Rotary Table Puzzle

[MontanaAardvark]

Thanks for the clear explanation, RJ. This is another example of what I always say about every piece I make is a puzzle. I don't have much experience at this stuff and there are boatloads of tricks I don't know.

The thing that confuses me is that I can see how I might have a couple of mils error in my measurement, but when I do the cut, the center of the cutter is off about 35/40 mils. Remember the Looney Tunes when we were kids and Elmer Fudd or someone would get a giant question mark in the air over his head to show his confusion? I have a cloud of question marks.

Last night you mentioned videos. I found this one, which is a very straightforward trick, but one I don't have the parts for. Since the RT has an MT2 axis, I'd have to turn an MT2 plug like his, and don't really know how to do that on my big lathe. I don't have any handy 1/2" dowel pins. I do have a bag of 1/4" dowel pins I got with intent of making some fixtures for the mill, along with a 1/4" collet, so I might be able to make something like what he does. Or get one of these MT2 to 1/4" mill holder that ought to get me there. I think that for that ($13.95 with two day shipping), I'll give it a try

I have a 2x2x1 block of aluminum I could clamp to the table and cut a half or 3/4" tall cylinder with an End Mill and the RT. Make it less than an inch diameter, so that I could get my micrometer on it. I assume that the same trick with diameter works with both X and Y.

 

[woodchucker]

That's how I started out. Put my 2MT dead center in the RT and then centered the spindle over it by eye with a collet holding a center/edge finder. That's when I discovered that if I rotate the table 180 degrees from where I started, the two centers are no longer in line.

Return it.

 

[MontanaAardvark]

Return it.

Unfortunately, I've had it for 17 months, so I doubt they'd take it back.

 

[GL]

A little off topic. But relating to your engine build and at the risk of getting some flack...you can make a round hole with a boring bar or an end mill with a rotary table on a mill (or the right diameter cutter). Because there are a finite number of steps in the servo system, an interpolated circle is still an approximate circle. Reducing the number of steps to the absurd, an interpolated "circle" could be a square, with rounded corners. Maybe it is close enough, maybe not for a press fit bearing in an engine. The smaller the circle the more the error amplifies.

On topic, to get an indicator of what the real world says and since I wanted to see if I saw any runout on the 12" yuasa table at work. Maybe a tenth. Checked my 12" Veryex, about the same. Both are used and have some indicators of use by people who don't get it - why anyone would allow a mill to touch a table is beyond me, but poop occurs when you get used equipment sometimes. Looks like you have some good advice on centering things up. Making it work is often more than half the battle, and why the setup takes way longer than the doing it. But, hey, you weren't really trying to sleep at 3am anyway. Good luck, have fun.

 

[RJSakowski]

Thanks for the clear explanation, RJ. This is another example of what I always say about every piece I make is a puzzle. I don't have much experience at this stuff and there are boatloads of tricks I don't know.

The thing that confuses me is that I can see how I might have a couple of mils error in my measurement, but when I do the cut, the center of the cutter is off about 35/40 mils. Remember the Looney Tunes when we were kids and Elmer Fudd or someone would get a giant question mark in the air over his head to show his confusion? I have a cloud of question marks.

Last night you mentioned videos. I found this one, which is a very straightforward trick, but one I don't have the parts for. Since the RT has an MT2 axis, I'd have to turn an MT2 plug like his, and don't really know how to do that on my big lathe. I don't have any handy 1/2" dowel pins. I do have a bag of 1/4" dowel pins I got with intent of making some fixtures for the mill, along with a 1/4" collet, so I might be able to make something like what he does. Or get one of these MT2 to 1/4" mill holder that ought to get me there. I think that for that ($13.95 with two day shipping), I'll give it a try

I have a 2x2x1 block of aluminum I could clamp to the table and cut a half or 3/4" tall cylinder with an End Mill and the RT. Make it less than an inch diameter, so that I could get my micrometer on it. I assume that the same trick with diameter works with both X and Y.

The video you linked and several by Mr Pete that followed are both good ways to center. They do say that the insert plug into the into the RT socket is a quick but not necessarily the most accurate way but as Tom showed it did get him within a half thousandth.

There are some assumptions made; that the mill spindle has no runout and that the RT socket is concentric with the RT axis of rotation. As long as the assumptions are good, the plug method will get you close enough for almost all purposes. If you have spindle runout. the indicator method will cancel out the runout. If there is runout on the RT, neither of these methods will be appropriate and a method like I had first suggested should be used.

Concerning using a plug, your idea of using and end mill holder should work. I am assuming that you are looking at the 1/4" because of the dowel pins that you already have. How are you planning on using it? You could insert a pin which would fit an R8 collet in your lathe, in which I would recommend getting a larger diameter. You can easily turn a a zero runout pin to to diameter. Another way would be to sweep the outside of the end mill holder with an indicator. I would expect that the outside would be concentric with the taper but that would have to be verified since that surface isn't critical to function of the end mill holder.

You could turn an MT2 taper with your 3540. You would have to offset the tailstock and turn between centers. You will also need some way of verifying your work. A common way is using a mating socket and blueing. You could also use a dial indicator and known length spacer ro measure carriage movement. I would set the dial indicator up in the tool holder and set a carriage stop up. Run the carriage up to the stop and run the dial indicator into the taper surface and make a reading. Without moving the cross feed, back the carriage from the stop and place the spacer between the stop and the carriage and run the carriage to the spacer. Read the dial indicator. You now have a difference in radius of the taper and a known distance between them which will allow you to calculate the raper.

Since you have a CNC mill, you could also make rhe taper on the mill. Chuck an appropriate length of of 3/4 round in the mill spindle and use the mill as a vertical lathe. I would pull rhe 4 way tool holder from the lathe and mount it in my mill vise with an suitable lathe tool. Cutting the taper is then a fairly simple G code program The specification of an MT2 is .7000" major diameter, .5720" minor diameter, 2.5625" length. The difference in diameter is .04995" so on a single side, the increase is .024925". A G code block for making the cut would be something like G91 G01 X-.0250 Y-2.5625 if the cutting edge of the tool was located on the spindle axis in y and to the left of the spindle in x. I would then return to the start and advance my tool by my depth of cut and repeat. Keep in mind that the movements are the reverse of what you would expect for normal milling.

 

[MontanaAardvark]

I had an interesting few hours in the shop yesterday and can't say I have much additional insight.

To begin with, I may not have been clear that I'm using the table with the rotational axis vertical, parallel to Z. I've measured my spindle runout close to the collet and found it barely moving my DTI, so less than the .0005 marks on it. Are all of my collets that good? I don't know for sure.

I decided to clamp a block of aluminum to the rotary table and machine a cylinder in it. A convenient diameter to use seemed to be .750. I'd move the mill in X only and use a .250 end mill. This is easy stuff, right? A 3/4" diameter means a 3/8 radius, and a 1/8" radius to the cutter's center means the center of the spindle should be 4/8, 0.500", from the center of rotation. So I moved X to 0.500, started the cut and rotated the table 360, dropped the cutter .050 at a time and made cuts to make the ring 0.500 deep.



You might be able to see the slots I started to cut in from the sides in both +/- X so I could fit the micrometer in there, but I stuck the calipers on it. (the half inch slot is too narrow for the micrometer)

The diameter is almost 0.700. That means the spindle was really .025 closer to the center of rotation than it should have been. With that big a difference, I don't need to use micrometers, but I could cut the second pass on those slots so that it's wide enough for the micrometer.

That tells me that if I put the edge finder and find that right edge of the cylinder, it should come out at 0.350 - if I use my edge finder and add its radius, the means the edge should read .450 on the DRO. I don't recall what it read at the moment, but I think it was around .465. I set the DRO to .450, what it should have read.

Now I go to the negative X (left) side of the cylinder. The X should read -.450, right? Nope. -.433. That gives 0.350 and 0.333 or 0.683 diameter? When the calipers read 0.700?

Faced with that confusion, I quit for the night.

Not very evident in the picture, but evident by looking at it is that the Y axis is also off. I don't think it's 1/8 off, but could be more than 1/16.

It seems to me that this big difference in the X axis could conceivably be a problem with accuracy of the motion - motor tuning in Mach 3 or the hardware. I haven't verified that in a while, it was accurate before, but I can do that fairly easily, at least comparing what I measure that block of aluminum to be with calipers to what the mill says it moves.

The only things I can think to do now is verify the accuracy of motion, then find the center for both axes on that cylinder and then try to repeat the engraving point trick and see if it turns a donut or it really looks like a pinpoint.

 

[MontanaAardvark]

Not sure why this box is here?

 

[RJSakowski]

I had an interesting few hours in the shop yesterday and can't say I have much additional insight.

To begin with, I may not have been clear that I'm using the table with the rotational axis vertical, parallel to Z. I've measured my spindle runout close to the collet and found it barely moving my DTI, so less than the .0005 marks on it. Are all of my collets that good? I don't know for sure.

I decided to clamp a block of aluminum to the rotary table and machine a cylinder in it. A convenient diameter to use seemed to be .750. I'd move the mill in X only and use a .250 end mill. This is easy stuff, right? A 3/4" diameter means a 3/8 radius, and a 1/8" radius to the cutter's center means the center of the spindle should be 4/8, 0.500", from the center of rotation. So I moved X to 0.500, started the cut and rotated the table 360, dropped the cutter .050 at a time and made cuts to make the ring 0.500 deep.

View attachment 266033

You might be able to see the slots I started to cut in from the sides in both +/- X so I could fit the micrometer in there, but I stuck the calipers on it. (the half inch slot is too narrow for the micrometer)

The diameter is almost 0.700. That means the spindle was really .025 closer to the center of rotation than it should have been. With that big a difference, I don't need to use micrometers, but I could cut the second pass on those slots so that it's wide enough for the micrometer.

That tells me that if I put the edge finder and find that right edge of the cylinder, it should come out at 0.350 - if I use my edge finder and add its radius, the means the edge should read .450 on the DRO. I don't recall what it read at the moment, but I think it was around .465. I set the DRO to .450, what it should have read.

Now I go to the negative X (left) side of the cylinder. The X should read -.450, right? Nope. -.433. That gives 0.350 and 0.333 or 0.683 diameter? When the calipers read 0.700?

Faced with that confusion, I quit for the night.

Not very evident in the picture, but evident by looking at it is that the Y axis is also off. I don't think it's 1/8 off, but could be more than 1/16.

It seems to me that this big difference in the X axis could conceivably be a problem with accuracy of the motion - motor tuning in Mach 3 or the hardware. I haven't verified that in a while, it was accurate before, but I can do that fairly easily, at least comparing what I measure that block of aluminum to be with calipers to what the mill says it moves.

The only things I can think to do now is verify the accuracy of motion, then find the center for both axes on that cylinder and then try to repeat the engraving point trick and see if it turns a donut or it really looks like a pinpoint.

Here is an analysis based on your description. The red lines represent the cylinder that you machined. It will be concentric with the RT rotational axis. The black lines deal with your edge finder. The reason that the total distance between the two positions is less than the diameter of the cylinder plus the diameter of the edge finder is that you are not lined up on the diameter of the cylinder. The x position of the cylinder is .0085" and the y position is -.0871". If you move to those coordinates and set x and y to zero. you should be close. I would make that change and recheck both x and y with the edge finder again. You should be golden. Once satisfied with the setting, I would remove the cylinder and sweep the MT2 socket to check for runout. If you find that good, you should be OK using the method in the link you gave.

 

[Doubleeboy]

Since my spindle has #3MT, I use my live lathe center to get the RT centered, then bolt it down. Simple and accurate.

If you have a high quality rotary table like a Moore this method is great. If you have a Chinese budget rotary table this method may leave a bit to be desired. More than one model making acquaintance of mine has found that the MT bore of the RT is not on center, could be off a couple or more thou. If that difference is of no issue to your level of precision required no problem, but if you need a round machined feature located to precise points the budget RT may leave you high and dry. Early on I had a no name RT from Wholesale tool, after being burnt by the out of place MT bore several times I got rid of it. With more experience now I would have made a dummy slug to fill MT leaving a stub that I could machine true with each use, to help locate true center. So basically what I have spent too much time describing is dont trust the MT to be dead center on the RT unless its a very high end unit.

 

[MontanaAardvark]

Here is an analysis based on your description. The red lines represent the cylinder that you machined. It will be concentric with the RT rotational axis. The black lines deal with your edge finder. The reason that the total distance between the two positions is less than the diameter of the cylinder plus the diameter of the edge finder is that you are not lined up on the diameter of the cylinder. The x position of the cylinder is .0085" and the y position is -.0871". If you move to those coordinates and set x and y to zero. you should be close. I would make that change and recheck both x and y with the edge finder again. You should be golden. Once satisfied with the setting, I would remove the cylinder and sweep the MT2 socket to check for runout. If you find that good, you should be OK using the method in the link you gave.
View attachment 266035

I think you're exactly right. I took that .433 and .450 and split the difference (.017/2) and offset the zero on X so that both ends of the diameter (which was eye-balled (and looked a little better than your drawing to my eyes). Then repeated for Y. Then I swept the cylinder with my halves indicator and it stayed within .001, except for a couple of divots in the cylinder that were naked eye visible. (A rookie machinist mistake - I ran the outer part of the spindle into one of my clamps. It's visible in the picture above - top clamp.)

I then went to 0,0 and used a different (sharper) engraving point and there was essentially no movement - .001 or .002.

I think the next phase is to pull the fixture and go back to the work piece. (I have enough clamps here to keep the house from moving, and I don't think I get that alternative with the real piece.

Again, this is from "The Shop Wisdom of Philip Duclos", so I'm hesitant to put a fully dimensioned drawing here, but the part looks like this (a few dimensions obscured).


Duclos put the cross hairs shown in the center of the circular part of the pedestal over the axis of the RT and then used a 3/4" EM to cut half the outer profile, then moved the clamps to the other side, one at a time.