How to set up 4th axis for location

Picture a rotary table with the center line running parallel to the X axis. Setting X is simple, bump against the end of the part or the end of the blank and you have your X.

Setting Z is also fairly easy as you know what your height to center of your rotation is, and it will always be the same. You can mill a face and rotate and verify height afterwards too.

Now comes Y. Normally on a round part, I just pick up the center of the part/stock and I'm there. But I'm now making a part that is not centered on the Y axis center. It is not a symmetrical part either. I can center on the dovetail fixture which should be pretty close.

My concern comes when it gets down to finishing close tolerance dimensions. With a .001 mis-location on Y and on Z, how can I finesse this down? Is the Z location wrong, or perhaps just the finish tool was off by .0005? What about Y? Narrowing down whether it is a Y fixture location, z tool location or diameter compensation or even tool deflection just sounds like a nightmare to work thru.

Do you guys make a sacrificial part blank and face mill it square to set Z and then put a hole in center of Y to verify set up? What methods do you use to set this up efficiently? I would sure love to gain some knowledge on your methods.
Thanks

Houndogforever said:

Picture a rotary table with the center line running parallel to the X axis. Setting X is simple, bump against the end of the part or the end of the blank and you have your X.

Setting Z is also fairly easy as you know what your height to center of your rotation is, and it will always be the same. You can mill a face and rotate and verify height afterwards too.

Now comes Y. Normally on a round part, I just pick up the center of the part/stock and I'm there. But I'm now making a part that is not centered on the Y axis center. It is not a symmetrical part either. I can center on the dovetail fixture which should be pretty close.

My concern comes when it gets down to finishing close tolerance dimensions. With a .001 mis-location on Y and on Z, how can I finesse this down? Is the Z location wrong, or perhaps just the finish tool was off by .0005? What about Y? Narrowing down whether it is a Y fixture location, z tool location or diameter compensation or even tool deflection just sounds like a nightmare to work thru.

Do you guys make a sacrificial part blank and face mill it square to set Z and then put a hole in center of Y to verify set up? What methods do you use to set this up efficiently? I would sure love to gain some knowledge on your methods.
Thanks

Click to expand...

Z is just relative to your tool length offsets. So if your tools are all .001 shorter than they are supposed to be you can comp your Z fixture center height.

When you first setup your 4th you should be able to cut a square with the bottom of the tool (all 4 sides). Measure for thickness and adjust center height. Then use a 3d indicator and find center in Y axis off your cut stock. Once you have these two numbers you should be good for as long as you dont take the 4th off....

However... you are more than likely running this on a C frame vertical that will move the Z and Y axis in thermal growth of the machine so you will be chasing dimensions throughout the day because your center line will keep moving. Easiest way is to add a renishaw probe to use to hold tight tolerances. Cut your datum and probe.

Doing 5 axis work (similar enough) I try to finish as much of the critical sections using 1 strategy. Either use all Z finishing or all side finishing. I know in reality you can't always do this but the more you can limit to one source of error the better off you will be. Also the Z axis error will double in your part so I'd try to use the XY and rotation to finish more than the Z axis cutting.

The better you dial everything in on a test part at the beginning of the job the better off you will be. If you know at 8am you are adjusted perfect but at 4pm you are off .001 then you will be able to comp it. If you try to just setup new tools, new fixture, new part and cut first shot you will always be kind of guessing whats off.

One way is to use tooling balls and construction holes to pick up offsets at angles. It can be on the part or on the fixture. I would recommend coming from the tooling ball at every work offset.

You could edge find a feature, rotate 180 and edge find again.

Rogue Willie said:

You could edge find a feature, rotate 180 and edge find again.

Click to expand...

That's normally how I do it, pick up the same feature on both side of the Y axis with my Haimer.

As others mentioned Z I cut the top face, spin it 180º and cut again, measure the part and split the Z position.

To find Z, clamp a part in a vise and use a facemill with fresh inserts to face both ends of the part by rotating -90.0 and +90.0. Measure the part with a mic and comp the Z accordingly.

To find Y, rotate back to 0.0 and probe the part to find the center.

Like dstyr said, axis growth is going to happen, especially Z. The easiest way to comp Z is to touch off a dummy tool and comp the Z common offset by some fraction of the difference between the old and new values. That fraction is dependent on where your rotab centerline is relative to the table and the spindle. Another way is to probe a fixed reference block mounted to the table.

Of course you can also probe the part itself but that can add cycle time since you'd have to take multiple finish passes.

Here is the first finished part out of steel. A few minor corrections during the aluminum set up phase, a complete and total F-up, and now I'm inside of 15 minutes from a dovetail prepped block to this. Just need to mill off the dovetail and drill and tap a 7/16 hole thru the center line of that big corner radius.

Set up is really key to this stuff. Making sure the rotary face plate is flat and square, even if needing to shim it a couple .001. I got the TIR across the face plate to be .0006 and called it good seeing as the closest locational tolerance on this is +/-.005.

Then I pre cut some squares to set up exact Y-axis center line and Z height levels. It looks like one project will be to make some dovetail blanks that I can use as set up parts to destroy for the future. maybe a 2" aluminum round bar with the dovetail on one end and at center. Then I could mill it to 1.75, then 1.50, then 1.25 etc as I keep reusing it until I make another.

Thanks to all on your suggestions, I'm looking forward to these parts now.


PS, sure wish I had probing, but this old Fadal VMC15XT has served me well since I bought it back in 1994.

Nice Job! Part looks great.

Sacrificial set-up parts/stock for 4th are a must.