PDA

View Full Version : Question regarding use of rotary table on mill---



brian Rupnow
06-28-2008, 10:08 PM
http://i307.photobucket.com/albums/nn294/BrianRupnow/part1.jpgGentlemen--I spent the day milling out a main frame for a new model steam engine project, and it was a great success.--That is to say, I didn't cut off any fingers and didn't ruin the part!!! I started with a peice of 1" x 3.5" aluminum flatbar and actually ended up with a pretty swoopy looking part. Now my question---I want to mill a radius on one end. I do have a 1/2" diameter hole in the part I want to mill at what will be the center of the radius. My rotary table (which I have never used yet) has 3 T-slots on the top rotating part, and a hole for an MT2 tapered collet or spindle. My plan is to turn a peice of aluminum which will locate in the MT2 tapered hole inthe center---(not a tapered part, just a round one---I'm going for a locating device, thats all), and has a turned diameter extending above the top of the rotaty faceplate which will locate in the 1/2" hole in my part. I will attach the part to the T-slots in the top of the rotary table using T-bolts. I will attach the rotary table to the bed of my mill using the T-slots in the base of the rotary table.- I will locate the rotary table and part in a relationship to a 4 flute end mill, so that the side of the end mill is tangent to the side of the part to be milled. --Jeez, I hope this is making sense--Then, I should be able to turn the round handle on the side of the rotary table to make the top of the rotary table rotate through a 180 degree arc, thus cutting an arc around the end of the part, using the center of my 1/2" hole in the part as my centerpoint of radius. (the part I an cutting is 1/2" thick aluminum.) Do you understand me??? Am I going about this in the correct way???---Brian

RobbieKnobbie
06-28-2008, 10:52 PM
hmm, I think I followed you through that.

It sounds like you're on track... but one thing you'll want to do is start a little past tangent... maybe .020 off the part. Then mill through in a couple passes (how thick is the part?). You can then move in and clean up that last .02 in one pass.

You didn't say if you have the part directly on the rotary table... you might want to sandwich a sacraficial bit of aluminum or something under the part so you don't foul the face of your brand new rotab. You could also use a thin parallel or something and make sure the parallel isn't in the path of the cutter.

Rich Carlstedt
06-28-2008, 10:52 PM
Brian
You got it !
The only commentary I have is to start with the spindle and the rotary table centered together.
The easy way to do that is if you have say a 1/2 dowel or pin in the center of the rotary table, and to raise the table up to a 1/2 collet in the spindle.
snug the collet lightly, and then lock your rotary table down.
That puts the two centerlines together without any error, then loosen the collet, and lower the table.
Robbie's suggestion is a good one.
I keep a supply of plastic sheet (.090) that the local lumber yard sells for storm windows.
The plastic is great, and when boring through a part, the plastic chips are easy to see...which means stop

Rich

Your Old Dog
06-28-2008, 11:28 PM
My neighbor made me a taper to fit my rotab and I bored it out to 1/2". Now I can make slugs of various sizes to fit into the bored out taper tool he made me. It's probably a mousey way of doing it but it works fine for me and I know I'm on radius.

Mcruff
06-28-2008, 11:45 PM
The easiest way to align the center of the rotary table to the spindle is to use a mag base on the rotary table with an indicator. Basically you crank the indicator needle around the spindle.
What every shop I have ever worked in did for the rotary table was to put a set of dowell pins (usually .250) at a known location off the center of the table in both the X and Y directions, that way you have something that you can align parts with at a known distance from center using cheap gage blocks or adjustable parallels

oldtiffie
06-29-2008, 01:44 AM
There are two, possibly three questions to be asked here?

1. Do I want to use the rotary table? If yes, go no further;
2. Do I have to? If yes - again go no further; and
3. If the answer to 2 is No, then proceed.

A warning and a caveat.

When cutting have your "X", "Y" and "Z" feeds and your quill locked or clamped. Make sure your draw-bar and collets are firmly tightened.

If you feel ill-at-ease with the following either take it very cautiously or just don't use it.

Mark it out and cut the bulk of waste off with a band-saw or hack-saw.

Use light cuts - 5 to 10 thou each time will do.

Use a "small-ish" cutter (say 1/4" to 3/8").

DO NOT CLIMB MILL else it may "grab" and get the better of you. Conventional milling should be OK.
(I'd "climb" it but that's me).

Use "stops" fastened to the mill table or fixture.

Drill/bore the 1/2" hole first - before you cut it to length - or keep a 12" to 18" "lever arm" ("handle"?) for milling and then cut the job to length after the milling/radiussing is completed.

I use variations of the following methods.

1. By Marv Klotz - one of if not the most inventive and innovative members of this forum.

Note the use of stops and a "burr" cutter (aka "rotary file") instead of a milling cutter

http://i200.photobucket.com/albums/aa294/oldtiffie/M_K1.jpg

In use, the fixture is clamped in the mill vise. A rotary file, held in a collet, is lowered into the slot seen in the other pictures. The y-axis is used to advance the work into the spinning file a few thou at a time. After each advance the work is swung back and forth between the stops to remove material.

If you make one of these, exercise care in its use. Your hands will be close to the spinning collet and rotary file. For extremely small pieces, I solder the part to a larger piece of metal to use as a handle or else use a small hand vise to grip the workpiece.

http://i200.photobucket.com/albums/aa294/oldtiffie/M_K2.jpg

Another view of the bottom showing the pivot pin holding arrangement.

http://i200.photobucket.com/albums/aa294/oldtiffie/M_K3.jpg
A view of the underside. The big block is grasped in the milling machine vise. Through the big block is a threaded rod with a hole into which the various pivot pins fit. Tightening the nut on the threaded rod locks the pivot pin into a V-groove in the main block to keep the pivot pin vertical.


2.
The next is from a well-known US machinist:

http://i200.photobucket.com/albums/aa294/oldtiffie/Rounder1.jpg

This (with stops) is the basis of the methods I use. I pack the part to be milled up with a say 1/8" thick flat washer so that I can keep the job within the milling cutter (say by 1/16") and still have 1/16" clear of the mill table, vice vee-block or whatever I have the spindle mounted on/in.

I have a screw thread sticking up above the job (on the spindle) and put a flat washer on it over the job followed by a "nyloc" nut or perhaps a spring/"star" washer followed by a nut to suit. I torque the nut up to get a "good" resistance" on the bar/lever/job but not so tight that I cannot move and "feel" the job as it moves under the cutter.

[Edit]
It is absolutely essential to have that nut and washer on the top as said but its other important purpose is to make sure that the job does not "climb up" the bolt/pivot and/or the end-mill/cutter as the reactive forces due too the spiral in the cutter is the tendency to "climb" (up) the cutter. The reactive forces of/on the spiral of the cutter is to make the cutter "climb down" the job and out of the collet. These will be of no concern if the collet holds the cutter tightly and the nut and washer's hold the job down. Make sure to that the bolt/pivot is firmly held in the vice, vee/block or what-ever. These forces and reactions are neither peculiar nor restricted to this set-up. It is just the normal forces and reactions in milling at any time.
[End edit]


It is very wise to put stops on this method too - just use the same principles as Marv K. I usually use long bolts screwed and lock-nutted to a piece of spare steel plat which is clamped to the mill table to suit.

If in any doubt - go back to using the rotary table.

If it were me on this job on a rotary table, I would disengage the worm and wheel drive on the rotab and put at least one steel/metal bar sized to suit the slots in the rotab table and use them as handles as before.

brian Rupnow
06-29-2008, 11:47 AM
The operation was a success!!! The patient lived!!! It was a trick---the radius wasn't at the end, it was half way up the peice, but that is to hard to explain with text, and all the same rules apply. My rotary table works excellent, and I'm glad I spent the money to buy it. Here is a picture of my set up, and of the machined part. The round part with the red end is the locator I machined to go in the center of the rotary table faceplate. to locate in the 1/2" hole in the part.
http://i307.photobucket.com/albums/nn294/BrianRupnow/millset-up004.jpg
http://i307.photobucket.com/albums/nn294/BrianRupnow/millset-up001.jpg

deltaenterprizes
06-29-2008, 01:23 PM
Great set up. A smaller diameter 4 flute end mill would malk a smoother cutting action while you were rotating the part and allow you to go a little faster when rotating the part. Try it next time on a piece of scrap, first a bigger one,then a smaller one and see if you notice the difference.You can spin the smaller bit faster also to give a better finish.

Nice work!

dockrat
06-29-2008, 01:53 PM
Nicely done!! I agree with Deltaenterprizes....I now hardly ever use an endmill bigger than 1/2". In most cases I use a rougher for the major metal removal then switch to a 4 flute carbide and high speed for the final finishing cuts. Your project reminds me of my first rotab project where I made a combination spindle drawbar/vise wrench out of 1/2" steel plate.

http://i253.photobucket.com/albums/hh67/Dockrat1/IMGP0613Small.jpg

oldtiffie
06-29-2008, 08:35 PM
Very nice job and well executed Brian.

lane
06-29-2008, 09:02 PM
I will add a little trick I use for you and any other newbe out their,are any one else for that matter.
most but not all rotary tables have a morse taper hole in the center . Either a #2.3.are4 . Get you a arbor of you size taper usually a arbor for a drill chuck ,Cut the tang off and insert in to the rotary table and mark to a few thousand below flush . remove from table put in lathe and face off to your mark . try in table to make sure it is below flush. If so put arbor in lathe spindle you may have to sleeve up to fit and drill and Bore To a real close slip fit on a 1/2 dia pin . Bore hole only about 1 inch deep with a 1/4 inch drilled through hole for knocking out pin.
Now any tome you need to cut a radius on a part with a center hole you can turn up a pin to fit the 1/2 inch hole in the table and turn the other end to fit the part . Save your pins at some point in time you will have a collection of pins to fit about any thing. once the tapered plug is inserted in Rotary table just leave in from the own, and your 1/2 inch hole will always be ready. quick and dirty center location. less set up time more machine time.

brian Rupnow
06-29-2008, 09:05 PM
Thanks for the kind words, fellows. Here is a picture of the engine I am currently building, showing the finished part that appears on the milling machine. It is "test assembled" with the flywheel, crankshaft, and main bearing. The bore and stroke of this engine will be the same as the first engine I built, a month ago, but this one will be a double acting engine with steam (compressed air in my case) being ported to both ends of the cylinder alternately, which will effectively double the power, without changing the bore or the stroke.----a pretty neat trick!!!
http://i307.photobucket.com/albums/nn294/BrianRupnow/SEMIFINISHED001.jpg