I am not sure this is the best place to post this… so admins please feel free to move it if it is better suited elsewhere.
I purchased the PwnCNC rotary attachment for my 1F Elite Foreman last year. I am finally getting around to learning how to use it.
One of the services I offer in my woodworking business is spindle reproduction. So, for example, someone has a stair railing, and it’s missing or has broken spindles that can’t be purchased anymore, I will duplicate turn them. Until now I have done this using a traditional lathe, but I would love to be able to use the CNC to do it, especially when I only need to make one or a few. Particularly with spindles that have small diameters and / or smaller more intricate details on them.
I have spent the last few days experimenting with the first such job, and am looking for guidance / advice from anyone with experience in this area regarding the following:
The best way to get the profile into the CAD / CAM. I currently use Vectric Aspire. I tried taking a photograph of the original spindle, using a trick from my crime scene tech days. I placed a ruler in the photo. I imported the photo into the software, placed two guidelines 1 inch apart, and then enlarged the photo until 1 inch on the ruler was on the guidelines. I figured that would get the scale correct. I then did a bitmap trace and was able get what appeared to be a good profile, after some node editing of course. I assigned a molding toolpath to it, and sent it to the CNC using a tapered ball nose bit. The result was still not to correct scale. I think part of the issue, or maybe the whole issue, is the parallax error from the camera?? The left and right ends of the spindle in the photo are farther away from and off at an angle from the lens… thereby introducing error when I do the trace? Next I am going to try tracing the profile onto paper with a scribe, and using the Shaper Trace to get it into a vector.
Speed. It took the machine almost 11hrs to carve 11 inches of spindle. Obviously, this is pretty impractical. I was able to significantly reduce the rounding toolpath time using a technique I found over on the Vectric forums, where you use the spiral gadget to do a continuous rotary movement in conjunction with a continuous X-axis movement. But I cannot seem to figure out how to apply that to the molding toolpath. Would I be better off with a two-rail sweep? Any suggestions on how I can speed up the carve time? I’ve seen videos of CNC’s doing continuous rotary carves and the rotary is turning much faster. Is that possible with my setup? Also, I did try adding a large area clearance toolpath but according to the software it only added more time to the carve.
It sounds like your on the right track with tracing the form. Another alternative to your method might be measuring with a caliper to quantify it. Theres limitations in vectric without having a hardline to trace.
I have a couple of recommendations, but none will be faster than doing a spindle on a lathe.
First, I’m Y wrapped around X (vectric wraps an axis around another axis and you can do Y wrapped around X or X wrapped around Y) so mine is parallel to the X axis.
It’s good you found the rounding tool path.
Instead of having the rotary rotate and have the spindle increment, i think maybe have the axis go left and right and having the rotary motor increment.
After that, things like step over & bit diameter, and feed rate have the greatest influence, and i would suggest bumping them up. Depending on the depth below the rounding tool path after the first pass its only shaving as it goes.
I don’t think that’s possible with vetric. They have the rotary range 0 to 360 back to 0.
Other cad software might be able to do more, but i haven’t looked.
Again i would rather increment the rotations and travel along the X axis moving left and right rather than rotate and increment the X axis
In summary, take a picture with a white background and a size reference. Upload it to gemini.google give it a prompt e.g. give me a silhouette of this picture… You get a png. I them used Adobe Express to convert that to SVG. All for free (for now).
I haven’t done any cutting on my rotary yet so can’t really help there.
To add to this: you want to be as far away from the object you’re photographing as possible to remove any lens distortion and as much parallax as possible. Depending on your phone, you may be able to correct for that in software on device, but it might be better to add additional references around the spindle and correct for lens distortion in photo editing software.
Placing the ruler at the midline of the part may also help, and a full grid around the part would be even better. By midline, I mean with a 1” spindle resting parallel to the floor, place the ruler so the scale of the ruler is 1/2” off the floor. Ideally the ruler is longer than the part so you can correct any errors along the whole length of the part
Fusion’s CAM will allow you to rotate forever and ever, but you’ll probably want to swap in g-code to tell the rotary to go back to 0 the fastest way possible, otherwise it will “unwind” for as long as it took to “wind up”.
Great idea for using a CNC rotary. Another option might be to use one of the many brands and styles of contour gauges to capture the profile. You would likely need to take multiple profile readings and then piece them together.
Also, instead of photographing items for tracing later in CAD, I have found that using a flatbed document scanner is much easier than trying to position a camera at the correct distance and perfectly planar alignment. As long as the item fits within the X and Y dimensions of the scanner bed and is not too tall, this method works very well. If the part is slightly too tall, you can sometimes leave the lid up and drape a piece of fabric, white or black, over the item to help improve the scan.
By design, images produced by a flatbed scanner maintain a consistent 1:1 aspect ratio. When I first started using this method, I included a machinist ruler in the scan for reference, but the dimensional variance was barely noticeable, if at all.
Thank you Chris. Yes, I fully agree it will never be anywhere near as fast as turning on a lathe, but if I could get it even to maybe three or four hours for a spindle, I would be happy with that. Again, I’m looking to have this capability only for those spindles having more than usual fine detail, asymmetrical, etc., that just are more difficult / time consuming to do (or can’t be done) on the lathe.
I also have my rotary set parallel to the X axis, but when I assigned the molding toolpath and sent the code over, it automatically did it by indexing the X movement and turning the rotary in full 360 moves back and forth. I agree it makes more sense to index the rotary and have the X sweep continuously back and forth… how would I change that?
Having said that… Vectric does appear capable of continuous rotary turning while the X sweeps the profile, as stated I did it on the rounding using the spiral wrapping gadget. This method appears to be even faster yet, based on what I have seen. I think maybe I need to use a two rail sweep to get it to work, as opposed to a molding toolpath.
Thank you all for the responses. After MUCH trial and error… photographing, scanning, tracing… I have finally had success by using a compass scribe with the tip bent outward to 90 degrees. I placed the spindle on a piece of paper and scribed the profile onto the paper using the compass. Then I used the Shaper Trace to photograph the trace, import it into Aspire, and with just a couple of minutes of node editing to tune things up, I had a near perfect and to scale profile vector. I did have to do it in two halves, and then bring them back together in Aspire. Now if I can just figure out how to get around it taking all day and night to carve…
Also, I now find myself looking into 3D scanners. Does it ever end? LOL.
Once again… thanks Chris! So yes the whole key is I need to be doing this with the 3D toolpaths as opposed to the molding toolpath, which does not give me those options.
Can also think of alternative ways to do something… like for example if your fluting, try a single line with a 1/2" bowl nose bit, then use a profile toolpath with project onto 3d tool path selected and your selected depth. Vectric does rotary by flattening out the tool path (which is why it can’t carve below the mid point) so if you only want sections done with a fine bit i would draw a vector around it then set the finishing tool path to the selected vector(s). It’s a little teadious to learn, but me doing the chess set, well i learned a lot doing it.
I’ve never messed with the moulding toolpath. I read the docs on it, and said to myself i don’t see me needing that.
Final Update: So I was ultimately able to get the rotary to do a continuous rotary carve on the entire spindle length, using Milo Scott’s method. I ran the 1/32” TBN at about 800ipm, and the entire carve completed in under three hours, including the IDC 1/8” Badger roughing pass. Here is a link to a YT short I made, showing the process and there is some footage of the machine carving:
Here are some things I learned the hard way:
I attempted to make a roughing pass with the IDC 1/4” Beast bit, and that was a mistake.
I was concerned about spindle whip with this particular spindle, because the diameter gets pretty small at some points. That was a big part of the reason I wanted to do it on the CNC, because I don’t have a steady rest for my lathe yet. What I found was that instead of whip, you get vibration on the CNC… sort of a harmonic vibration that travels through the spindle and into the head / tail stocks. I made a steady rest of sorts, using a couple of skateboard wheels, that attaches to the T track on my spoil board. That solved that problem. Eventually I plan to do a long form YT video which will show that as well.
I attempted to make a roughing pass with the IDC 1/4” Beast bit, and that was a mistake. Again, because the spindle gets thin, I found that the bit was so aggressive it would flex (pull) the spindle up as it passed over, so much that it was readily apparent just with the naked eye. I assume switching to a down cut bit would cause the same problem in reverse. Perhaps it would have worked OK on a larger diameter spindle. But for this one, I switched to the 1/8” Badger and that worked much better.
I came across a document in a couple different threads over on the Vectric forums, written by Milo Scott. It explains how to use the wrapping gadget, spiral layout tool, to induce the continuous rotary rounding toolpath. I applied that same method to the 3d spindle profile, using the TBN bit in a 2D profile toolpath, start and cut depths set to zero, machine ‘on’ vector, and checking the ‘project toolpath onto 3D model’ option.
I have the document in PDF format but can’t seem to figure out how to attach it here. Let me know if you would like me to get it to you some other way.
