Official Luthiers Forum!

The CNC stuff is coming along, but I've run into a problem that is getting me stuck. I'm trying to carve an archtop tailpiece. I'm attaching a render of the design, which I've done in Rhino v.5. The tailpiece has a 12" radius on the top, as well as two spherical cut-outs on the side to make it pretty.



I'm using RhinoCAM to set up the machining. I am able to use a horizontal finishing operation (a 3d operation) to carve the spherical cut-outs on the side, and that operation functions and generates toolpaths just fine. But when I try to use horizontal finishing to carve the 12" radius on the top of the tailpiece, it gives me an "open loops" error. Any clue what would cause that error? Could it be the string holes? I have tried generating the toolpaths with those holes selected as regions (in addition to the perimeter of the top surface) and without those holes selected as regions, but I'm getting open loop errors either way.

Thanks for any suggestions you can offer.

The way we would go about this is first we'd patch the holes different layer different color just to make life easier for the initial toolpathing, then we'd draw a box to the extremity of the part........ , increase the box to at least 5/8 to center of the tool.... we'd then draw a curve at the lower part of the box and offset the curve 90 degrees below the part by 1/2 the distance of the tool. This now is your region. We'd also use a ball nose bit. By doing this the bit will actually clean the part to O plan even though it is a ball nose. ( We'd also add to the part additional material for index holes somewhere.... to be cut off with the reverse/final operation) We'd run horizontal roughing with the first go round then we'd run parallel finishing for the final passes..... you can add or subtract pocket or drill cutouts where every it works best..... Hope this make's since as we did it fairly quickly..... (still several more toolpaths that need to be added...... this is Rhino version 4..... we do have the latest and greatest just not on the machine I was on).

Lot of different ways to approach this..... we just found if you do some additional drawing it speeds things up when you get ready to actually make the part.

Blessings,

Kevin

Thanks, Kevin. I'm at a very basic level with this, so I'm working through your comments. My first thought was that perhaps by patching the holes that might solve the open loops error that I'm getting. Unfortunately, I'm still getting open loops errors even after patching. Any idea what causes the open loops error?

As a follow-up, I have deleted the holes for the strings for now to eliminate that as a possible culprit. But when I try to select the upper perimeter of the tailpiece as a region, I still get open loop errors. It's not an open loop -- this is a solid extruded from a single curve, and I'm just trying to select the upper edge as my region. Very frustrating. I would be happy to e-mail someone the 3dm file, if someone can help me pinpoint what I'm doing wrong that is generating the open loop errors, I would much appreciate it!

For a 3D operation like that, you can try not selecting any regions whatsoever. I think you might have to select stock but when you don't select regions, it should just make the tool paths where they need to be.

Open loops means you've selected a containment region (a 2D sketch) that has a gap in it somewhere.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

p.s. I think it's worth noting that when doing 3D finishing, VisualMill isn't the greatest at dealing with the edges of the 3D surface. Often times, it's best to extend the surface out a little past 1/2 your tool diameter so that the direction change happens off the work piece. Generally speaking, the edges have to be dealt with separately to avoid blowout.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

Thanks, everyone!

I discovered the open loop solution (with MecSoft's help) -- there was a teeny tiny gap at the upper right corner of the tailpiece that was a separate curve. I don't know why it was there, but selecting that curve fixed the problem.

I appreciate the suggestion on extending the surface past the edges to address problems with direction changes. I'll work on that. It looks like there are better ways to set up the toolpath than what I've been doing, so this is very helpful.

If you use regions and go the 5/8 of the bit beyond the part this is all handled and you want experience problems as Andy refers to with blowout. You maintain a clean part with construction parts or additions on different layers and colors that are easily turned off or on for the toolpathing ........ (On this part you wouldn't have to draw a box for the region you could follow the part but we feel that it's just easier to stay simple so the time saved for such a small part is nil...... You can ask Rhinocam to place a box stock around the part and you'll get the box or you can do an offset part..... again time savings for a non-square box is nothing in the overall picture.) We seldom ever just let Rhinocam determine the toolpath without picking regions unless we are using 4th axis. Think you will find this is the slow way to toolpath if you do.

Blessings,

Kevin

Along the lines of what Kevin suggested - you can actually create a contour that is offset by 1/2 the diameter of your ball mill and use that for your region selection. This will ensure that your part is fully carved while minimizing unnecessary toolpaths...

Trev

_________________
http://www.PeakeGuitars.com

Using the chain command in the modify tab is a good thing to try when you're having trouble with open loops.

I make models of parts with all holes and whatnot for rendering, but I use 'defeatured' models for machining. All holes, pockets, and slots are machined from curves and points, not from 3D geometry, which keeps the finish surfaces clean.

Before my CAM system supported rolling off edges and corners cleanly, I also used surfaces that were extended by 1/4" on all sides to make sure I didn't have reversal marks at the perimeter of my parts (and then cut them out with a toolpath based on a curve). So the surface I toolpathed with for a carved guitar top, for example, was larger than the top on all sides by 1/2".

This is what I machined my pinless bridges with:

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services