits



jgourlay
08-23-2011, 11:35 AM
Gents,

I have some really basic questions about sliding fits and how to get them. And then an "application" question.

First, I note that the main QUALITATIVE difference between a class III and Class IV fit is that "Wobble or shake between mating parts noticed only on parts with short bearing length." (Class III).

How do we define "short bearing length"?

Second: when a drill bit drills an imperfect hole, how is this imperfection expressed? Let me detail the question this way, for a .375" hole. I can imagine that a drill bit could drill a perfectly round hole, but undersized. Or perfectly round, but over sized. Or "not round", with some parts of the hole touching the imaginary.375" circle, and no points of the real hole exceeding that .375" circle. Or I can imagine a "not round" hole with some points larger than the .375" perfect circle and some points not.

Third: what does the answer to 2 mean for process? For example, would I go into the metal with a standard 3/8" drill and then a .375" reamer. Or would I go in with a "U" size drill, and then a .375" reamer?'

Fourth: For my class III or IV fit, would go with .375" hole, then shoot for a .375" "cut", followed by scrubbing with 100grit? Assume that I don't have a tool post grinder, and that I'm not going to get one because of the number of people who have warned me never to toolpost grind on a lathe that I want to do accurate work on 10 years from now. Or, would I shoot for .376 and then work down to, say, 400 grit at .375" or .374"?

Now, the application question: for my application is Class III even needed?

Here is the application. I want to turn a pen such that there is no discernible transition between the wood body and metal fittings. "Discernible" means "the user can't feel any difference in the transition". Users in this case will be other "making stuff" folks, meaning they have intentionally practiced and *highly* developed sense of touch.

So, the key here is concentricity during the turning of the wood body. Concentricity of the fittings being a different topic. The body is made as follows: a brass tube roughly 2" long is glued into the wood. Into either side of the brass tube is slid a bushing. Depending on ID of the tube, this fit will be loose with some shake or VERY tight. Most are loose with no shake, to tight. I toss out the shaky ones.

This assembly is slid onto a steel rod, threaded at each end. On one end of the steel rod is threaded into a morse taper adapter that inserts into the lathe spindle. Onto the other end of the steel rod is threaded a brass nut meant to provide pressure between the morse adaptor and the bushing on the right side. This both provides drive friction and tensions the rod. The right end of the rod is indented for a live center in the tail stock. Because of the VERY high rpms, dead centers are not used and many penturners have had very bad experiences trying to use them.

What I found is this: a new steel rod usually lasts for a pen or 3 before cutting forces and who knows what else bananizes it, and I get a very hard to measure but nonetheless perceptible out of round "step" in assembly. SO, I'm making my own mandrel, but making it 3/8" rather than the typical 3/16.

I'll also have to make my own bushings, or drill/ream store bought ones. Thus the sliding fit question. Any thoughts then on fit and how it pertains to concentricity in this application? Picture below shows the setup.

[http://t0.gstatic.com/images?q=tbn:ANd9GcTyD6J8qUvkJAp2cX-pRS2qpQuqWY539MIlSGRM8XD8HvOdc05F]

philbur
08-23-2011, 12:04 PM
I think you need to tidy up your link, it doesn't work. I tried to guess the correct format but still doesn't work.

Phil:)

Evan
08-23-2011, 12:14 PM
How do we define "short bearing length"?

According to Professor Alexander Slocum of MIT anything less than "square" is short bearing length. That means the length is equal to the diameter. Square is the lowest that will prevent cocking and much more desirable is 1.5 to 2 times the diameter for a linear rod bearing.


when a drill bit drills an imperfect hole, how is this imperfection expressed?

An imperfectly sharpened 2 flute drill bit will usually drill a somewhat triangular hole. A three flute bit will drill a somewhat square(ish) hole.

The answer to 3 is Yes, use a reamer.

Using abrasive paper is not a good way to achieve a very close fit. It will inevitably cause a turned down edge. Lapping with a plug and grinding compound is much better. 100 grit is far too coarse. You should be able to obtain a very close fit with a good reamer.


Trying to mate a hard and soft surface perfectly with no ridge is difficult. A fingernail test can easily detect a ridge of much less than .001". The best way to do this is to make the soft part a little oversize and then work it down with fine abrasive paper mounted on a flat surface.

Scottike
08-23-2011, 01:12 PM
Machinery's Handbook specifies an RC class 3 fit to have a clearance of .005" min. .0015 max. for a nominal size range of .24 - .40".
RC class 4 clearance is .0005 - .002" for the same size.
You want to drill your hole undersized before reaming, how much depends on the material your cutting and the desired finished hole size.
Leave too much stock to ream can cause problems with chip removal, stuck reamers, and breakage.
Not enough stock left to ream causes excessive wear on the reamer and may not allow the reamer to fully cleanup (ream) the hole.
And of course, the speed, feed, and coolant (or lack of) will affect the finish.

jgourlay
08-23-2011, 04:06 PM
Evan/Scott: thanks.

So, some follow on questions. If I wanted to make the fit by working the shaft rather than the hole, is abrasive paper the best way to do that given the absence of a tool post grinder? Also, what is the role of SIZE versus SURFACE FINISH with regard to these fits?

Drill then Ream: so, I understand "undersized hole then ream". Does a .375" bit give an undersized hole? Or do I need to go to a "U" sized bit? "U" sized seems a LOT under (.007"), but is it really? I'm concerned, as you all pointed out, about a stuck/broken reamer. Note that these collars are going to be either 4340 or S7, although I'll harden after machining. If U size is too small, then what do people do? There is a 9.5mm bit (.374")--but that seems too large given Scott's "too little material" caveat. What do you advise?

In terms of the FINAL product, sanding the wood to the bushing works fine to create a zero-transition from the wood to the fitting IF the whole rod/bushing/body assembly is running true.

becksmachine
08-23-2011, 07:01 PM
Evan/Scott: thanks.


Drill then Ream: so, I understand "undersized hole then ream". Does a .375" bit give an undersized hole? Or do I need to go to a "U" sized bit? "U" sized seems a LOT under (.007"), but is it really? I'm concerned, as you all pointed out, about a stuck/broken reamer. Note that these collars are going to be either 4340 or S7, although I'll harden after machining. If U size is too small, then what do people do? There is a 9.5mm bit (.374")--but that seems too large given Scott's "too little material" caveat. What do you advise?


.007 would be a nice amount to take out with a reamer, however it would be a matter of the wildest conjecture that a drill that size would actually make a hole that size. Maybe some small amount of the hole surface area would end up close to the drill size, in between the gouges and annular rings the drill would make when a chip wedges itself between the drill bit and wall of the hole. And this assumes a perfectly centered/aligned center hole/spot drill to start, and a drill bit that is perfectly centered in that Jacobs chuck or whatever means is used to hold said drill bit. Let us also assume that the drill itself is somewhere close to the advertised size and that it has been sharpened with equal length lips and a center point that is actually in the center.

Maybe try a 64th or 32nd undersize and then run the "U" size drill through the hole before the reaming operation.

Dave

Scottike
08-23-2011, 07:07 PM
You could try the "U" sized bit, as long as the hole had a decent finish (well lubed and a new bit), and the reamer is able to fully cleanup the hole. But your doc would only be .0035 and that doesn't leave much room to clean things up with the reamer. I think I would go down a size smaller on the drill bit to 23/64, that would give you a doc of .0078.
Remember that your depth of cut with the reamer will only be 1/2 the difference between the rough hole size and the finish dia.
Your pieces don't sound like the hole is deep enough for chip buildup to be much of a problem even using the smaller drill bit.
In all cases use a good cutting oil liberally - I prefer a dark high sulfer oil, but any lubricant made for tapping would work and the dark sulfer oil can stain some materials.
Once the reamer enters the hole, don't stop feeding until the chamfer on the reamer exits the hole or is as deep as you need it to go, then try to pull the reamer out of the hole at about the same rate it went in at.
And never stop or reverse the rotation of the reamer while it's in the material, it'll damage the cutting edges.

As far as size vs finish, the finer and smoother the finish the the truer your sizes will be, the longer they'll stay that way, and the stronger your fits will be. (but the more difficult they are to achieve).
A rough(er) finish will have more voids in metal to metal contact and less bearing contact area. Picture a round wood rasp with a 1/2" od inserted into 1/2" id tube. Only the points of the rasp will be in contact with the wall of the tube. The actual amount of area in contact with with the tube is only a small fraction of the total available area. Metal finishes are exactly the same but on a much smaller scale. The better the finish, the finer the points of the rasp become and the more contact area you have to suppport a bearing, hold two pieces together, or slide along.
I always try to achieve the fit and finish I need or want while I'm turning the part to size but failing that, I prefer to use more something rigid than just abrasive paper or cloth, I find that just the paper wrapped around the workpiece can result in tapers, hollow spots, rounded edges and can be dangerous. If I do use paper or cloth I wrap it over the end of a piece wood or metal and use it like a file, less chance of fingers and hands interfering with the chuck rotation that way, and it gives me more control of the amount of material being removed and where it's removed.

edit: If your just using the paper to give your work it's final appearance, you might try using a lapping compound. Just lay something over the ways to guard against the grit, put some of the compound on a paint stir stick and work it back and forth over your workpiece.

RussZHC
08-23-2011, 07:35 PM
Take this for what it is worth as the precision you are talking about could be a bit out of my league.


I want to turn a pen such that there is no discernible transition between the wood body and metal fittings. "Discernible" means "the user can't feel any difference in the transition". Users in this case will be other "making stuff" folks, meaning they have intentionally practiced and *highly* developed sense of touch.


IF the real goal is the bold within the quote, I would suggest, if possible, reducing the number of "connections", each time something is fit to something else the error could become more, I am thinking, as example, the threaded rod to Morse taper to tailstock.

The info that jumps out at me is the bushings to rod and then rod being "clamped" to provide impetus to turn/spin...this clamping could impart all sorts of random/uncontrolled variances from where you start and certainly tough to duplicate from pen to pen (assuming you want to do this more than a single time...such as a test to prove a point, just saying).

Unless I am mistaken, and that is certainly possible, it sounds like an expanding mandrel would suit the process more BUT getting or making one that small could be tough [ditch the bushings and the rod, replace with expanding mandrel whose ends could spin on centers].

Not sure the rpm you are talking about (did I miss a given number?), but precise and fast is NOT cheap. Royal and Riten spring to mind as well as others. Royal, as example, makes centers .00005 TIR and 12 000 rpm. Now those are live/revolving centers, still...

As previously mentioned, the biggest issue IMO could be dissimilar materials, unless you have some way of the wood not moving at all over time.

Not to be flip but you could take the opposite approach and leave both wood and metal rough enough that discerning where one roughness started and the other ended became difficult...likely not a finish that would feel good to the touch.

firbikrhd1
08-23-2011, 08:36 PM
I have no real advice with regard to achieving your goal but rather wonder whether you might not be chasing your tail. Wood and metal being very different in their expansion/contraction rates, and wood being greatly affected by humidity whereas metal isn't so much affected, it might just be that achieving your desired fit isn't possible, or at the very least, temporary and unsustainable. Even wood of the same tree, laminated and sealed will eventually show some discernible difference at the joints.

Given the above, could you redesign your pen such that the transition points are intentionally different but still appealing to the touch and esthetically? While that might not be an appealing machining challenge for you it would certainly make production easier, faster and more forgiving.

If you must continue on your quest for your original goal perhaps using a hard wood and soft metal might allow you to achieve the desired affect, temporarily at least. Perhaps Lignum vitae and gold anodized aluminum or brass, for example. The Janka scale of hardness might be helpful in selecting a wood that would be suitable in comparison to the metal you are using.

http://en.wikipedia.org/wiki/Janka_hardness_test

If you could find a cross reference for hardness of materials between the Janka Scale and various metals your goal may be closer to being attainable. Even so, wood machines and works differently than metal so sanding the two to achieve a fit such as you describe likely wouldn't be possible.

huntinguy
08-23-2011, 11:53 PM
for the hole I would drill 11/32 then ream to U then let the part cool and ream to .375.

100 grit is too course for what you want. You need to be closer to 400 or 600. But doing what you are proposing freehand is going to be difficult. Heat will make the part measure larger than it will be when cool. Variation in who knows what will make the part wavy and keeping it straight will be a job. (I have done a few parts like you are proposing.)

As I understand it you are trying to make all the external parts of the pen fit without any transitional changes.

Why not just assemble the pen and then turn and polish the OD as one unit?

jgourlay
08-24-2011, 02:38 PM
Gents:

Thanks for all your great help so far!

A question/comment for those commenting only on the metal aspects:

I appreciate the value of achieving final surface finishing and dimensional compliance off the tool rather than with sandpaper. Question: on a small machine like what I have (1940's era Craftsman benchtop lathe), with the work I have (a 3/8" diameter 10" rod), how many thousands away from the final diameter do I STOP cutting with the sharp-edged rough tool, and start cutting with a rounder edge tool? And how many thou should I take off with each pass to get that shiny clean dimensionally correct result?

Also, what are your thoughts on feeding it first one with with the tool engaged, and then without adjust the feed at all, reversing everything. It's strange to me that I always get shavings (though very light and wispy) when I do this. But I do it because, well, it keeps taking off material (so it must be a good thing to do...). Other hints for best surface finish?

Wood/metal/transition:

First, let's establish that the desired transition is possible with a lot less ass-achery than I'm undertaking. But I'm undertaking it because I want a much beefier version of the standard set-up. Beefier so that it will last for more than 3 or 4 pens. Thus: the basic approach is sound.

Wood: you are dead right on harder woods. I work cocobolo, ebony, and the like. Hard to do this well with, say, soft spalted maple. Having said that, there are turners out there who do this on softer woods successfully. PART of the trick is to undersize a wee tad, then build up a cyanoacrylate thick film that can then be blended into the fitting diameter using 12000 grit sandpaper.

"disguising the transition": I have been thinking, hard, about this for years. The fundamental problem is twofold. First, whatever you do to disguise the transition has to be visually interesting. There are, broadly, two schools of "visually interesting". One is "high tech", the other is "hand made". The problem with both is the second leg of the fundamental issue: how you do something that is "handmade" without making look "homemade"? The difference between "handmade" and "homemade" is precision of fit. So, the standard approach is to make the most precise fit possible between to round things. The "disguise the transition" approach entails making a very precise fit between two "not-round" things. Precise fitting between round things is, as you can imagine, FAR easier than making a precise fit between two not round things. For example.... In one instance your task would be to make a perfect fit between a round brass rod inserted into a stainless tube. Then you want taper from the stainless tube into the brass, and polish. That would take you gents all of five minutes. A second example, respecting the requirement of visual interest, would be to inset a 6 pointed brass star into the end of a 6 pointed cocobolo hole. THAT is a nightmare. Now, you wouldn't need to have a perfect "feel" transition because the brass star could poke up. But any imperfection, no matter how tiny, between the star plug and star hole is going to scream like a banshee.

Doing the wood and metal at the same time: tried that. The problem is that a straight pen is a boring pen. At a minimum, you need a gentle curve. This gentle curve is achieved either hand tools or CNC. I don't have CNC. Hand tools, on the other hand, aren't going to cut stainless steel. Well, they might, but instead of a highly polished gentle curve, you'll get a big divot as it grabs the gouge and hurls it across the room. Damhikt!

firbikrhd1
08-24-2011, 08:40 PM
Unfortunately I haven't much more to offer to resolve your problem. The only thing I can come up with that may work for the final finishing of the transitional areas is the use of a "shear tool", or "shear bit". I have no idea whether it will work but it only takes .001" to .003" cuts and is used on materials that are usually difficult to obtain a good finish on. Here is a link to a site with further information.

http://www.gadgetbuilder.com/VerticalShearBit.html

If you choose to try this tool for your application I would be interested in the outcome. Good luck with the result!
Steve

Scottike
08-24-2011, 09:33 PM
Since I don't know all of the particulars of your setup and machine I just give you some general guidelines that work for me.
I usually stop roughing at 2 to 3 times my roughing doc from the finish dim and change to my finishing tool.
That next couple passes have a doc 1/2 my roughing doc.
The next 2 or 3 passes 1/2 doc of the previous pass.
The remaining passes I start reducing doc and aiming towards the finish diminsion. (In a perfect world, I reduce doc by 50% each pass until I hit the finish diminsion in about 2-3 passes with the doc I want to finish with)

elf
08-24-2011, 10:03 PM
Doing the wood and metal at the same time: tried that. The problem is that a straight pen is a boring pen. At a minimum, you need a gentle curve. This gentle curve is achieved either hand tools or CNC. I don't have CNC. Hand tools, on the other hand, aren't going to cut stainless steel. Well, they might, but instead of a highly polished gentle curve, you'll get a big divot as it grabs the gouge and hurls it across the room. Damhikt!

Perhaps a graver would give you the finish desired without sanding: http://www.sherline.com/gravers.htm

CNC and hand tools aren't the only way to cut complex shapes. A Rose engine would be an interesting way of creating unique pens: http://www.ornamentalturners.org/forum/viewtopic.php?t=7&sid=91f99fd5f6d28f2f67d5724948b70fa0

Paul Alciatore
08-25-2011, 12:47 AM
I think a re-design is in order. Instead of going for a precision fit in terms of a hole and a cylinder that fits that hole precisely, you could leave that fit loose and machine a pair of angles on the ends of the two external pieces. 45 degrees would be ideal with one facing in and the other facing out. These matching 45 degree tapers would be machined at the same setup as the external diameters so they are concentric with is. Now the two parts will self align. To prevent the sharp 45 degree edge from breaking down into a rough edge, put a 90 degree flat on it for the final ten thousanths or so and a matching 90 degree step on the mating part.

danlb
08-25-2011, 01:00 AM
Gents:

Doing the wood and metal at the same time: tried that. The problem is that a straight pen is a boring pen. At a minimum, you need a gentle curve. This gentle curve is achieved either hand tools or CNC. I don't have CNC. Hand tools, on the other hand, aren't going to cut stainless steel. Well, they might, but instead of a highly polished gentle curve, you'll get a big divot as it grabs the gouge and hurls it across the room. Damhikt!


The last one I did, I used hand held tools to shape most of it, but used a sharp HSS bit in the toolpost to do the area where the wood met the ferule. It worked out fairly well.

I almost forgot to say... Another trick is to deliberately put a 45 degree groove where they meet. Do it as part of a pattern and people ignore the fact that you have a seam there.


Dan

jgourlay
08-25-2011, 08:52 AM
Rose engine: now that is just cool!

oldtiffie
08-26-2011, 03:53 AM
"Sliding" fit (for metals etc.) is one of a range of classes of fits.

The Tolerance and Limits for each class of Fit over a comprehensive range of sizes is summarised for general/HSM use here:

http://i200.photobucket.com/albums/aa294/oldtiffie/Limits_and%20_Fits/Limits_and_Fits1.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/Limits_and%20_Fits/Limits_and_Fits2.jpg

Juergenwt
08-26-2011, 02:14 PM
Oldtiffie has it right. You can find all recommended fits in ISO 286/DIN 7157.
Many companies still use the old way of describing the way two parts fit together i.e. easy press fit, tight press fit, sliding fit, push fit etc. etc. Well, a push fit for an Italian may be different from that of a Japanese or a Russian or a Polish craftsman. You will not get very far with these descriptions if you do international business. Time to get the correct tables and use those standards.