Official Luthiers Forum!
http://w-ww.luthiersforum.com/forum/

Inlays done on my Techno
http://w-ww.luthiersforum.com/forum/viewtopic.php?f=10106&t=24906		 Page 1 of 1
Author:  1bordeaux [ Sat Dec 05, 2009 12:01 pm ]
Post subject:  Inlays done on my Techno
Hi Guys,
Thought I would share a few inlays done recently on my cnc...
Comments welcome, I've got a lot to learn!
Of course the butterfly was routed by hand, and the tattoo image wasn't complete when the image was taken, but you get the idea....

Paul
Attachment:
butterfly inlay 006 (2).jpg
Attachment:
butterfly inlay 020 (2).jpg
Attachment:
Tattoo inlay 006 (2).jpg
Author:  Parser [ Sat Dec 05, 2009 2:03 pm ]
Post subject:  Re: Inlays done on my Techno
Looks great! I bet you'll be routing by hand less and less...! [:Y:]
Author:  1bordeaux [ Sat Dec 05, 2009 3:53 pm ]
Post subject:  Re: Inlays done on my Techno
The strange thing is how addictive it becomes to get a design to cut "right". In the interest of learning, I have done some client inlays in 4-6 hours whereas hand cutting would have taken 1 hour or less, although it's usually on the small stuff.

It is cool to have a standard pattern being cut in one room while I hand cut in the other!
Author:  Tim McKnight [ Sun Dec 06, 2009 5:32 pm ]
Post subject:  Re: Inlays done on my Techno
Nice work Paul. What diameter bit, depth of pass and feed speeds did you use?
Author:  Sheldon Dingwall [ Mon Dec 07, 2009 11:23 am ]
Post subject:  Re: Inlays done on my Techno
Nice work.

Another challenge is how you lay out your pearl blanks and get them into your CAD program. I've been gluing them to an mdf spoil board, taking a photo with a 6" rule for reference and importing that into Rhino. The last set had some scaling errors due to the length of the spoil board in comparison to the rule. From now on, I'm going to just measure the length of the spoil board and use that to scale.

If anyone has a better way to do this I'd like to hear it.
Author:  1bordeaux [ Mon Dec 07, 2009 12:53 pm ]
Post subject:  Re: Inlays done on my Techno
Tim McKnight wrote:
Nice work Paul. What diameter bit, depth of pass and feed speeds did you use?


.0156 bit from precisebits, .013/ pass @ 7.5ips.

I have gotten into the good habit of checking each bit for runout at every tool change, which helped improve cutter life and quality of cuts.
Author:  Bob Garrish [ Mon Dec 07, 2009 2:18 pm ]
Post subject:  Re: Inlays done on my Techno
1bordeaux wrote:
Tim McKnight wrote:
Nice work Paul. What diameter bit, depth of pass and feed speeds did you use?


.0156 bit from precisebits, .013/ pass @ 7.5ips.



IPM...unless you've got a -really- nice spindle ( 1.8million RPM or so :) )
Author:  1bordeaux [ Mon Dec 07, 2009 3:14 pm ]
Post subject:  Re: Inlays done on my Techno
Umm.... No, we work really fast here in upstate NY... wow7-eyes

You're right, I meant to say we type really fast...
Author:  Parser [ Mon Dec 07, 2009 4:16 pm ]
Post subject:  Re: Inlays done on my Techno
I break multi-piece inlays into separate blocks and draw them on sketches of the shell blanks.

Here's a blue marlin inlay I did recently with white and black mother of pearl in Indian rosewood...as well as a few screenshots to show the CAD/CAM process:
Image

Image

and here's after inlay and a little sanding:
Image

I cut the shell and the inlay cavity using my K2. I offset about .004" per side (to the outside) on the cavity cuts and only had to do minimal hand fitting to get everything in there. On single piece inlays I can get away with a little less gap. I used a .031" end mill at 25,000 RPM and about 2 or 3 ipm on both the shell and the rosewood. My K2 uses a porter cable router as a spindle and the runout on these isn't as well controlled as a true spindle...so I run on the slow side. All in all though, the thing works really well and sure beats the heck out of a jeweler's saw!

Trev
Author:  Stuart Gort [ Sat Mar 13, 2010 2:51 am ]
Post subject:  Re: Inlays done on my Techno
Those feed rates are a little surprising. These inlays (or at least the finshed edges) are cut with a .030" two flute endmill at 4000 rpm and 20 ipm. I step down about .020" as I go depending on the type of wood.

The trick I use is to first define the edge by using a ball mill and getting more aggressive after that.

Check it out.....

Using a contour path.......if you take an .0625" diameter ball and program your first cut to be a -.010" depth, then offset the cut by -.0083" the ball will cut to a -.010" depth with the edge placed right on your programmed contour line. This establishes that edge regardless of the grain direction. Every subsequent depth can be made much more agressively without much chance of a rip.
Author:  Tim McKnight [ Sun Mar 14, 2010 8:38 am ]
Post subject:  Re: Inlays done on my Techno
Z,
Inoticed tuner buttons in the top picture. Tell me a bit about your process to cut buttons please.
Author:  Stuart Gort [ Tue Mar 16, 2010 2:37 am ]
Post subject:  Re: Inlays done on my Techno
Tim McKnight wrote:
Z,
Inoticed tuner buttons in the top picture. Tell me a bit about your process to cut buttons please.


Hehe.....you WOULD ask. It's the most fixture intensive thing I've done yet.

I'm in the middle of making tooling that allows for multiple sets to be made during an operation. The first time I did it I just made one at a time - while I was goofing around with cutting wood. Technically....tuning knobs were the first parts I ever made from wood.

I'll get pic's up when I'm done with these tools next week. That will go a long ways to explain this process. For now, I've done the first op on about 25 sets of knobs. I've made these in maple, toasted maple, purple heart, paduck, wenge, and bloodwood. The cycle time will be about an hour per set which I will shorten some but the process now guarantees not to rip anything. These knobs are truly nifty.

Operation #1 starts with a stick of bloodwood - 1" x 1" x 8" (long grain) out of which I cut six knobs. I cut one of the flat sides with a surfacing operation and the outside profile is cut with a contouring operation down to below the lower part plane. This contouring op follows the principals laid out on the post above. I start with a surfacing op, then a shallow 3D contour cut with a ball to establish the profile edge without ripping, then a stepped down 3d contour with a ball to finish the profile down further, then swich to a flat endmill to finish the base. The six parts remain connected on a .25" base. I'm trying to keep the continuity of the grain intact and make these in matched sets.

Operation #2 requires a tool that holds two sets of these knobs (12 knobs) in two rows. The fixture allows clamping pressure to be independently applied to each knob so they hold in place as the machine cuts them apart. On this op the second side is sculpted with a surfacing operation and the basic shape is finished. The operation more or less follows the concept above...the deft use of ballmills to define the profile edge in order to guarantee no rip out.

Operation #3 requires a tool that holds two sets of the knobs on edge so that a cavity can be milled out of the bottom to constrain the square pole of the machine head. This cavity is oversized so that it can be filled with epoxy and then later milled to fit the square pole after the epoxy cures. The effort here is to eliminate the possibility of cracking over time as the machine head is used. The epoxy will stabilize the wood and be far less prone to crack than the wood itself.

Operation #4 requires a tool that holds 12 knobs on their edges in order to countersink and drill the screw hole that holds the knob onto the peg shaft.

I'll try to get nice photos along the way to illustrate this.
Page 1 of 1 All times are UTC - 5 hours
Powered by phpBB® Forum Software © phpBB Group
http://www.phpbb.com/