4th axis setup

How do you set the location, xyz of 4th axis rotary table? The manual from what I’ve read tends more to 5 axis and using the dwo tcpc options, that I don’t have,to setup. Also there is nothing on the internet or on haas website that I’ve seen that clearly talks about the 4th alone. Everything I see regard a tilting 4th axis and will have a picture of a 5 axis trunnion.

I went into setting but like a lot of things on cnc controllers, the same page acts differently depending on what mode your in and I thought i screwed up bad last night when I lost rotary zero but I found the file and reloaded it.but, That froze the hole machine up till I figured out what I did and fixed it but, I don’t see anything about 4th only rotary setup. The center of rotation,z,im sure is obvious but, what do I need to do so that when I run a part it knows exactly where it is on the table? just like if You had probed a corner of a vise.

Not sure I understand the question? You would tram in the Y axis for Y zero, X0 would be the left/right end of part (just like anything else) and Z zero would be the center of rotation in the Z axis, ie if you have a 1" diamter bar, touch off the top of bar at Y0, then subtract .5 to get to center.

^^ All assuming you are using the 4th axis mounted so the bar/parts run left to right in the X axis.

If you are probing, can use the 'regular' probe routines, the only thing you need to do is subtract half the bar/part diameter for Z, the other axis will be set by your probe routines. And if you have an orientation to hold in A (like a flat face on something) remember to set your A axis to zero as well.

Yes sir correct, it is mount with the bore parallel with the x. This is what I’ve done so far. I got it trammed in the Y and secured. I chucked a 4” diameter of aluminum round stock and probed the xyz. Then I tried to run a test cut with fusion 360 cam and it thought the workpiece was higher about 4 inches higher as it was cutting 4” of air above the part. It might just be a setting in the cam software I’m looking past? But I’ll have to look into that.

Shawn_Laughlin said:

Yes sir correct, it is mount with the bore parallel with the x. This is what I’ve done so far. I got it trammed in the Y and secured. I chucked a 4” diameter of aluminum round stock and probed the xyz. Then I tried to run a test cut with fusion 360 cam and it thought the workpiece was higher about 4 inches higher as it was cutting 4” of air above the part. It might just be a setting in the cam software I’m looking past? But I’ll have to look into that.

Click to expand...

Are you programming centerline in your CAM? YZ should be center to get everything to work out. You could program from top, but once you rotate the part it will get wonky.

In effect your Z moves will be positive on the top side, and negative once you move past center int he negative direction. I would *think* (without seeing your part) you should see a mix of positive and negative Z values in your program.

Shawn_Laughlin said:

Yes sir correct, it is mount with the bore parallel with the x. This is what I’ve done so far. I got it trammed in the Y and secured. I chucked a 4” diameter of aluminum round stock and probed the xyz. Then I tried to run a test cut with fusion 360 cam and it thought the workpiece was higher about 4 inches higher as it was cutting 4” of air above the part. It might just be a setting in the cam software I’m looking past? But I’ll have to look into that.

Click to expand...

Sounds like you are on the right track.
Its been my experience that when programming a 4th axis if I am hand programming I use the outside diameter (or top surface(s)) as Z0.....but when using a cam system I will always use the center of the indexer as Z0.....
I am sure others have differing experiences
In the machines I am programming right now....our indexers stay in the machines. I program with Z0 being at the center of the indexer.....the face plate being Y 0 (our indexers are mounted 90 degrees from yours, they rotate around the Y axis) X 0 being the centerline of the indexer. Then if my part is not fixtured on center....i figure that all out and put that into my cam system....
This way my guys never have to indicate/edge find home. until there is an oops.

A snippet of drilling code from a program we run. Notice most of the Z values are positive since Z0 is the center of part.

( SPOT 1/4-36 )
N8490 T2 M6
N8500 G0 G90 G54 X.35 Y0. A360. S6723 M3
N8510 G43 H2 Z3.
N8520 M8
N8530 G98 G81 Z.285 R.425 F6.7
N8540 G80
( SPOT 0-80 )
N8550 A540.
N8560 X.45
N8570 G98 G81 Z.153 R.285 F6.7
N8580 G80
( SPOT 2-56 )
N8590 X.1125
N8600 G98 G81 Z.141 R.285 F6.7
N8610 G80
M9
N8620 M5
N8630 G91 G28 Z0.
N8640 M01
( DRILL .089 )
N8650 T12 M6
N8660 G0 G90 G54 X.35 Y0. A360. S4292 M3
N8670 G43 H12 Z3.
N8680 M8
N8690 G98 G83 Z-.04 R.425 Q.03 F8.6
N8700 G80
M9
N8710 M5
N8720 G91 G28 Z0.
N8730 M01

Might be a good idea to keep a +Z offset in the system for these early tests, trying to make sure you don't have a crash. Once you've done some dry runs and seen that the paths look as expected, then you can remove the offset to try some proper cuts.

make sure you review your PostProcessor file for F360 and their HSM cam. Lot's of REM comments and some things you may or may not need to review. For 3+2 we most certainly did. I thik there are some 4th items in there... PS what year is your Haas?

If you are cutting on the perifery or where there is simultaneous rotation and XYZ motion remember to put the diameter (or radius) of the part in the settings. Otherwise the machine cannot keep them in sync, at least on my '91. Does not apply to an M function box.
If I am machining on the side I would make Z0 the part. That way the Z values are the depth, you do not have to subtract the radius of the part from your Z cut.
I was drilling spoke holes in a hub so the rotary axis was inclined to the machine X. Setting zero on that was a little more tricky.