View Full Version : why can't I v-carve circles with z axis only

01-07-2010, 05:25 PM
hi, i'm trying out RhinoCAM 1.0. I have a pattern of small circles (1/8" - 1/4") that I want to engrave.

When I create the 2-1/2 axis MOp using a v-carve bit, rhinCAM has the bit plunge and then follow a small circular path in the x/y plane. Is it possible to just make it plunge and come up (moving only in the z axis)? My bit is wide enough, and my cut level is deep enough to make this possible. Maybe I'm just missing an option.

01-07-2010, 09:03 PM
Unless I am misunderstanding you, the operation you are describing is drilling, not v-carving.


01-08-2010, 12:28 PM
Maybe drilling is the better word. Basically I have hundreds of circles that are all different sizes - and very few are exactly the same. They form an image, and I want to recreate that image on a painted wooden board by cutting through the paint where the circles are.

I thing the best method is to use a v-carving bit and just have it plunge straight down, going lower for the wider circles, etc. I don't want the bit to trace a circle in the X/Y plane, I just want it to plunge down and come back up (yes, drilling; but knowing that deeper = wider).

Is v-carving the wrong MOp? If I select hole making > drilling it tells me the v-carve bit isn't right for drilling.

01-09-2010, 06:05 PM
V-carving is used for "tracing" the shape of the letters in x-y. What you want to do is drilling.
Create a "drill" with the included angle and diameter of your v-carve tool. Lie, in other words. Since you are going to specify the depth yourself in the MOP, the tool definition doesn't even have to be accurate.
You will need to group the "dots" into regions by size, in other words, all of the "dots" of .100 diameter will be in one region, dots of .09 diameter in another region, etc. When you create a drilling MOP you select a region (describes the centers of the holes) and assign a depth in the drilling parameters, which will be applied to all of the hole locations in that MOP. Trig out the depth required with your tool to create the diameter you need for those "dots", or just do some test cuts and measure. Make sure you do not enable the option to "add tool tip to drill depth". You want to specify the actual depth.

Other "dot" sizes grouped by regions will be drilled to their appropriate depth(s) in a different MOP.

Make sense?


01-11-2010, 11:04 AM
It was not mentioned what MOP you are trying to use.
You should use the engraving MOP.
Is that what you are trying?

01-11-2010, 12:48 PM
Thanks Joe, that does make sense. I was hoping there was an easier way, but I guess v-carving isn't thinking of the circle as a circle, but as a line to trace, as you say.

Darebee, yes, I've tried both engraving and vcarving MOps.

01-12-2010, 08:06 AM
I misunderstood the 1st post.

The drill cycle is probably the most logical choice. You can assign the same tool number as the existing V-bit to a newly created drill tool (with the same geometry - of course). The CAM wont allow a drilling OP with a milling tool (or viceversa)and this is the way around that - the CAM doesn't check for multiple occurrences of the same tool # in the tool library.

However I figure you should be able to do it in engrave by just having a POINT in the center of the circles selected. It should just feed in at your plunge rate and retract again. They will still need grouped by size and therefore individual MOPs.

I use VisualMill and have not tested this so I could be mistaken ;)