4th axis on the mini

[JFettig]

I just got my rotary table from LMS and started making parts to convert it.
what I would really like to do is put the stepper behind the table and enclose almost all of it with sheet metal, but for now Ill just stick the stepper strait off the end of the screw. So far I have made the coupler.... and kinda designed the rest.

I just finally figured out to calculate the degrees per step, and it occured to me. How are the feeds set? if I was to cut with X and A axis would I use a really slow feed on the A axis or does it calculate that? it says that the A axis will turn at 1800 degrees per minute, how would I use inches per minute?

I dont have the camera handy otherwize I would post some pics. I will have to get some up soon.

Jon

[3t3d]

Basically the control doesn't know what the feedrate is for a rotary since it depends on the diameter or radius of where the cutter is in relationship to the axis of the rotary.
So, how do controls cope with this you ask?
They use inverse time feedrate. Instead of specifying the feedrate you specify the inverse of the time to complete the command block.
Why use inverse time? You ask now....
Well that way, the smaller number is a slower feedrate, and the larger number is a faster feedrate. The post processor, or the programmer has to calculate the appropriate feedrate, knowing how far from the axis cernterline the tool is.

So, the short answer is, the programmer has to do the calculations.
And, all the controls that I have owned, and used rotary tables, will use regular feedrate. I don't know what the relationship was from feedrate in IPM to degrees per minute. But most jobs, I used the TLAR (*) method of setting the feedrate for the motion with the rotary table.

Most operations I have done with the rotary table though, was postioning the work, to machine multiple faces. Only a couple of jobs actually used rotary and linear motion combined.

Pete

[JFettig]

Thanks 3t3d, that helped some. I supose the next step is to get this thing finished and mount it up and play with it. I am assuming I still zero my tools at the top of the stock right? Do I do something to tell it how far it is from the center line?

Jon

[3t3d]

I just ran a job on the 4'th axis.
Every machinist will have a different way to touch off a part. Some will go on a holy war to convince you that their way is the best. It really depends on the part, and the starting stock etc. etc...

Some parts start with stock that is already machined on the bottom. In that case, I touch off the bottom of the ( vise, parrallels, fixture etc.) and then add in distance to reach the top of the part.
Some parts start out with oversize stock, and no reference to the bottom.. yet. For those, I touch off the top, and program the top of thepart below zero to account for the top being cut off. Or, I touch off the vise, parrallels, or whatever..

Last week I had a part in a fixture on the rotary axis.
This is setting it from A, Y, X. and Z.
I jogged the axis until a test indicator read zero front to back. Then I set the offset for the rotary to zero.
Next I touched off the front edge of the fixture. And noted the Y axis. I jogged the rotary to 180 degrees. And touched off the same point on the fixture, but now it is on the backside. The difference of thos two readings was the center of the fixture, on axis of the rotary.
Next I touched off an edge on the fixture to set the X axis.
Next I touched off a surface at 0 degreee for the rotary, jogged the rotary to 180 degrees, and the surface I touched off before is now upside down. So I clamped a parrallel to it, and touched off of it again. The difference is the Z height for the center of the rotary axis.
I could then set my Z height above that point to match what I needed.

So, it really depends on what your part looks like, and how you planned the job.
There are as many ways to do it as their are people to do it.

hope this gets some ideas going.

Pete

[JFettig]

Thanks, that definately got e somewhere.
Lets say I got 1/2" round stock sticking out of the chuck that will be on my rotary table and I want to cut a spiral.(just generic)
I set y zero centered in the stock and z zero on the top right?
for reference, I will say its a 1/8" ball mill 1/16" deep,
So the code would go something like this:

G0 X-.125 Z.1875 A0
G1 X0 F8
G1 X1 A360 F? (lets say I want to cut at 8 ipm, would I put 8 in there?)
then out

to make a full revolution of the table, I simply do A360 right?
lets say I want to do 2 turns, do I have to change the code to this:


G0 X-.125 Z.1875 A0
G1 X0 F8
G1 X.5 A360 F?
G1 X1 A? what do I put in here to tell it to keep spinning? do I have to use incremental coordinates instead of absolute?
then out

Thanks for the help,
Jon

[3t3d]

Well, it all depends on your controller doesn't it?
I can write:

N300 G01 A720. X1.0

And get two revolutions of the table.
What that does is "wind up" the table (or the control as you see it)
On one of my machines this code:
N310 G12 A0
Will not move the rotary, but it will cancel out the "wind up"
Example 1:

N400 G00 A720.
N410 G00 A-10.

Example 2:

N400 G00 A720.
N406 G12 A0.
N410 G00 A60.

In example 1, the table will spin for two revolutions, then reverse for two revolutions, plus reverse ten more degrees.
IN example 2, the table will spin for two revolutions, then forword 60 more degrees.

Again the control determines what G codes YOU need to use. Probobly not G10, maybe yes. Check your documentation, or better yet, experiment.

Now, what does the feedrate do to your rotary axis speed?
(Shrugs) I don't know. Experiment, or look at your documentation. See of you have inverse time feedrates, or if you just have to make some calculations, and submit a feedrate that does what you want.
You'll figure it out. I can tinker with parameters inside my control, and trick it into all kinds of behaviour. For example telling a different gear ratio from the motor to the table, and again lie to it about the number of encoder pulses.
Basicllay get something that works, and will be intuitive <__LATER ON__>

Hope this gets you going some more.

Pete ..... (which is 3t3d sideways, sort of)

[3t3d]

One more thing to talk about with a 4'th axis setup...
I want to shown wrong here.. Someone speak up on this point.

Any CAM software that I looked at that supports 4'th axis work does not support moving 4 axes at once. They only support positioning, and and at most three axis of motion, until you get into some failry high end CAD/CAM packages, maybe over $6,000. In fact when I was trying to solve a problem several vendors told me I had to go to a 5 axis package to get simulatanous motion in 4 axis.

The actual example that I had is the equivalent of rotating a crankshaft, and cutting tapered threads on one of the crankpins while it is spinnning. That does require four axes of motion simulatneously.

Pete

[Stevie]

Ok to do the C axis rotation with my 4 axis setup
I simply told it to go 1440 dgr and a linear move at the same time; if you specify the feed in that line it will feed the linear at the feedtrate and calculate the feed of the C axis to match the length needed to mill

So my command was simple
G01 C1440 X25(mm) F50
The software calculates the feed for the C to make the cut end at 25mm after 4 rotations
This is for TurboCNC

[Stevie]

I just tried a quick one for you bud

This is a G01 C360 F1.5 (IMP selected)
Stop action photo; can't believe my camera caught the cutter at 3000+ rpm and it looks dead still; good job the chips are flying or you'd never believe me

[JFettig]

Thanks a ton. New cameras do a great job of catching stuff still. I have seen 8000rpm fans be caught still.

About how fast does that guy turn when you give it that command? close to the equivalent of 1.5ipm linear?

Thanks,
Jon

[Stevie]

Nope seems slower
But how to measure it I have no clue

[3t3d]

Originally Posted by Stevie Ok to do the C axis rotation with my 4 axis setup I simply told it to go 1440 dgr and a linear move at the same time; if you specify the feed in that line it will feed the linear at the feedtrate and calculate the feed of the C axis to match the length needed to mill So my command was simple G01 C1440 X25(mm) F50 The software calculates the feed for the C to make the cut end at 25mm after 4 rotations This is for TurboCNC

Thanks, this helps illustrate what I trying to explain. If you are cutting on the rim of a 150mm disk, and the X distance is 3mm, then the feedrate will be a LOT faster than you want. The control will calculate how fast it needs to complete the X move, but cannot possibly know how far from the axis the cut is happeneing. Therefore, the X distance will be at a feedrate of 50, but the rim speed to get in 4 rotations completed will be MUCH faster than the X travel. It may try to travel 3mm in X, but it will have to travel 1885mm on the rim to complete 4 revolutions. So, the cutting speed will be about 628 times faster than you specified with:
G01 C1440 X3 F50

So, for any significant offset from the centerline, or any short move in X or Y, combined with longer moves in A (or C), either the programmer or the POST needs to calculate the correct feedrate. Except for the case where the cutter is very near the centerline, it can be quite different than the feedrate would indicate. In those cases, specifying the time to complete the cut makes more sense.
And using the inverse of the time makes a smaller number feed slower, and a larger number feed faster. If your control supports inverse time.
And the control cannot possibly know what the radius is where the cut is happening. So the programmer or the POST needs to calculate the needed speed.
Pete