Has anyone used the Carvewright to produce inlays?

[DonavanLane]

I am trying to use the CarveWright to make a simple Inlay produced from a Filigree 07 Pattern Outline.
Help! I can’t seem to get my Inlay Cutout (Female) to match the same size (Width) as the Inlay Insert (Male).
Has anyone used the Carvewright to produce inlays?

[bergerud]

I have it on my list of things to try. I thought you just use the inset to be plus or minus the bit radius when you select the (straight) bit. Is it way off or is there just problems where the path curves sharply? Does it look right in Designer and carve wrong or does it look wrong in Designer?

[DonavanLane]

Yes, you are correct. Thanks for responding quickly Bergerud. I agreethat I need to adjust the INSET of the 1/8 Straight Bit. But there appears to be two problems. In orderto cutout the middle section of the Female Inlay, it must also use the 1/16carving bit.

I purchased the machine to create perfect inlays.

So, in order to create the female Inlay I had to create TWO outlines superimposedon top of each other, One Outline Path for the Straight Bit and a Second OutlinePath (copy/paste of the same outline) for the carved area.

For the Straight Bit Outline, I adjusted the Inset to be .613 (Radius of the1/8 Bit). That worked in that the 1/8Bit traveled the correct path, but the Second carved Outline doesn’t have aINSET selection. Any idea how to alsoinset the Carved 1/6 Bit?

I spoke with Tech support and they shared that in order to create a matchinginlay I have to manually adjust the size of the patterns (Outline). I have a hard time believing that this has tobe guesswork trial-and-error to make the two patterns match in size. I would be cutting tons of patters in orderto get it right.

Any input would be great appreciated.

[Jeff_Birt]

Remember the 1/16" carving bit is tapered so you will not get striaght sides or an accurate sized cut with it.

For the female part you have the basic idea, use a carve region to create the pocket. What will happen though is that the taper of the carving bit will make it slightly larger. If you add a 1/8" feather you can keep the pocket from coming out over-sized. Now, using a second outline like you did before, with an inset, you can clean up the pocket sides with a straight bit and have it come out the correct size.

For the male part of the inlay you will want to use a straight bit to cut it out. You can use the cut-out tool to apply the correct offset automatically.

Even after all of this you will have to do a little experimentation to get things to come out right. Even a CNC machine is not 'perfect'. The bits will never cut 'exactly' their own diameter, any run-out in the chuck and the small out of bit flexure that occurs will have an effect. Not to mention that wood can compress as its being cut and spring back ever so slightly. American Woodworker did can article comparing the CarveWright to two other small CNC machines, all of them required tweaking to get the inlays to come out right.

[AskBud]

Just a thought, have you considered the assignment of 1/16 cutting bit to do the carve?
If you have no other carve areas on the MPC, which need the standard carving bit, it might work to go to "Board Settings" and assign the best bit for the job. It might just be what allows you to only need to tweak your pattern.
AskBud

[DonavanLane]

Awesome Idea Jeff! I would never have suspected adding a feather to the carved region. I'll run home early and try this and send a picture of the completed result.

[DonavanLane]

Thanks AskBud for the heads up about the 1/16 bit. Did you mean the 1/16 straight bit? I tried to order a 1/16 straight bit but the CarveWright folks said they were in the process of determining a new Vendor for that bit and had none available. Anybody have a 1/16 straight bit they would like to sell that works with the new Model C (CarveTight?) Chuck?

[bergerud]

Suppose you choose the 1/8 straight bit as the pattern bit in board settings instead of the 1/16 carving bit. Outline your pattern and carve region. It will be a radius (0.0625 not .613) larger than you really want. Then for the male part inset by the full 1/8. (A 1/16 straight bit would half the error.)

You know there are more fundamental problems which designer has no hope of solving. The simplest of which is that the bit cannot cut a curve which turns faster the its radius. One cannot inlay a square because of the corners in the female part will be round.

[DonavanLane]

Thanks Bergerud, is there a way to enter four digits after the decimal for the INSET?

I was only able to enter three digits, thus forcing me to round the 1/16th radius decimal conversion from 0.0625 to .613

[bergerud]

No way I know of but you mean 0.063 not 0.613

[DonavanLane]

Yes, thanks for catching that. The radius conversion I meant was 0.063.

[AskBud]

Suppose you choose the 1/8 straight bit as the pattern bit in board settings instead of the 1/16 carving bit. Outline your pattern and carve region. It will be a radius (0.0625 not .613) larger than you really want. Then for the male part inset by the full 1/8. (A 1/16 straight bit would half the error.)

You know there are more fundamental problems which designer has no hope of solving. The simplest of which is that the bit cannot cut a curve which turns faster the its radius. One cannot inlay a square because of the corners in the female part will be round.

Think about it! In a pre CW world, how did/do you make your carved inner corners square? Didn't you use a hand tool such as a chisel or knife? Don't those things still exist?
AskBud

[liquidguitars]

Remember the 1/16" carving bit is tapered so you will not get striaght sides
or an accurate sized cut with it.



I use the 1/16" carving bit all the time for inlay it's a good fit for all inlay work up to about .25" thick and of coarse it's very accurate. I use the taper to my advantage.

[bergerud]

The square was just an example Bud. Anywhere where the offset curve crosses the evolute will not be carved. This could be a problem if the curve "wiggles" a lot or has many cusps and you are using a 1/8 bit. Not as if I know what I am talking about, I have yet to try inlays!

[Kenm810]

Squaring your carved inner corners, -- with a little practice these have worked well for me.

[DonavanLane]

Jeff Birt - you are a genius. Your trick of using the 1/8 Feather and then playing with the INSET dimensions worked perfect. I made a very near match. After testing here are the findings to make a very good, near perfect Inlay:

Female Inlay "Pocket" Thickness/Depth 1/8 Inch (0.125) Best Inset 0.074 using a 1/16 Carving Bit matched with a 1/8 Straight Bit.

For those that wish to create Inlays, here are the steps to create an Inlay from the outline of a Basic Pattern.
Step 1 - Create the female inlay pocket first, using a 6” Length, 2.75” Width and .75” Thickness board
1. Choose File, New, use the board settings above
2. Choose the Pattern Tool, Choose Filigrees – Filigree 07 and place on board – Right Click on Object, choose Center | Center Both
3. Right Click on object, Choose Outline Pattern(s)
4. In the carving windows – delete the initial Filigree 07 carving so only the first “Path” outline remains. The Filigree object to be deleted will be the second object.
5. Select the new First “Path” from the carving window, right Click on the object and copy to clipboard, then paste,
6. Choose each object and right click, choose Center | Center Both
7. Now you have two “Paths” placed identically on top of each other – this is so the second path 1/16 Carving bit can carve the inside and the first path is for the Straight 1/8 bit to make perpendicular edges. Note: If you have a Straight 1/16 bit I suspect this will work even better for tighter circles.
8. Choose the First Path – Select Bit, Choose 1/8 Straight bit – Set Inset to .074 (.074 when using a 1/8 Straight Bit), set Depth .125 Inches, Click ok
9. In the carvings Window, Choose the Second Path – Click Carve Region icon. Set the depth to 0.125
10. Choose the Feather Icon, Feather 1/8 Inch, Accept (Make sure feather is inside object).
11. Be sure to cut your physical stock to with a width of at least 2.75” and length adding 7 Inches to your total length, for this example physical length 13” with thickness .75”
12. Save and Upload
13. Follow machine prompts to cut.

Step 2 - ”Straight Cut” the male Inlay, using a 6” Length, 2.75” Width and 0.125” (1/8”) Height board (0.125 important Measurement!)
1. Choose File, New, use the board settings above, be sure to set thickness at 0.125, and proceed with the “Invalid Dimension” minimum board size alert.
2. From the Previous Pattern above from the Carving Window copy to the clipboard the SECOND Path (Choose Second Path – CTRL+C) from the Carvings Window (Or choose Filigree 07 from the same Pattern Tool choice used above. Paste (CTRL + V) to the new project.
3. Right Click on Object, choose Center | Center Both
4. Right Click on the pasted object and choose Outline Pattern(s). Notice you have another Path in the Carvings Window. Delete the initial path (Second in the list), leaving only the outline.
5. Click on the new outline object and choose Cut Path Icon, Flip Cut and Accept
6. Save and Upload, When prompted for Auto-Jig, Choose Ignore. Note: You will need to attach (Double Sided Tape works Great) your male Inlay 1/8” stock to a ¾” Thickness Board (At Minimum ½ Inch) with a width of at least 2.75” and length 13” ..adding 7 Inches to your total length, for this example physical length 13”. Basically, you need to match your host board size to your Inlay Stock size.
7. When you are at the CarveWright machine, choose the following prompts. The most important prompt is when the machine asks “Select Cut Through Depth” you must choose #1, Project!
8. Project Menu – Press Enter
9. Choose Project, Enter
10. Stay Under Rollers?, 1- Yes
11. The machine will now measure the board
12. Keep Original size?, choose 1
13. Center on Board, 2 (Or choose where you want the cut to start)
14. The machine will measure the board again
15. Cut board to size? 2 - No
16. Select 1/8 Cutting Bit – Enter
17. Load Bit – Enter
18. The machine will find the surface
19. Select Cut Through Depth, Choose 1 - Project
Machine will now start to carve the piece, placing tabs. When completed, remove tabs and sand where needed. You should have a near perfect match.
Hope this helps you create a great Inlay.
Donavan

[liquidguitars]

This video show the 1/16" carving bit in action, the video shows some chips but that just the waste, the key is to flip the inlay stock so ya have a wedge surface making a good fit.
at frame 0:09 you can see the inlay the abalone is face down.


http://www.youtube.com/watch?v=5U99l9SuHgw

[Jeff_Birt]

That is a clever idea Brandon, take advantage of the taper to help hide the joint.