VCarveProInlay

From Shopbot Wiki

Contents

Using VCarvePro for inlaying:

This method of doing inlays with VCarvePro was developed by ShopBotter Paul Zank and Damian Durante. It is rapid, accurate, versatile, and easy to use. Although the following description is highly detailed to assist the first time user, creating a V Carved inlay is actually very simple and the process of creating a VCarvePro inlay was developed to get from artwork to final product quickly and accurately as possible. The pocket is V Carved with one set of parameters and the inlay is V Carved with a second set of parameters.

It's advantages over other methods include:

  • Fast cutting using standard bits
  • Eliminates handling of individual pieces
  • Inlays with hundreds of pieces in less than an hour
  • Extremely fine level of detail without fragile parts
  • Sharp interior and exterior points
  • Eliminates the traditional “bit offset” and associated CAD work


How VCarvePro Inlay works

VCarvePro Inlay makes beveled inlays using a V bit to carve both the inlay and the inlay pocket. It is VCarve Pro’s unique ability to correctly handle the bevels on lines, arcs and points that allows the inlays to be cut without bit diameter offsets encountered with traditional CNC inlay techniques. The resulting inlays rest in their respective pockets by contact along the sides of the inlay and pocket. This creates extremely accurate inlays showing little or no gaps between materials and rivaling the very best hand made inlays.


The versatility of VCarvePro allows both pocket and inlay to be cut using the same software and same V bit but with simple differences in parametrics between the cuts. The optional use of an end mill may be useful to further reduce production time by hogging out large flat areas. (This capability is already native to VCarvePro.) Note that additional CAD work, such as compensation for bit diameter, is not required. The inlay itself is created with a backing which provides a base for multiple and otherwise fragile parts.

The Original Artwork
The Original Artwork


Preparing the Artwork

If the artwork is already in one of the following formats, it is ready to be used.

    V Carve native format (.crv) 
    DXF format (.dxf)
    Encapsulated Postscript (.eps) in vector format

If the artwork is still in a bitmap format (such as .bmp, .gif, .jpg, …) use V Carve Pro 4 to create a set of vectors from the bitmap.


Choosing the inlay depth

Typical values for the depths are:

    Inlay Flat Depth = 0.2”
    Inlay Start Depth = 0.2”
    Inlay Pocket Flat Depth = 0.3”
    

(Note that these values assume that the pocket material is at least 0.4” thick and that the inlay material is at least 0.5” thick.)

These values will insure a tight fit on the sides and leave a 0.1” gap between the inlay and the pocket bottom which will be filled with glue. They provide a large margin for error and final sanding. At the end of this process, the inlay backing (which may be holding many parts of the inlay) will be removed. The final inlay and the inlay pocket will be sanded flush.

This diagram is provided for reference only; you do not need to understand the diagram to make V Carved inlays
This diagram is provided for reference only; you do not need to understand the diagram to make V Carved inlays


Create seperate files for the pocket and the inlay

  1. Start V Carve and open the artwork file if it is a .crv file or import the artwork if it is a .dxf or .eps file.
  2. . Make sure there are no open or duplicate vectors by using the select open vectors and select duplicate vectors functions in the edit menu.
  3. Save the file twice under different names. It is suggested that you name one of them as (artwork name) pocket.crv and the other as (artwork name) inlay.crv.


Creating the pocket file

(For our example we'll use a flat depth of 0.3”)


  1. Open the (artwork name)pocket.crv file
  2. Select all of the vectors which define the pocket.
  3. Click on the toolpaths flyout.
  4. Select the “create V Carve / Engraving toolpath” icon.
  5. Click on the flat depth check box and select a flat depth. (If using the values suggested above, set flat depth to 0.3”)
  6. Select the V Tool. NOTE that the same angle V Tool must be used for both the pocket and the inlay! If possible, use the same bit. Use a small final and clearance stepover of not more than 3%.
  7. Select “calculate” to compute the toolpath.
  8. Optional Step – If there are large areas of the pocket which will be flat, it may be more efficient to also use a flat area clearance tool (an end mill) to cut flat areas very quickly.
  9. Using “Save Toolpath”, Select the appropriate post processor and save the cut file(s). Be careful to include the bit description in the file names(s) for future reference.
Graphic of the inlay pocket
Graphic of the inlay pocket
Preview of the inlay pocket
Preview of the inlay pocket


Creating the Inlay file

The pocket artwork must be flipped left to right to create the inlay, A “hog out area” is defined around the inlay, and finally, the inlay cut file is computed with a 0.2” start depth and a 0.2” flat depth.


  1. Open the (artwork name) inlay.crv file
  2. Select all of the vectors which will define the inlay.
  3. Using the Mirror Selected Vectors function from the Edit Vectors icons, horizontally flip the vectors left to right. Next select “Close”.
  4. Use one of the “Create Vectors” icons to create a polygon around the inlay. Using the rectangle icon is the simplest one to use. Make sure the polygon leaves at least double the margin as the cut is deep. The area between the inlay artwork and the polygon will create the inlay backing. Next select “Close”
  5. Select all vectors (including outer polygon).
  6. Click on the toolpaths flyout.
  7. Select the “Create V Carve / Engraving Toolpath” icon.
  8. Set the pocket start depth. (If using the values suggested above, set the “Start Depth” to 0.2”.)
  9. Click on the flat depth check box and select a flat depth to the desired depth. (If using the values suggested above, set flat depth to 0.2”.)
  10. Select the V Tool. NOTE that the same angle V Tool must be used for both the pocket and the inlay! If possible, use the same bit. Set final and clearance stepover value of 13%. This will allow us to use the v bit to hog out the area between the inlay and the outer polygon.
  11. Select “Calculate” to calculate the cutting path.
  12. Optional Step – If there are large areas of the pocket which will be flat, it may be more efficient to also use a flat area clearance tool (an end mill) to cut flat areas very quickly; however, this decrease in cut time is at the expense of a bit change.
  13. Using “Save Toolpath”, Select the appropriate post processor and save the cut file(s). Be careful to include the bit description in the file names(s) for future reference.


Graphic of the inlay
Graphic of the inlay
A preview of the inlay with its backing
A preview of the inlay with its backing


Even though it looks all wrong, it does fit correctly. The rills are an artifact of the 13% stepover which was used to reduce hog out cut time. They are in the inlay backing and will be removed when the backing is removed. If one decided to use an end mill for hogging, the rills will not appear.


Assembling the Inlay

At this point, the cut files have been created for both the pocket (on the left) and inlay (on the right). After the inlay and the pocket have been cut, trial fit the inlay into the pocket. The fit should be snug and sort of snap into place. If cut correctly, there will be a gap between the pocket and the inlay base of 0.2”. This is intentional and provides a space for glue squeeze out and a margin for lateral and angular misalignment. If the fit looks good, apply glue to both the pocket and the inlay. All mating surfaces should be covered but excessive glue should be avoided. With clamps and/or weights at the ready, press the inlay into the pocket and apply pressure with clamps or weights until the glue sets.

When the glue is fully set, cut off the excess part of the inlay (the backing). Using a radial arm saw adjusted to just clear the inlay base is a quick way to accomplish this. A drum sander can also do the work (but very slowly). Yet another option is to remount the assembly back into the cutting machine and mill off the inlay backing. The process can be repeated as necessary for additional inlay grain directions or for different materials inlaid into the same base.


Assembling the inlay in pictures

The pocket
The pocket
The inlay and backing before the excess wood under the clamps is cut off
The inlay and backing before the excess wood under the clamps is cut off
The inlay setting in the pocket. Note that it rides high but it is obvious when it is in place.
The inlay setting in the pocket. Note that it rides high but it is obvious when it is in place.
Copying the position of the inlay onto the pocket piece with a pencil makes it much easier to reposition the inlay after glue has been applied
Copying the position of the inlay onto the pocket piece with a pencil makes it much easier to reposition the inlay after glue has been applied
The inlay backing being removed.
The inlay backing being removed.
The backing has been cut off and it is ready for sanding. (The clear shiny stuff is superglue.)
The backing has been cut off and it is ready for sanding. (The clear shiny stuff is superglue.)
The finished inlay
The finished inlay



Sample Inlays

A Butterfly inlay
A Butterfly inlay
Closeup of the left wing
Closeup of the left wing
Hummer
Hummer


--Paul Zank 12:15, 12 Aug 2007 (EDT)

A Problem that will Occur When Using "Small" V-bits

It is instructive to mention one problem that can come up with this technique. If you use "too small" of a V-carve bit some problems can occur. The first toolpath made to cut the 7.5 inch diameter star inlay shown below was created with a 1/2 inch diameter 90 degree V-bit. The "Start Depth" was 0.2 inches and the "Flat Depth" was 0.2 inches. When the toolpath for the inlay was previewed in V-Carve Pro, the following result was obtained:

Image:Problem_with_using_small_diameter_bit.jpg

Not only are there large "divots" at all 5 inner star corners, but the rest of the edges of the cut do not begin their taper until after a short vertical drop. This problem has been discussed on the V-Carve forum, and can be eliminated by using a larger diameter bit. This is shown in the next photo:

Image:Problem-resolved-by-using-larger-diameter-bit.jpg

It is worth discussing WHY this problem happens. The reason is that Vcarve Pro assumes that you will not be cutting any material until the bit gets below the "Start Depth". The Vectric folks provided the "Start Depth" to allow you to v-carve or inlay at the bottom of a pocket. So VCarve Pro does not actually constructing a tool path until it gets to depths below the start depth.

Another "watch-out":: if you specify a value of 0.25 for the Cutting Parameter "Pass Depth", the program will still only create one pass because it thinks it is only cutting a total of 0.2 inches deep.


--Harold Weber 08:31, 20 May 2009 (EDT)


Contributors
Paul Z, Harold weber
Personal tools