Cutting 'real' curves

[barrys]

OK, so I'm new to all of this but I've been woodworking for a while and have been a computer geek for way too long. So, in talking to my dorky friends, this issue came up:

Dorky Friend: So, when you create an image for submission to a cutting program, is it a polygon mesh or a NURBS surface.

Me (moron): Um, it's a NURBS surface in the CAD program but I export it as a polygon mesh for consumption by the toolpath generator program (MillWizard in this case).

Friend: Well, polygons, by definition are made up from little line segments. Won't you loose all of your nice real curve definitions?

Me: Hmmm. I think the polygon resolution is fine enough to make all the curves look natural.

Friend: Well, these things are like plotters, right? A plotter can draw a perfect circle which is what makes them so cool.

Me: Yup. The drive screws of the machine can do that too. Maybe the toolpath programs interpolate the polygon mesh curves back into smooth curves but I'm not sure. etc. etc.

So, what do all of you gurus think? I'm guessing that the more I'm willing to spend on software, the more smooth my curves will be. I've also heard of some of these machines advertizing "true ISO curves" or something like that.

Please respond if insomnia or boredom are getting the better of you...

Thanks,
barry

[richards]

Forget the software for a moment and think in terms of the machine. The X-axis direction is always 90 degrees from the Y-axis direction. Either axis moves in finite steps; therefore, at the machine, everything ends up as small straight lines.

In my opinion, no matter which software program you choose to use, you still have to deal with the basic functionality of the machine. Even if the software can compute a perfect curve, the machine can only move in two directions (forget the z-axis for this example). The smallest move is one step in either the x direction or the y direction. If both the x-axis and the y-axis are commanded to move at the same time, then the actual move is a very small 45-degree cut. So, in actual practice, the cut will always be a straight line, either on the x-axis, the y-axis or at an angle to the x or y axis.

If you cut a very small circle, the x-axis vs the y-axis movement may become a factor; however, remember, we're dealing with a machine, a cutter, and the medium (wood, metal, plastic, etc.) that we're cutting. The actual part being cut may exibit a smoother or rougher cut than the program called for.

[gerald_d]

In addition to what Michael said, think about the actual cutting bit and the shape of the groove that it will be cutting. There comes a point when you:
- stop programming, changing bits, and letting the machine run for hours to remove hardly any material
- and when you decide to grab a piece of sandpaper and take off the last ridges "manually"

With complex shapes cut by a router, you can never eliminate the "manual" finishing step, despite what the salespeople of toolpath software try and tell you.

[ron brown]

Barry,

One can designate the toolpath in most CAD programs. This would eliminate any "Polygon mesh" problems that might occur. Any inconsistancies caused by the "Whiz-Turd" magical toolpath software would be eliminated. One can also design toolpaths where the bit "stays loaded" - that is not comming in and out of the material. This is probably a larger factor in smoothness on most CNC machines than the segmented mesh "El Geeko" might dream up.

Some will say, "The secret is in the software." I will contend the secret is in KNOWING how to use your software. Some want software that will do all but cleanup after they use toilet and do it with one click and no thinking (not that they had though to engage their minds befor this time). Others understand a proper toolpath can be more efficient and faster running than those designed by all but the most expensive CAM programs and can be fairly reasonable.

I use RHINO and VECTOR. I do very little carving. BUT, I can do work like that using those two programs. I've thought about getting a copy of TurboCAD and seeing if I could do the same things in TurboCAD as I can in RHINO. I have exported toolpaths from RHINO to the ShopBot DXF converter and watched the toolpath in the V3 previewer. It seems to work well. TurboCAD off Ebay and the DXF converter would be a less than $100 solution to complex toolpath writing. But it will be time intensive on the screen and to learn.

Ron

[hespj]

Barry S

I'm not a SB user yet (I'm scratching together the extra funds needed to buy an Alpha), but I have experience (some bitter) of getting CAD drawn parts CNCed.

If I understand you correctly, aside from the question of the machines resolution, you are concerned that using a polyline or polygon mesh will produce a faceted cut or surface rather than the originally drawn smooth curve. For instance a hemishere might be cut looking like a geodesic dome rather than the smooth hemishere originally drawn in the CAD program. I have certainly had this happen when getting parts CNCed - the laser cutter we use tells us to send polylines as they can't use splines. As a result we sometimes get cut parts which are more faceted than they appeared on the computer screen.

The trick is to use polylines/polygon meshes with more vertices than you thought you'd need. It also helps to print out the curve and eye along it to check for smoothness - faceting is going to show up on the cut part much more easily than on the computer screen.

Also, if one cut part is to fit neatly inside another (for instance a letter "S" fitting inside a letter "S" shaped hole), make sure you use the same polyline for both parts so that the vertices are in the same place on the "S", and on the "S" shaped hole.

[ron brown]

John,

There are a lot of options when trying to get "smooth" lines and curves. That is one of the "Tricks" of actually KNOWING what your software is doing. really curved stuff might need to be converted first to lines with a lot of "points" then using the points to make short arcs. I have actually used arcs to smooth an area and forgotten to build all the related curves the same way..oops. Fortunately, a little sandpaper and it was not noticeable. Except, I always run my hand over that carved piece and can feel the minute "facets" each time I see it.

One of the most common missconceptions is the more points a curve has the smoother it will be. Just the opposite is actually the truth. The fewer points one can use to model a curve, the smoother the curve and the resulting surface will be.

The amazing thing is few others know there are imperfections in projects one does. I know I seldom tell anyone when I screw things up - except if someone is there who will benefit from my solution.


Ron

[chamcook]

Another factor which affects the smoothness of arc moves is the circle arc resolution setting in the control software. The default setting of .050 (which after all is just under 1/16 of an inch) leaves a noticeably faceted appearance to the 3/8 inch radius inside corner arcs in many of my yacht interior door frames.
This setting can be found in the Values-Units dialog. The finest setting is .005 but this causes my machine to choke on the long top arch curves which are also represented as single arcs. I suppose that this is caused by some sort of memory issue. I'm a little hazy on that.
A setting of .01 seems to be a good compromise for me. This became an issue when it was taking more time to sand machine marks out of frames that were cut on the ShopBot than frames that were still being done with a hand router following a template. The finer setting setting makes a big difference in smoothness of these inside corners. I am refering here to arcs that are represented by single lines in the CAD program and single CG commands in the ShopBot file.

[hespj]

Ron:

" really curved stuff might need to be converted first to lines with a lot of "points" then using the points to make short arcs."

This is a good idea. Why didn't I think of that. I must try it. It's got to be smoother than lines.

"One of the most common missconceptions is the more points a curve has the smoother it will be. Just the opposite is actually the truth. The fewer points one can use to model a curve, the smoother the curve and the resulting surface will be."

I would rather say "The fewer points one can use to model a curve, the FAIRER the curve and the resulting surface will be." although I can see that if the arc method you suggest is used, it will also result in a smooth curve. The trouble with using the minimum number of points is that when the curve is converted to lines it will be neither smooth nor accurate; and if converted to arcs, it will be smooth, but not accurate.

I find the best bet is to model the curve (or surface) with the minimum number of control points to ensure fairness, and then convert it to a polyline (or mesh) with a large number of points (or surfaces) to minimise faceting and to closely follow the original curve.

This works for me, but as I said, I havn't got a ShopBot yet, so don't know how it translates to SB. A few suprises in store no doubt.

David:

" The default setting of .050 (which after all is just under 1/16 of an inch) leaves a noticeably faceted appearance to the 3/8 inch radius inside corner arcs in many of my yacht interior door frames."

As I say, I've no experience of SB yet, but does the dia of the cutter make a difference here, with larger diameters producing smoother work. In fact I'd have thought 3/8" rad cutter would give a very good 3/8 rad corner. Or am I missing something?

John

[ron brown]

"The fewer points one can use to model a curve, the FAIRER the curve and the resulting surface will be."... well, fair might have been a better - and the correct choice of words... and it will need to be converted to arcs after it is "faired".

Davis's problem is interesting....

Ron

[artisan]

As one of the one's Ron is probably referring to as far as the "secret's in the software" comment, I have to say that I still believe in this largely. I can still cut time from my work far faster with a clean design than with a tooling strategy. Getting a model as "clean" as possible has become the holy grail for me. However, I have lately begun to turn my attention more to tooling strategies as a compliment to this process.

There is no pushbutton answer to most problems. I am surrounded by $100,000 (gerber) to $200,000 (onsrud) machines within 5 miles of my shop. They run high end software that makes many decisions very nearly pushbutton. However, I still cut their unusual and non standard dimensional pieces here in my shop with the Shopbot. It's more noisy and less sexy than those other marvelous machines (I have to manually change my bits), but it is nice "Knowing" that that solid software strategies and good tooling strategies are still at least as important as the machine....D

[mrdovey]

For me, it's been an interesting learning experience that's led me to write an ever-increasing number of DOS modules that produce temporary SBP files "on the fly" that are executed immediately after generation and then deleted.

Some of the things this has made possible have been [1] specification of a maximum error tolerance for curves, [2] generation of the minimum number of tool moves to satisfy that maximum error tolerance, [3] huge reduction of SBP file space requirements, [4] production of code that adapts to the current cutting tool, and [5] the ability to perform calculations to the highest precision available from the PC's floating-point processor which is much more precise than the precision available from the normal ShopBot software.

The downside (there's always a downside) is that I need to add another step to the part program development process that follows the FC (conversion from DXF to SBP) step to replace sections of FC-generated code with "calls" to the DOS modules.

The upside is that when I specify a (runtime) maximum error value of, say, 0.0010" for curve generation, there's no visible evidence of faceting.

So far I've only needed DOS modules for elliptical arcs, sine and ogee curve segments, and bessier curve segments; although I have been writing a few modules to "macro-ize" some standard joinery operations. [Ron: The locking lap joint is one of these, since it needs to adapt to the thicknesses and widths of both members, as well as to the current tool diameter]

Morris

[chamcook]

John,
A 3/8 radius cutter would give a perfect 3/8 radius corner.
I am using a 1/2" compression spiral to give a good top and bottom edge.With this cutter a 3/8"radius inside corner at .050 resolution leaves the aforementioned facets. I could have designed these parts with a 1/4" inside radius to fit the radius of the bit exactly but went with 3/8 to keep the bit moving. Having the inside radius the same as the radius of the bit would cause the bit to stall momentarily in the corners which I was afraid might cause heat buildup and burn marks. This is all the more likely since on this machine I have to run the finish pass pretty slow to prevent 'bouncing' and leaving little dimples in the corners even with the 3/8 radius. This machine has two Z's with one of them being a Columbo Spindle (ie a lot of weight) so you have to be carefull not to go charging into the corners. I rough out at 2.5 ips and slow down to 1 ips for the finish pass.You can see the nice shavings from the roughing passes turning into dust on the finish pass and can 'feel the warmth' if you scoop some up with your hand. My PR machine with a single Porter Cable Z is not as succeptible to bouncing if you go into corners fast.
This is all part of the learning curve. I first thought the marks in the corners were due to bit chatter caused by the climb cut strategy. When I noticed that the marks from deeper and deeper roughing cuts always lined up I began suspecting dirt on the rails and bearings (which I still consider to be a concern). Now I'm on to circle arc resloution and fine tuning the speed of cut.
It is a pretty small detail butI feel that by playing with all these parameters I am putting out better parts.