[Cadal]

I'm looking into a Taig cnc mill to do prototyping/ small production machining.

I'm curious how it handles arcs without a consistent radius ie: generated by bezier or vector spline in cad.
(done a lot of googling to no avail)

I'm wondering if some machines, software, etc do better in this regard, or
if in any cnc platform, nonconcentric curves must be broken down into a series of concentric ones.

Thanks and any knowledge very much appreciated
Christian

[UUU]

I would be expecting this to be a function of the CAM process, converting the drawn curve into machine movements, rather than a function of the machine itself.

I've seen G-code that is a series of very short straight-line movements, as tangents of the curve being cut. Depending on the tolerances you're working to - and the mechanical resolution of the machine itself, these should produce an acceptable result.

e.g a Taig mill producing engravings out of VCarvePro will be working in this way and the results are lovely.

[Cadal]

Thank U

The CAM to g-code process was one of the things I was thinking about.
It would stand to reason the resolution of any arc converted to short enough segments would be high.

Can anyone say if Mach 3 produces good results in this type application.

[BAMCNC.COM]

Hmm I use RhinoCam and have yet to get a smooth radius on anything, it is a lot of little straight lines, I have a Taig with .0002" or so backlash on X and .001" on Y, should I not get better cuts, or is it something I'm not understanding in Cam, or did I draw it wrong in Rhino3D?

I draw a circle, then add some straight lines going into it, then trim some of the circle out, think of a wrench, should I actually draw arcs instead? Hmm...

I use Mach3 aswell.

[LaserImage]

Hmm I use RhinoCam and have yet to get a smooth radius on anything, it is a lot of little straight lines, I have a Taig with .0002" or so backlash on X and .001" on Y, should I not get better cuts, or is it something I'm not understanding in Cam, or did I draw it wrong in Rhino3D?

I draw a circle, then add some straight lines going into it, then trim some of the circle out, think of a wrench, should I actually draw arcs instead? Hmm...

I use Mach3 aswell.

I'm inclined to think it's something in RhinoCam or your Mach setup. I use Corel Draw and/or Vcarve Pro to generate the lines/arcs/etc., and then output to Mach3. I have had no problems with smooth circles,arcs,etc.

Gary

[Cadal]

Bam:
On the drafting end, using two lines to intersect a circle and trimming should not be any different than using an arc tool. The resulting arc you get should have a specific center and radius spec.

Gary:
In Corel or Vcarve do you use spline, bezier, or similar type vector curves, or consistent radius arcs? It seems Mach3 would convert all vector cad in the same way. Thanks for the input

[BAMCNC.COM]

Hmm, my inside radius usually look very good, outside looks horrible.. I'll do some research tonight, thanks, I'm sure its RhinoCam, could be something I haven't check marked?

Would it matter if before I put my wrench through cam if I join the arcs seperately from the lines I wonder? I've been having the whole wrench outline joined into a single line(curve)

[rlockwood]

I'm looking into a Taig cnc mill to do prototyping/ small production machining.

I'm curious how it handles arcs without a consistent radius ie: generated by bezier or vector spline in cad.
(done a lot of googling to no avail)

I'm wondering if some machines, software, etc do better in this regard, or
if in any cnc platform, nonconcentric curves must be broken down into a series of concentric ones.

Thanks and any knowledge very much appreciated
Christian

Splines must be exploded into arcs/lines. Most cad/cam software will have some sort of "Arc-Fit" function to handle this, with a maximum deviation tolerance. Others will explode to lines, which causes some level of faceting (think disco-ball). If your software only explodes to lines, you will have a trade off to make, and your NC controller will come into this equation. Too few facets and your part looks ugly. Too fine of facets and your controller can "data starve" (meaning it wont be able to process the lines fast enough to achieve the desired feedrate). With modern controllers (even pc based ones) there is a balance in between that is acceptable in both regards.

In either scenario, the issue wont be directly related to your taig, as these issues will be the same with any PC based controller-- regardless of what machine its connected to. Many machine controllers are marketed as "high speed", and this is in reference to the data starving condition.


Another thing to consider, however, is that most 3D tool paths are broken up largely into small straight line (g1) moves, as g-code only inherently supports arcs (g2/g3) on one of the three cartesian planes (XY, XZ, YZ, g17-19 respectively). Arcs can be spread evenly over a distance in the "other" direction of the plane, but are defined purely by a radius and start and end coordinates.

[UUU]

I visited a shop last night where their Taig had just finished making some small oval brass plates - table numbers for a restaurant. So I had a look at the G-code to see how long the straight segements were, that made up the oval. this code would have been generated with V-carve. The three steps I picked had lengths of 0.899mm, 0.845mm and 0.870mm, if my pythagorous is correct (even if my spelling of it is not).

The Taig in question is not new - and is set up at 314.96 steps per unit - it may be that the drivers are full or half step, I don't know the leadscrew pitch to tell.

[Cadal]

Splines must be exploded into arcs/lines. Most cad/cam software will have some sort of "Arc-Fit" function to handle this, with a maximum deviation tolerance. Others will explode to lines, which causes some level of faceting (think disco-ball). If your software only explodes to lines, you will have a trade off to make, and your NC controller will come into this equation. Too few facets and your part looks ugly. Too fine of facets and your controller can "data starve" (meaning it wont be able to process the lines fast enough to achieve the desired feedrate). With modern controllers (even pc based ones) there is a balance in between that is acceptable in both regards.

In either scenario, the issue wont be directly related to your taig, as these issues will be the same with any PC based controller-- regardless of what machine its connected to. Many machine controllers are marketed as "high speed", and this is in reference to the data starving condition.


Another thing to consider, however, is that most 3D tool paths are broken up largely into small straight line (g1) moves, as g-code only inherently supports arcs (g2/g3) on one of the three cartesian planes (XY, XZ, YZ, g17-19 respectively). Arcs can be spread evenly over a distance in the "other" direction of the plane, but are defined purely by a radius and start and end coordinates.

Rlock thanks that helps!

I see how this is basically a software issue and more specifically how arcs are converted to g code. The description of the Curve and Arc fitting function on the Vcarve features page explains it as you did.

I also see how various g-code programs may approach things a little differently ie: geared more toward mechanical parts or signs/carving.
Also that program can represent a sizable investment.

There's probably some discussions I should look into regarding pro/con of g-code programs - any help appreciated

Christian

[BAMCNC.COM]

I fixed my issue in RhinoCAM aswell, It's in preferences, makes arcs linear paths or something, just un check it.

[UUU]

I tried engraving some text from CamBam for the first time today. Most of the curves were rendered as a series of short arcs. A sucessful oucome.