Need Advice Turning wood w/ Sherline cnc lathe

[C&Me]

Hello everyone, i am new here and seeking some advice about cnc wood turning for small parts.

I am considering the Sherline CNC lathe for making beads from exotic hardwoods. I currently use a homemade duplicator with my unimat. "http://www.youtube.com/watch?v=omQ4m0vUDLQ"]YouTube - DIY minilathe copy modification

my question is, will the sherline have enough torque to make these
pieces faster than i can manually? I realize there is a great facility
in being able to design the profiles and store them on the PC, rather
that having to hand pierce each template, but i am a bit nervous that all
of the few videos i have seen of non-professional cnc wood turning
were dreadfully slow.

The folks at the Sherline CNC forum have recommended getting the cnc-ready lathe and buying better components.

Can anyone let me know if they think i would be able to make the parts in the video faster with the sherline cnc (upgraded) than with the duplicator? Any videos that might be informative? Or other small CNC lathes that might be more capable?

thanks in advance for your advice and suggestions

justin

[Heinz Reimer]

Hi Justin
I own a Sherline 5400 lathe and a P/N 8760 driver box that I use mainly for metal, but have done some wood work as well. Spindle torque is more than adequate. The rapid moves with my setup are probably half that of your manual roughing cuts in the video. The finishing cuts look about the same. I'd expect the finish to be better with CNC due to the rigidity of the setup, perhaps saving you time on cleanup. Overall I think the times would be fairly similar. If it's of use to you, post a dimensional sketch of your part and I'll give you a closer estimate of the machining time.

I agree that you can increase the speed and performance somewhat by getting better drivers or using servos, however, the machine isn't really designed for high speed and the best you could hope for is maybe a doubling of what I have.

Regards
Heinz Reimer

[C&Me]

Heinz,

Thanks a lot for your reply, that is encouraging news. I will post a sketch of the part. Is it realistic to think i could do the sharp details with a tool on a rear tool post that would then part off the finished piece? I appreciate your help,

thanks again

justin

[LeeWay]

I think if you got a lathe large enough to put your blanks through the spindle or at least held by the jaws, you will have no trouble with these profiles. Since you wouldn't be using a tail stock, the open end would be a breeze. A threading tool would likely cut the rest as well as part off the finished part to a point.
I don't have a Sherline, but if it is more accurate with less backlash than a minilathe, I'd say go for it. Especially if you have lots of designs and need lots of parts. With the cnc, it will give you more time to do other stuff while the lathe cuts out your parts.

I think you would have less waste too if you can do through spindle holding. I don't know if the Sherline chuck can hold that though.

I also think you could build a small dedicated lathe pretty cheaply. You could even use collets to hold the work.
Take a look at this little monster here.

[Heinz Reimer]

Hello again Justin

I spent a pleasant afternoon trying this out. I assumed the units on your drawing were mm. My apologies for the poor quality video: all I had available was a cheap webcam. "http://www.youtube.com/watch?v=Wfr2lYxpJm0"]YouTube - Movie 5 The run time for the program is 88 seconds. One could probably get close to a minute with more aggressive roughing and better optimization of toolpaths.

My first tries resulted in a lot of tear out and quite a poor finish. This was with a 60 degree threading cutter, minimal rake, as is used for metal, and a continuous right to left finishing pass. So I thought back to my childhood, when I spent hours watching my father at the lathe. He was a master wood turner, a veritable human CNC machine. He worked for a furniture company before mass automation, and could turn endless duplicates by eye, with only occasional checks with the calipers. I tied to duplicate his movements and the way he held his chisels, ground a 1/8 inch HSS toolbit, mounted it with as much rake as the Sherline toolholder would allow, changed the direction of cut, and got a substantially better finish. The samples in the picture are straight off the lathe, without sanding or hand touch up. One is walnut, the other probably birch. I expect that with additional tinkering with tool angle, feed and spindle speed, it could be better yet.

The workpiece is being held in a three jaw Taig chuck with soft jaws bored out to hold ~3/4 inch round stock. This gives a large clamping surface and holds wood very securely. Mine are bored to maximum depth, though I think that for these pieces, half that distance would be enough and leave you with less waste. I"d be reluctant to use the stock Sherline chuck for wood, the clamping surface is very small and you'd risk spitting the work piece. Taig also makes a four jaw scroll chuck with soft jaws, which would allow you to start with square stock. If you do go this route, (Taig chuck on a Sherline lathe), be aware that the first few threads on the back of the chuck are cut back, and that for full engagement of the threads you need to bore about .1" of relief from the back of the chuck.

Some other details: The control software is EMC2, highly recommended. Gcode for roughing was hand written. The finishing path was traced from your sketch in Coreldraw, exported as dxf to CamBam, which converted it to gcode in the XY plane (CamBam doesn't "do" lathes); then a simple search and replace to change all Ys to Zs in text editor. Finally, a bit more hand editing such that finish cuts are always with the tool moving into the workpiece. Very circuitous, but it's what I have and doesn't take nearly as long as it may sound.

Front and back tool holders are good option on a lathe if you don't have a tool changer. You could mount a roughing tool on one side, and a finishing/parting tool on the other. You may need to modify existing tool holders or make your own to get the correct rake for wood.

Regards
HR

Out of curiosity, what are these for?

[C&Me]

Heinz,

That was very kind of you, thanks for taking the time to do that. I happen to be traveling at the moment and for some reason can't access you tube so have not yet seen the video, but the parts look great. What was the spindle RPM? Do you think it would be better with higher RPMs? I will let you know when i have seen the video. The parts are for prayer beads.

[Heinz Reimer]

Spindle RPM was 2780, which is the maximum with stock pulleys. Optional pulley sets can be purchased that will let you go to 10,000 RPM. Feed for the roughing cuts was 20 IPM, and 5 IPM for the finishing cuts. I did search briefly for information on optimal feeds and speeds for wood but didn't find much that was useful. If this was a milling operation with the wood blank a router bit of similar diameter I certainly would be using a much higher RPM. My impression was that high RPM and modest feed rates gave the best finish.

Regards
HR

[C&Me]

Hello to all,

Heinz, thanks again for your video, it convinced me to get the lathe, which i am now trying to get running. I have managed to do some simple moves, and am happy with the way it is cutting, but have hundreds of questions. I tried doing what you did with CamBam, though i am using mach3. What seemed to have happened is that when i replace the 'y's with 'z's, the original y value should be the x value. So for example if the first move in the cambam generated program is to move along the x axis 15mm and the y axis 3mm. After replacing y with z it is plain that it should be moving along, not x at 15mm but z. so the two axes are switched. I realize i have not explained this very clearly....but Can you explain what i am doing wrong?

IF you would be willing to post the code you used in the video it would be of tremendous help.

thanks again... a couple of other questions below:

Can anyone explain why the actual distance traveled along my z axis on my Sherline Cnc Lathe differs from the amount i have entered into the Mach 3 software? When I actually measure the distance it seems to come up around 3mm extra. Also, My z axis seems to jog opposite what the arrows on the keyboard indicate, while the x axis corresponds to the arrows. I am assuming that the reason for the above has something to do with the fact that the z axis moves left, towards the chuck when i enter positive values and right with negative values...is this opposite what it should be? Thanks

[Heinz Reimer]

Hi Justin
Your first step is to get your software communicating properly with your hardware. Did you get a metric lathe with the Sherline driver box or are you using something else? Step motor drivers from various manufacturers all have their own unique timing requirements, and the software needs to be configured to match. The Sherline driver can be troublesome with software other than their own because it needs step pulse durations substantially longer than what's commonly used by other manufacturers.

Lathe conventions are that +ve z moves the carriage away from the headstock, and that for a front mounted tool holder, +ve x moves the cross slide away from the workpiece. It does sound like your z is reversed. Though I'm not currently a Mach user, I do still have an installation from a few years ago when I tried the software, and the way to reverse the axis movement is : Config > Homing/Limits > check "reversed" for the z axis.

3 mm between commanded and measured movement indicates a significant problem. Common causes include:
1. The software is configured incorrectly and is sending the wrong number of steps/unit travel. (This is the only reason I can think of for measured movement greater than commanded)
2. Steps are being "missed" for a variety of reasons such as incorrect pulse timing settings, or velocity and acceleration settings that are too high
3. Mechanical binding of the slide



To check that an axis moves the commanded distance, try the following: Zero both the handwheel and the axis in software, then issue an MDI command such as g0 z5. The motor should turn exactly 5 revolutions (assuming a metric lathe) and the hand wheel should be in exactly the same position it started from. If it behaves correctly, stress the system by making it go back and forth a short distance a hundred or more times. For example run a program such as


g0 z0
g0 z5 (repeat 1st 2 lines many times)
g0 z0
m2

The carriage and hand wheel should return to the starting position.

Regards
HR

(I'll answer the other part of your question later.)

[Heinz Reimer]

Hi Justin

Here are a few files to demonstrate how you can generate lathe toolpaths using Cambam. "Beadmm.dxf" is a drawing of your part. Note that the centerline is aligned with Y, which we intend to eventually convert to Z. I suspect your problem may have been that you had the centerline aligned with X on your drawing. The origin is set such that when on the lathe, X0 will be the lathe centerline and Z0 will be next to the chuck.

"Beadmm.cb" is the Cambam file. I've divided the curve into 8 segments. (simply click and drag to select the desired segment, then select the profile tool. Do this for each segment in the order you wish them cut) The odd numbered segments are where we want the toolbit to cut as it is moving away from the headstock, and the even numbered segments are where we want it to cut as it's moving towards the headstock. If this were a milling operation, the former would be conventional milling while the latter would be climb milling. So for each of the segments, select the appropriate MillingDirection in the "Spindle Control" section. Select the feedrate, then select machining > produce gcode.

With a text editor such as notepad, open the gcode file you've just created (Beadmm1; it actually looks almost identical to the Cambam file). Delete all of the lines, in their entirety, containing a Z value. Change the G20 to G21 if you're using mm, and not inches. Change the G17 to G18 to denote that you are using the XZ, not the XY plane. There may be some other codes such as S0 (spindle speed), M3(spindle on, CW rotation), M5 (spindle stop), and M6(tool change), which don't apply to your setup. You can remove them, though they'll probably just be ignored by the control if left.

Now use edit > replace to change all of the "y"s to "z"s, and save the file. The resulting file will give you the finishing pass for your part, however, the end of each segment will be linked in a straight line to the beginning of the next, so the last bit of editing you need to do is add a line for an x retract, such as g0 x8, at the end of each segment. The resulting file is "Beadmm2".

This doesn't include any roughing cuts, but you can easily add them to your drawing and use the same procedure to generate the toolpaths.

The actual file run in the video is "cnczone4.ngc". It's not pretty, a reflection of a lot of hand editing and me learning what works with wood...

Hope this helps you get started.
HR