Turning with 4th axis

[dsnellen]

I would suggest that Andy simplify 4th axis MOP. Rewrite the procedure to do something like I mentioned above. Draw the profile on the XY view. Set workplace top at radius, select the lathe machining option. This option converts the Y profile to an Z movement. Need a field to determine value used to rotate object 360'. On mine, because of gearing, an A=3 is a 360 rotation. Other fields are already present (step over, tool, etc).

Actually, CamBam already does this with a 3D profile cut. For a given Y, it varies Z based on X. With Y = 0.00, select an A value that give a 40% +/- step over and move X while A rotates under the cutter. Z then cuts profile. For example, a 20% step over of a 0.25" bit is 0.05" per rotation or 20 rotations for each inch. A complex profile is really nothing more than repeated 3D movements on a constant Y axis. A true 4th axis MOP would be easy to develop considering 99.99%+ of the code is already in CamBam.
Dave

[Bubba]

"This option converts the Y profile to an Z movement. Need a field to determine value used to rotate object 360'. On mine, because of gearing, an A=3 is a 360 rotation. Other fields are already present (step over, tool, etc)."

See, yours A-3 =360, mine A-3=3 units (3DEG of rotation), others? Anyway, the control software I'm using Mach in my case does the translation of rotation per unit (mm, Inch, DEG )

And yes! It would be nice to have a rotational MOP.

[kvom]

Machining the profile on the Z axis requires a ball endmill and yields a scalloped facet whose width is constant based on the endmill diameter.  The DOC is also likely to be limited according to the material as ballnose cutters don't like deep passes.   

Milling with the Y axis as in this case allows a straight endmill to cut with the side flutes and yields a flat facet whose width is dependent on the DOC.  Two different cases.

[dsnellen]

Machining the profile on the Z axis requires a ball endmill and yields a scalloped facet whose width is constant based on the endmill diameter.  The DOC is also likely to be limited according to the material as ballnose cutters don't like deep passes.   
<snip>

Not true. Z axis milling does not require a ball endmill. You can any cutter shape you want consistent with desired pattern. I often use a round or cove 1/4" or 1/2" cutter depending on the slope I want and X distance to cut it. Use a V or butterfly bit for a twisted rope type pattern. A bowl cutting bit or large endmill is great for a long taper often found on furniture legs. I often use an 1" endmill because it gives me the desired pattern or for rough shaping. It's a matter of coordinating A with X and Z with the cutter shape to achieve the end result. Exactly the same as with 3D profiling. DOC is not limited. Since you are concurrently cutting both sides of a rotating stock, a .125" depth is equal to a 0.25" reduction in diameter in one pass.

It may be a "six of one, half dozen of another" discussion. I just see side milling to make an object round as being a backwards way of approaching the problem. In the OPs video, the piece could have been made in 2 or 3 passes. That's all.

Dave

[kvom]

My post was assuming CB will not generate rotation moves simultaneously with X/Z.  A flat endmill cutting a profile like this using only Z and X moves on the centerline doesn't seem as if it would work properly.

In retrospect, the roughing pass in the original video  isn't necessary as far as I can tell.

[dsnellen]

My post was assuming CB will not generate rotation moves simultaneously with X/Z.  A flat endmill cutting a profile like this using only Z and X moves on the centerline doesn't seem as if it would work properly.

In retrospect, the roughing pass in the original video  isn't necessary as far as I can tell.

Correct. A axis moves simultaneously with X/Z.

[Rushwind]

I have been wondering, since the Y axis doesn't move during the MOP, couldn't you figure out how to model this as a 3-axis MOP? That is, set up Mach3 (or whatever control software) to treat "the rotation axis" as Y, so when it sees "G1 Y1", it rotates the rotation axis 1 inch (or one full rotation) around the original diameter of the workpiece. Treat X and Z as normal.

Then it would come down to drawing the part properly in CamBam to reflect this (I assume it would look like the extruded/unwrapped version of itself).

With this type of behavior, you could do some really intricate "indexed lathe" work, like cutting a totem pole. The G-code would just cause Mach3 to move the rotation axis to and fro instead of causing the Y axis to move back and forth.

I wondered about the different radii as the workpiece gets narrower, but I think there's a G-code to compensate for depth (Maybe G64?)...

Seems like it would be worth a couple pieces of scrap wood to try it out, for someone who already had a 4th axis up and running.

Any reason why this sort of thing wouldn't work?

[Bubba]

As I play with the rotational axis more and more, I have concluded there is simple way to do almost any thing using CB to design the "flat Pattern", wrap it in cheap program $20.00 "CNC Wrapper" and cut it on either dedicated 4th axis drive(my case) or plug the rotational drive in place of your either Y or X drive, align properly and it should give right results. Remembering the your drives you going to swap out have the same characteristics, ie the same amount of movement and direction of a swapped drive, did that and it was a pain so I use a dedicated setup. Once configured and tuned is there available any time is need it, don't need to worry about swapping cables and reconfiguring, unless you are using stout motors and drive the 4th axis straight up, no need to worry about it. My diy 4thdrive is worm gear driven 10:1 ratio, so even thou I'm using the same motors on all my drives the fine tuning is different. Sure be nice to own a true $axis cam, but as hobby I'm not prepared to spend upward of $800.00 for program, so I just watch the Z axis is exercised...  

[dsnellen]

I have been wondering, since the Y axis doesn't move during the MOP, couldn't you figure out how to model this as a 3-axis MOP? That is, set up Mach3 (or whatever control software) to treat "the rotation axis" as Y, so when it sees "G1 Y1", it rotates the rotation axis 1 inch (or one full rotation) around the original diameter of the workpiece. Treat X and Z as normal.

Then it would come down to drawing the part properly in CamBam to reflect this (I assume it would look like the extruded/unwrapped version of itself).

With this type of behavior, you could do some really intricate "indexed lathe" work, like cutting a totem pole. The G-code would just cause Mach3 to move the rotation axis to and fro instead of causing the Y axis to move back and forth.

I wondered about the different radii as the workpiece gets narrower, but I think there's a G-code to compensate for depth (Maybe G64?)...

Seems like it would be worth a couple pieces of scrap wood to try it out, for someone who already had a 4th axis up and running.

Any reason why this sort of thing wouldn't work?

This probably wouldn't work. The Y axis movement would need to be less the the circumstance of the stock. A program to do this already exists. I think its name is cncwrapper. It is used to wrap designs around an object. It treats a circular object as if it were a flat object. It also assumes there is a 1 to 1 correlation between Y and A. This is different from cutting a typical chair leg where a combination of flukes, discs, rope and tapers are more the norm.

[dsnellen]

I finally got a chance to play some. The idea was to take a couple of shapes and cut them using the A axis. First I created a ball shape and another shape with sloping curves leading to a round over top. Used CamBam lathe to create the gcode. I then wrote a Perl post processor program to covert the gcode into something I could use. It makes the finish pass a subroutine and inserts code to call the subroutine x times with a varying Z height offset variable. It also changes all Xs to Zs and Zs to Xs so the gcode with work with Mach3 mill. Also inserts the appropriate A statement with the X statement. It actually works quite well. Not really efficient as it cuts a lot of air but I am encouraged. Attached a couple of pictures.

Mach3Turn doesn't work for me. First, can't get it to activate the motors. Second, I don't understand it. Third, I have an 4'x8' foot mill with a 6" swing A axis NOT a lathe with a sideways tool holder with attached work table and finally why make things hard. Most CNC mills have vertical cutters, so why can't we have software (CamBam) that looks at a lathe the same way. Its nothing more than 3D cutting while maintaining a constant Y axis. What's so hard about that?

Dave