Control of Mill/Turn output (C axis vs Y)

[flatout3d]

Machine: Mill/Turn w/ C & Y capability

In this example I attempt to drill/ tap a single hole perpendicular to the z axis. I expect that the Y axis will not be employed in the output yet it is. I researched the forum for help and found examples that use a manual NC command (usepolarmode(in this file), and useXZCmode) however these did not change the posted output. I also see guidance to position the toolpath so that it is below the machine centerline to force C axis only positioning. I attempted this by flipping the X axis orientation in this file and the output did not change. Any help to build my understanding for how setup Fusion 360 to leverage C vs Y (with the other axis ) and vice versa is appreciated. I have included the post file and the fusion file.

[Anonymous]

Hole is pointing to model center line, Y0 in output before drilling cycle means that Y axis is being set to its home position, not being used.

Polar and XZC modes only work in G17 (XY plane), tool approach is in Z axis.

In setup of your file, you cannot use chamfer of model as both X and Z axis orientation, it is operantly being ignored by Fusion but if you had more complex model it would result in problems down the line.

If there are no usable features on model to reference X axis off of, make a sketch line, use plane or construction line.

[flatout3d]

thanks for considering this, in the model file provided the chamfer edge is used to define Z and the radial hole surface to define the X? In the output for a part like this I generally would not reference the Y axis or associated Y axis activation codes since, as you describe, the radial hole centerline is directly over the rotational axis. I would simply position in XCZ and drill through using X only. If there where several similar holes positioned around the part then I would reposition C only and repeat the X axis move to drill each hole.  How would this be accomplished in the context of this model?

[flatout3d]

This is another example in which the desired output is CX motion (end mill axis perpendicular to the spindle axis) to mill the ball nosed shaped offset radial slot. In this case I may want to use the Y to offset the tool to cut partially on the radial part of the ball end mill tip (instead of directly on the tip). How is this accomplished? Is it a similar problem?

[Anonymous]

When Y axis is not active, post outputs "Y0" as a way to prepare positioning of the tool. It's redundant function in post because after any use of Y axis, it needs to be zeroed before you can index turret on mill-turn.

If Y axis was left in off position, all your turning tools would be disqualified and unable to work.

If you had a hole pattern around tube, you could program one and set circular pattern to do the rest, as a result, C axis would index so that each hole is in line with X axis and repeat drilling cycle at each position.

[Anonymous]

You have to use wrap function to drive C axis so Trace is not going to work here, I used 2D contour.

Ignore the warning, you have to set compensation to off, which is in conflict with the fact that in wrap function tool compensation is not allowed.

Note the dummy body used for wrapping and .001 wide split in model to break the contour and allow for unwrapping of cylinder.

Also, you want the cut to start at shallow point on slot so that's where X axis in setup needs to point, that will become C0 when posted.

[Anonymous]

In your file using Trace, C axis is being indexed as tool follows sketch, not a conventional way of programming this feature because tool is wiping out model, crashing, due to wrong orientation.

Now, thinking outside of chip barrel, it posts in polar mode due to tool orientation and it should work, so long as you mount tool in radial orientation at the machine because programmed point is tip of ball end mill in either orientation.

[flatout3d]

Thanks, the circular pattern worked well and output the C index as desired. I will study the other examples you provided for tackling the offset  radial slot. Thanks again.

[Anonymous]

Did you miss my post above last one, shows you the way to do slot using radial tool orientation?

[flatout3d]

This one does output XYC, what I don't understand is why in this case the Y axis is constantly moving instead of just XC after the initially circular entry?

[flatout3d]

This one does not output any C axis code at all and has some large negative X values which I think will error out that axis limit. Not sure how to interpret this output, does it make sense to you maybe the G101 is playing a role? Checking the manual for G101 (straight line face contour generation) however the example from the manual shows an example with a simple slot across the face of a part and the output code does not output a negative X only a positive X to start with positioning above the stock dia. at C0 and then G101 C180  to produce a slot across the front face.

[flatout3d]

Yes I see that one, and have a reply below.

[Anonymous · Accepted solution]

If I post my file with radial tool orientation using Doosan post set to "Lynx", I get XC output after initial Z positioning.

If posted with Doosan post set to "Lynx with Y axis", I get XYC output because wrapping cylinder used is concentric with slot and not with C axis (main spindle centerline) and therefore post also uses Y axis option in all moves, why ?... if machine has Y axis post will take advantage of it.

If you post your file with Trace tool path where tool is in axial orientation, you get Polar mode output and by nature of that function tool will never go below C axis centerline.

I see some unfamiliar G codes in your file so I assume that is what your machine uses to activate and cancel polar mode.

[flatout3d]

Thanks for the help and ongoing dialog, it has helped me appreciate what is going on more fully. I appreciate the help and guidance you have provided