[rlrhett]

I recently downloaded an upgrade to my now long in the tooth version of MadCam, especially looking forward to the V-carve toolpaths listed in the "features" section of the website. Unfortunately, I'm completely stumped. I don't know how to create a v-bit in the cutter library. How do I give a bottom radius or diameter to a v-bit? Beyond that, I simply don't see a specific "V-carve" option and "along curves" doesn't really tell me anything. "V-carving" implies the ability to vary depth along the path, to have a start depth and flat depth. Don't see any evidence of that.

Is there a tutorial somewhere, or instructions? I can't seem to find one on the website either. Although I don't expect to do much "artistic" cam operations, I will do the odd inlay or lettering. I am especially interested in being able to v-carve inlay wood. If you don't know what I am referring to, please see:

D07 - VCarve Inlay Technique - YouTube

This technique allows you to make sharp inside curves, and is indispensable to anyone doing wood inlay. I don't expect to have all the convenient automatic features that V-Carve Pro has for this work. MadCam is not an artistic package. I understand that. Still, I should be able to manually recreate these steps. I am not sure where to even begin.

Does anyone have experience with this they can share, or point me in the direction of a tutorial?

Thanks.

[rlrhett]

Some progress that I will share here:

The obvious answer to how to create a v-bit was to give a bottom diameter and radius of 0. I still don't understand how to limit the depth of the cut. It appears that it will cut to the depth of the flute length. For example, if I have a 3/4" 90deg bit I can only engrave circles that are more than 3/8" (the flute length) in diameter. Anything less and the bit will just plunge to create the circle. I suppose I can play with the tool definition to limit the depth of cut.

I'll keep working....

[svenakela]

I'm not good at V-carving, it's not my cup of tea, but isn't V-carving always touching two boundary curves at the same time? That would not be possible with the image you posted, but I do understand your problem. I don't think a V-carve (check the help, search for V-Carving) care about a clipping plane. We could always ask for an improvement. If the V-carving noticed the clipping planes as a third boundary (depth) and also milled bigger regions as if they were pockets?

[rlrhett]

Yes, v-carve ignores clipping planes. It appears to ignore "stock to leave" as well. Might be useful to grey that out if someone clicks v-carving. I would love to request two additional features. However, first I think I have a work-around to duplicate the inlay process in the Vectric video.

Let us assume we want an inlay pocket with .2" depth as shown in the video using a 1.5" diameter, 90 deg bit also as shown:

To create the pocket with chamfered edges:

1. For areas that are wider than .2", create a pocketing pass with an endmill. As in the video, we'll choose a .125" straight bit. Set the depth .4", but leave .2" of stock. That should give you a pocket with straight sides that is .2" deep and offset .2" from the curve.

2. Create a v-bit tool definition that has a diameter of twice your intended depth of cut, regardless of the actual bit size. In this case .4". Note that this applies to a 90deg bit. These calculations will be differed for a bit with a different angle.

3. Create the v-carving toolpath using the usual boundaries curve and v-carving options.

You should now have a pocket .2" deep with 45deg chamfered sides.

For the male pattern with matching 45deg chamfered sides (or if you just want an embossed look):

NOTE: that for the embossed male pattern, the chamfer has to split the curves NOT preserve them as in a standard v-carving cut. Otherwise the part would sit at the surface and not fit inside the female pocket.

1. Create a box the size of your stock that encloses your artwork.
2. Create a pocket selecting your relief and the box. Set the depth to .3" with stock to leave at .1". NOTE: This is necessary per the above video to allow the male embossed pattern to fit inside the female pocket. You should now have an embossed pattern of your curves that is .2" tall and with a .1" offset.
3. Create a STRAIGHT bit that has the same diameter as your intended cut REGARDLESS of the actual bit size. In this case .2".
4. Create a profiling pass using the new bit set to .2" depth. When milling USE THE V-BIT for this tool path not a STRAIGHT BIT. The tool path should bring the apex of the v-bit to within .1" of the curve and .2" deep chamfering the edges. The boundary curves should now be half way down the chamfer allowing the male part to nest into the female part.

I haven't yet tested this with a real cut!!! The software upgrade was a Christmas gift, so sneaking off to the machine to test this workflow will have to wait until after. Still, I think this solution is inelegant. Any solution that requires custom "fake" tool definitions that can't properly be simulated is a bad solution. I'm hoping a real expert can suggest a better workflow.

In the mean time, two enhancements would make this work much easier:

1. A max depth of cut for v-carving. It would have the same effect as modifying the bit diameter, but without actually changing the tool definition.

2. Location of the boundary curves as a percentage of the cut. The default could remain that the boundary curves represent the clean top edge of the v-carve path and be represented 0%. However, if I wanted the boundary curve to represent the mid-point of the cut, I would specify 50%. If you wanted the curve to represent the deepest part of the v-carve, you would say 100%. This value would essentially be an offset of the bit towards the boundary curve represented as a percentage of the max depth of cut.

Of course, if you monkey with this setting you may get some unexpected results.

If anyone has a better work-around, or can see where this might not work and feels like saving me time/hassle/wood by pointing it out, please let me know!

[JerryBradley]

I have spent the last several hours trying to make V Carve work on some lettering on a wine barrel head I am carving. My experience has been that performance is very slow to generate tool paths and is intermittent at best, and will not work at all on some of my curves.. As best I can tell there are no tutorials for this feature and the help description is extremely basic.I have used this function in VisualMill and recall it was much more robust and very fast compared to MadCAM. In fact, I think I will go back to VisualMill so that I can finish up my tool paths.Hopefully Joakim can look at this function and improve its performance.

[svenakela]

I have spent the last several hours trying to make V Carve work on some lettering on a wine barrel head I am carving. My experience has been that performance is very slow to generate tool paths and is intermittent at best, and will not work at all on some of my curves.. As best I can tell there are no tutorials for this feature and the help description is extremely basic.I have used this function in VisualMill and recall it was much more robust and very fast compared to MadCAM. In fact, I think I will go back to VisualMill so that I can finish up my tool paths.Hopefully Joakim can look at this function and improve its performance.

I guess there is little carving info because the main focuses in MadCAM are tooling and 5 axis machining. Could you please describe how you would like the V-carving to work? Even a short description or explanation is better than nothing if you want to make a feature when programming. Unfortunately "application X is better" is not helping at all.

[JOM]

V-carving is just an extra function in madCAM. Otherwise it is no difference in using a V-cutter or any other kind of cutter in madCAM. All toolpath operations can be used with a V-cutter including roughing, finishing and curve milling.

I have made a video showing how v-cutters can be used in madCAM.
madCAM V-carving - YouTube

If you need help, you are welcome to upload your file here or at madCAM - Upload a File

Thanks,

Joakim

[rlrhett]

Dear Joakim,

With all due respect, but I cannot use all normal functions with a v-carving bit. I have tried to do a profiling cut with a v-bit, and the software would not let me. As long as I had the v-bit selected, whenever I clicked profile cut nothing would happen. As soon as I selected a non-tapered bit I could profile again. Had I been able to do the profiling cut with a v-bit, I would not have had to try the profiling pass with the straight bit in the workflow I outlined above.

I admit that I assumed since I couldn't profile that none of the other functions would work. I see you did a "along curves" path. I still have to wrap my brain around whether that created a positive embossed cut the right size, but it looks promising. Than you for your demonstration.

PS. I'm not getting any sound in the video. I get sound in other youtube videos. Is that me, or did you not narrate your screen cast this time?

That having been said, my workflow above is not effective for the intended embossing action. The advantage of this technique is to allow sharp inside AND outside corners when creating pockets/parts for an inlay. Using a straight bit definition for the profiling action does not take advantage of the v-bits unique variable/disappearing diameter for getting into tight inside corners. That is the whole point of this technique.

However, I think I have a new solution. Perhaps this is not necessary. Your solution might answer the depth question. My solution was rather than performing a profiling action, I can still create an embossing pass with the v-bit and vary the relative position of the tip of the bit by raising or lowering the boundary curves in the material.

1. Again, if I want to limit the depth of cut to 3mm, I have to create a false definition of the bit with a diameter of 3mm.
2. If I want the v-bit chamfer to split the boundary rather than preserve it, I need to lower the boundary lines in the z-dimension 1.5mm. The simulator won't give you accurate results because it doesn't know that you are using a 12mm bit, but I believe the end result will be the embossed male part that will sit inside the female part AND give you sharp inside and outside corners.

I will test the cut and post pictures of the result soon. I don't have software to make a screen cast of what I am talking about, but if it work perhaps someone else would like to.

I would still request an enhancement that will allow you to set the maximum depth and allow for an offset of the tip relative to the boundary curve without having to create false tool definitions or modify the original drawings.

[Jason Forbes]

2¢;

V-Carving should be a single operation with various settings to perform a variety of engraving effects. The V-Carve video from above does not provide the interior corners I'd wish to see. The rounding and some diving of the tool-paths are not preferred in many cases. I prefer a hard-edge chiseled look. Some projects may require a rounder look. I can produce chiseled look in madCAM but it requires a 3D model and I feel it's a waste of time when I'm certain a profile should suffice.

The following project required a chiseled edge. The Red Circle on the 'P' shows a common location for diving while crossing a deeper tool-path at an angle. The diving tool often leaves a line and reduces the quality of the finished product. Some font designs dive harder than others.

Note the sharp corners inside the engraving. I used a different CAM package and their V-Carving required extra work and manual tool-paths to produce these results.
Attachment 262230Attachment 262228


Examples of Sharp and Round inner corners. I'll attach the .3dm below.
Attachment 262234Attachment 262236

V-Carve Demonstration