What's new
What's new

Help with rotary table setup!

madkaw284

Plastic
Joined
Oct 16, 2018
Hello all and thank you in advance for taking the time to read this.
I am a welder by trade but very now and then have to get on the lathe and mill. I am by no means considered a machinist but do know my around the machinery really well. This (rotary table) is a particular area I would like to get better at and so I figured, what better place to ask. Anyway!
Let’s say I have to machine a few slots on a specified diameter on a piece of 4x4x 1/4” steel. With 4x4 being the finished size of the part, how do you guys center and along the part on the table? Of course after centering the rotary table to the chuck.
I’ve always just used a piece of stock larger than the finished dimensions, machines all the interior holes and then mill the outside edges to get the finished part but I know there has to be a way to indicate a finished size part on a rotary table.
Thanks again everyone


Sent from my iPhone using Tapatalk
 
but I know there has to be a way to indicate a finished size part on a rotary table.

Your fixture should hold it on center and concentric to the axis of rotation.
We use a 3 jaw chuck that we can indicate in, just like on an engine lathe.
Or we make soft jaws for odd shaped parts.
Do get it close, we just clamp onto a 1" dowel pin and indicate that in, then chuck onto the part.
 
Your fixture should hold it on center and concentric to the axis of rotation.
We use a 3 jaw chuck that we can indicate in, just like on an engine lathe.
Or we make soft jaws for odd shaped parts.
Do get it close, we just clamp onto a 1" dowel pin and indicate that in, then chuck onto the part.

Yeah, I get that once the table is centered that as long as you don’t move your cross slides that it will stay concentric. What I’m trying to figure out is how to hold down and align a part that has been cut to finished size so I can mill it accordingly. Here’s an example of a part I need to do. So say I’m given a plate that is cut to 3 1/2” x 5”, my rotary table is centered and I have center punched the plate to locate its center on the mill. I then locate that center punch and have it clamped down, now how do I align the X axis?


6c7cf017a592b4f59404a9fc142dc215.jpg

6c7cf017a592b4f59404a9fc142dc215.jpg



Sent from my iPhone using Tapatalk
 
You tram in the x axis with an indicator the same way you would the vise jaw. Then set you RT to zero.

You don't need a center punch mark at all. Zero the mill over the center of the RT the calculate the moves to to dial in the reference surfaces of the part with an edge finder.

You need two points of contact on one axis for location and alignment and only one point of contact for location. on the other.

If it's more than one part you could put fences on the rotary table to locate parts without measuring each one.

Heck, it might be easier to set up the fences with Gage blocks or an adjustable parallel and a center pin in the table. Set up the offset for the first fence and tram it in, then add stop block on the other axis.

You may be cutting a curve, but locating the part is still just a simple grid.
 
My RT has a MT center hole so a MT adapter will self center in it. Weather by good luck or good planning, my lathe has the same MT in the headstock spindle. So I find that I can machine an unhardened MT adopter in the lathe to whatever diameter the center hole in my part may be. Your part has a center hole and you can use it before it is tapped. Here is how I would proceed with your part.

1. Machine a MT adopter or whatever fits your RT's center hole with a pin that matches that center hole in your part. For best accuracy you can ream that hole to size.
2. Mount the RT on the mill and center it under the spindle. Lock the table down or zero the dials or DRO. Probably a good idea to zero the angular reading at this point.
3. Put the adopter in the RT and drop the part on it. Then the part is automatically centered under the spindle.
4. Use a DI to align the edge in the X direction.

That should do it.

A further note, I do not have one of those coax centering indicators so I also made an MT adapter with an accurate, reamed center hole. I use it in the RT with a piece of ground, round stock (shaft stock) in a collet to center the RT under the spindle. I move the table (X - Y) until that round pin enters the hole in the MT adapter easily. That centers the table under the spindle quickly and accurately. For better accuracy I can mount a DI in the spindle and sweep it around the OD of that projection on the MT adapter. That takes an additional arm to hold the DI in a collet.
 
My RT has a MT center hole so a MT adapter will self center in it. Weather by good luck or good planning, my lathe has the same MT in the headstock spindle. So I find that I can machine an unhardened MT adopter in the lathe to whatever diameter the center hole in my part may be. Your part has a center hole and you can use it before it is tapped. Here is how I would proceed with your part.

1. Machine a MT adopter or whatever fits your RT's center hole with a pin that matches that center hole in your part. For best accuracy you can ream that hole to size.
2. Mount the RT on the mill and center it under the spindle. Lock the table down or zero the dials or DRO. Probably a good idea to zero the angular reading at this point.
3. Put the adopter in the RT and drop the part on it. Then the part is automatically centered under the spindle.
4. Use a DI to align the edge in the X direction.

That should do it.

A further note, I do not have one of those coax centering indicators so I also made an MT adapter with an accurate, reamed center hole. I use it in the RT with a piece of ground, round stock (shaft stock) in a collet to center the RT under the spindle. I move the table (X - Y) until that round pin enters the hole in the MT adapter easily. That centers the table under the spindle quickly and accurately. For better accuracy I can mount a DI in the spindle and sweep it around the OD of that projection on the MT adapter. That takes an additional arm to hold the DI in a collet.

Ok, that’s a good idea. Actually if you look closely at the print that tapped hole is just off center of the axis of rotation needed to mill the slots but I get what you’re saying.
My other idea was to mount the part in a standard vice and indicate the edges and use a small center drill to just make a reference indent on the center of rotation on the part. Then mount and center the RT, zero out the DRO and put a center finder in the mill and bring it down to the center mark on the part. Clamp the part down and rotate the table and slide the x axis back and forth with an indicator on the edge of the part until it’s squared. Only problem then would be that my RT would not be on zero.
I would like to hear others ideas on how they would setup and machine this part.
 
You've not stated how many parts or the expected accuracy (tolerance) for the features, that makes a difference. I'd follow the suggestions others have made and use an edge finder on a finished part, a center finder won't be a good way to do this. Either clap the part directly to the RT or sit in a vise, whichever is best for you. If it's multiple parts you'll need a fence/stop for repeatable results. You probably know this but I'll mention it anyway. Always rotate in the same direction, I use clockwise, as the backlash in most RT's is enough to throw your readings off. Use conventional milling with an RT, climb milling will NOT work well with most RT's and produce a bad wall finish. You're going to need a DTI for some of this. Sorry I can't offer better suggestions, I'd have to see what you're working with. Indicate the center hole of the RT, not all of them are truly in the center, fences mounted to the RT for locating a precision vise. Precision vise with a stop for the part. Measure the precision vise and do the math, not a lot of shortcuts to this. Hope this helped.
 
I need to make two of these parts. Tolerance is +/- .008”

So you would suggest mounting a vice to the RT and not clamping directly to the table?
Just please understand that I’m trying to learn, not questioning anyone’s ideas.


Sent from my iPhone using Tapatalk
 
Need to make a bit of tooling to use my method, but its stuff that will be used for other work.

Need a 60*center for the mill:
What i do is take a 1/2" piece of drill rod, perhaps 2" overall length.
Grip in a good collet on the lathe and turn a true 60* center on one end.
Heat the tip with torch till the material goes non magnetic , then quench in oil using figure 8 motion.
Temper the hardened end by heating with propane torch to light straw and quench again in water or oil....

Setup your plate in a vise of on the mill table with side trammed to be true to the mill table axis.
Use edge finder to locate center of the needed features (center of rotation), and center drill the plate at that location.

Setup the rotary table on the mill and set the table rotation at zero...
Indicate in the center of the rotary table to be concentric with the mill spindle.

Fit sharpie into the spindle of the mill (collet to hold the OD) ..May need to make a sleeve for a collet here
Move along one axis the center width of the plate plus the approximate radius of the sharpie point..(long feed)

Run the quill down and touch the sharpie to the rotary table table and by moving the mill table (cross feed) draw a line that will be parallel to the work.....

Move the mill back to the center of the rotary table.
Install a center in the mill collet (see above)
Place the plate on the rotary table with one edge roughly aligned with the sharpie mark....
Bring the center down (quill) to enter the center drilling on the plate and using the quill handle lightly tension against the plate.

Use a soft mallet to tap the plate lightly to align with the sharpie mark, and clamp the plate, all while holding the center engaged...

Now, use an indicator to final align the edge of the plate to be true to the machine ........Do this by rotating the table....Be sure to make all corrections by turning hand wheel in the direction that you will
be rotating the part for your cutting (remove backlash)

Set Rotary table micrometer collar to Zero.
If you have a moveable degree pointer for the table also set it to zero (most have some adjustment here)....If that is not available on your table make a simple sheet steel pointer plate that is just plain(no pointer.
Install the new pointer plate and mark the zero with sharpie....The micrometer collar will be where you get the accuracy....

Move to and cut features as needed...be sure to account for backlash in the table worm...(The starting point for the rotary cuts need to be positioned by moving in the direction you moved to set the plate to zero.)...

Cheers Ross
 
Hi, You have probably gone ahead and finished the parts by now, but I think the drawing is deceptive. It looks like you have 2 different centers for your circular slots. The centers are .130" apart. That would mean two different set-ups or maybe having your part mounted on an x-y table, mounted on the rotary table. Tom from Mass.
 
Need to make a bit of tooling to use my method, but its stuff that will be used for other work.

Cheers Ross

This is the concept I’m going to use. Thanks a lot. This seems like the plan that will work best for my setup.


Sent from my iPhone using Tapatalk
 
Hi, You have probably gone ahead and finished the parts by now, but I think the drawing is deceptive. It looks like you have 2 different centers for your circular slots. The centers are .130" apart. That would mean two different set-ups or maybe having your part mounted on an x-y table, mounted on the rotary table. Tom from Mass.

You are correct. I believe an intern probably drew this print up, not the greatest clarity in detail! So yes, I will have to reposition the part after cutting the first slots.


Sent from my iPhone using Tapatalk
 
You tram in the x axis with an indicator the same way you would the vise jaw. Then set you RT to zero.

You don't need a center punch mark at all. Zero the mill over the center of the RT the calculate the moves to to dial in the reference surfaces of the part with an edge finder.

You need two points of contact on one axis for location and alignment and only one point of contact for location. on the other.

If it's more than one part you could put fences on the rotary table to locate parts without measuring each one.

Heck, it might be easier to set up the fences with Gage blocks or an adjustable parallel and a center pin in the table. Set up the offset for the first fence and tram it in, then add stop block on the other axis.

You may be cutting a curve, but locating the part is still just a simple grid.

With a little time and care setting up, you could do the whole part with a 1/4 inch end mill. Would not be the EASIEST way, but it could be done without too much misery if that was all you had.

Use a 2 flute end mill, they tend not to widen the slot, if doing it with a nominally sized cutter.

Just a matter of sorting out the sequence of moves, using due care with a clamp set, and some gage blocks or an adjustable parallel set, and a couple big ol' parallel bars to keep the moves going just where you want them to.
Some relatively clean cutting Al. sheet stock as a sacrificial plate under the work will allow a cut through the work, without gouging up the table, unless you do something foolish.

Clean up the stock square as you can get it, You can do that while the part is on the R/T from the outset, start from the hole that the 1/4 inch thread is going to be in, as your origin point, as that makes it a pretty handy place to start again from if you lose track while moving the part around. Drill and ream out as clean a hole as you can there and you will have a doddle to dial off it or center it up under a spud in the mill.

Plus or minus .008 inch isn't exactly angle grinder and drill press work, but you should have not to hard a time if you use care. Look at the edge of an 8 thou feeler gage with a magnifier. Or better, two stacked together. Compare that to a carefully scribed line. Easy! Just gotta wrap you head around how you plan to approach it. Make notes. Follow them tick off what has been done.
 
You are correct. I believe an intern probably drew this print up, not the greatest clarity in detail! So yes, I will have to reposition the part after cutting the first slots.


Sent from my iPhone using Tapatalk

Dude that is a pretty clear drawing, if a little overloaded with details that could have been clearer.

Beats hell out of the 23 Post-It's notes I was handed, to supposedly cut out all the pieces and braces for a tool I was supposed to make. Guy gave me dimensions and tolerances on a bunch of little fillet blocks that were to be welded in. 23 fricken 2 inch square Post-It's!

Or the seven different views of a reinforcement bracket for a VERY expensive piece of aircraft equipment, all printed out from a bad scan of a worse original, on a single page of letter size paper. That one WAS fun though, and I made a mirror image of that part the following week, so the work that went in to a one-time job saved us a couple hundred thousand in scrapped gear.

You may want to do some Trig to figure out your start and end points for the arcs, as well as to determine the measurements that will tell you if it's pooched.

And, the practice will do you good! :)
 
Dude that is a pretty clear drawing, if a little overloaded with details that could have been clearer.

Beats hell out of the 23 Post-It's notes I was handed, to supposedly cut out all the pieces and braces for a tool I was supposed to make. Guy gave me dimensions and tolerances on a bunch of little fillet blocks that were to be welded in. 23 fricken 2 inch square Post-It's!

Or the seven different views of a reinforcement bracket for a VERY expensive piece of aircraft equipment, all printed out from a bad scan of a worse original, on a single page of letter size paper. That one WAS fun though, and I made a mirror image of that part the following week, so the work that went in to a one-time job saved us a couple hundred thousand in scrapped gear.

You may want to do some Trig to figure out your start and end points for the arcs, as well as to determine the measurements that will tell you if it's pooched.

And, the practice will do you good! :)

It is a good drawing, but it’s not from one of the engineers that I’m used to working with. We have a good repertoire, he knows what I like to see on my prints. This one has everything on it, just have to do a little additional annotations.
Like I mentioned earlier, I’ve done lots of parts similar to this on a rotary table but I’ve always used a piece of stock that is larger than the outside finished dimensions, so I have a little wiggle room. I would machine all the internal features and then mill the outside dimensions to its final size. I just wanted to hear all the different setups you guys use to setup a piece that’s been cut to its final size.
I’ve really learned a lot in this thread and I appreciate everyone’s input. As I get time I’ll try to post up some pictures of the part in progress and then it’s final welded assembly. Here is another part of the assembly I completed yesterday.


2da27775f1f508d5a72abb7e4f72a0e7.jpg



Sent from my iPhone using Tapatalk
 
Good god, Just get it laser cut.

If you have to do it on the mill, put a 10 or 12” rotary table with the 4 jaw independent chuck on it and after centering the table, ( for .008, a Jacobs chuck whose nose taper rides on the edge of the center hole would be fine ) dial in your X and Y ( (with the dro if you have it) and go to work.

If you don’t have the big(ish) 4 jaw, use hold downs, and that al spacer plate.

Use a center finder with the cone tip in a center mark if your plate edges are not true (mill edge on hot rolled or rough bandsawn for example)

Or, start by making some custom tooling, center it within .0002, and waste a hole lot of time. A professional makes things to spec, or a little better. Time is money out here in the real world. Keeping it practical... (LASER CUT IT!)
 
Good god, Just get it laser cut.

If you have to do it on the mill, put a 10 or 12” rotary table with the 4 jaw independent chuck on it and after centering the table, ( for .008, a Jacobs chuck whose nose taper rides on the edge of the center hole would be fine ) dial in your X and Y ( (with the dro if you have it) and go to work.

If you don’t have the big(ish) 4 jaw, use hold downs, and that al spacer plate.

Use a center finder with the cone tip in a center mark if your plate edges are not true (mill edge on hot rolled or rough bandsawn for example)

Or, start by making some custom tooling, center it within .0002, and waste a hole lot of time. A professional makes things to spec, or a little better. Time is money out here in the real world. Keeping it practical... (LASER CUT IT!)

Feel better now after throwing your tantrum?
That’s real easy to say “just get it last cut” but it’s not happening in the particular field I’m in. Thanks everyone else for your help


Sent from my iPhone using Tapatalk
 








 
Back
Top