Arcs and Stepping question?

[CRWConstruction]

I'm new to working with CAMs but one thing I'm wondering is I noticed that with Visualmill, RhinoCAM and a few others that arcs and circles are all produced with stepping a bunch of straightaways. Is there a cam program that will create a real arc as it's toolpath or a way to make the CAMs I mentioned, use true arcs? The sales rep for the CNC machine we have told us before purchasing that the machine could make true arcs and not stepping like most others...but seems all the CAMs force it to use stepping as far as I've seen. Any suggestions?

[jemmyell]

Hi,

Most CAM programs will generate ARCs if they are present in the input artwork. It is probably the DXF file you are using. For CorelDRAW, use the DXFTool from CandCNC to generate a DXF with real ARCs and then use SheetCAM to make your GCODE.

-James

[ger21]

As James said, either you CAD drawing is drawn with line segments, or you're missing a setting in your CAM program. All the CAM programs you mentioned should cut regular G2/G3 arcs.

[CRWConstruction]

Don't know I've been using Rhinoceros 4.0 for designing all files so far and that produces arcs when the circle or arc tools are used but when I use RhinoCAM or import file into Visualmill or other CAMs to produce a G-code comes out with stepped toolpaths. You mentioned could be missing a setting, any idea what setting that would be? I've been scouring the file and operation settings since yesterday evening and can't find anything.

[RandK]

In VM5.0 it is in preferences>machining preferences. UNCHECK the 3 boxes that make it use linear segments (lines) for arcs.

[Hirudin]

I noticed the same thing CRWConstruction and also started my own topic... oops.

After you try changing the settings RandK mentioned please let me/us know whether it worked.

[etzz]

I too noticed the same thing with Rhino4.0 and Madcam. Ive just been using the software for a couple of days. I was about to post a question, but found this post. I havent investigated yet, but just noticed the circles were made of segments. I was wondering if mach3 would still drive the machine as a continous arc. Will post if I learn anything.
Regards,
Eric

[etzz]

Pasted below is what the developer of MAdcam (Joakim) replied to the same question in the MAdcam forum. I tried the suggestions and did see improvement, but there are still miniature line sigments. I checked the G-code, and there are no G2/G3 just smaller straight line moves (from what I can tell...I'm also new to this). So maybe to get perfect arcs for this sofware I would have to mod the G-code. Not sure if it would really matter much anyways (?).
Regards,
Eric


*************
There are two things to check.

1) The mesh tolerance in Rhino.
If the model is shaded when you select surfaces for toolpathing, madCAM use the Rhino render mesh. To control this, please select Rhino options/mesh. The settings should be something like this for inch (custom settings, maximum dist edge to surface = 0.001, Refine mesh and Jagged seams) for mm it should be (custom settings, maximum dist edge to surface = 0.01, Refine mesh and Jagged seams). If the model isn’t shaded, madCAM will calculate the mesh and use the tolerance set from madCAM options. I would recommend to always having the model shaded when selecting for toolpaths calculation. This way is faster and if setting the flat shaded view option in Rhino, you will get what you see. Please also have a look in the madCAM help-file/select-model.

2) The tolerance set for the cutter.
It is also a tolerance set for each cutter and this tolerance is used when calculating the toolpath. Smaller tolerance will give a smoother toolpath.

If still having trouble, you are welcome to send me the model and I will have a look and create some sample toolpaths and send it back together with settings.
************************

[etzz]

After some reading, the whole G2/G3 (circular interp) -vs- G0/G1 moves (tiny straight lines) is sort of tied to the machine controller (mach3 in my case) and its implementation of CV motion (constant velocity). CV motion tends to remove sharp corners in motion. So with CV enabled, you should get smooth motion and a decent finish anyway. A short blurb pasted from a mach3 doc:

http://www.machsupport.com/docs/Mach3_CVSettings_v2.pdf

**********************
Constant Velocity “CV” – This mode attempts to maintain a constant velocity during
ALL angular or arc moves while obeying the acceleration parameter. This is not possible
during some moves...such as single axis moves that change direction (i.e. Motion must
stop at some point during these moves). On moves where constant velocity can be
maintained, the corners will be rounded depending on how high the acceleration is set
combined with the CV Distance Tolerance (see below) . Higher accelerations and
smaller CV Distance Tolerance values will result in tighter corners and lower following
errors. Note, this is NOT the same as servo following error and has nothing to do with
PID control. Servo/Stepper following errors will be slightly WORSE than the CV
induced following error depending on how “tight” the servo loop is. Stepper motors will
lag as well (+- 1 full step), and will lose steps if pushed too far (VERY BAD).

Exact Stop – This mode accelerates and decelerates to each “point” in the gcode. Mach-3
only sees one move at a time and usually machines run somewhat rough and very slowly
in this mode. Exact stop should only be used where a machine must not round any
corners (inside or outside). However, remember that most CAM software will output
many tiny G01 moves to form arcs. In exact stop mode this type of movement will leave
very bad surface finishes and can be hard on tooling and machine components.
*************

[RandK]

The OP was asking about 2.5d work and getting interpolation of arcs/circles. The VM settings should fix that. Note that there is also a setting in the circle tab of the post configuration that can be set to segment circles (ie 180 degrees) if the controller needs that. That should make it use multiple G02/3.

In 3d solids/mesh work most CAMs do interpolation of the surface using G01's based on accuracy settings in the software. Higher accuracy means more short lines and code. I haven't set up VM since a computer change but I checked some old programs and they were all G01's for surfacing. I don't know about madcam.

[ger21]

Originally Posted by etzz After some reading, the whole G2/G3 (circular interp) -vs- G0/G1 moves (tiny straight lines) is sort of tied to the machine controller (mach3 in my case) and its implementation of CV motion (constant velocity).

Sort of, but not really. Cutting a circle with a series of straight segments will not cut the same as one using G2/G3. When using G2/G3, the cutter will stay on the path. If you're using straight segments and CV mode, Mach3 may clip the corners of your straight segments. This can vary greatly with acceleration and velocity settings. The smaller the segments, the closer it'll be, but G2/G3 is far better. Another reason that G2/G3 is better, is because the machine should run smoother making the continuous arc, rather than the series of short segments. Even with CV mode on, Mach may not be able to maintain the same velocity and smoothness of the G2/G3 moves.

As the previous poster said, if you're using 2D drawings from Rhino, you should be getting G2's and G3's. But if your working with a 3D model, it's normal to have all G1's.