Carbide Create V-carving (advanced)

From ShapeOko
Jump to: navigation, search

This is to be an advanced tutorial on working around limitations in the V-carving CAM algorithm in Carbide Create. Initial discussion at:

One step in it however, is not limited, carving a pocket around the text, and is presented first in addition to other tutorials. By request, the letter portion of this was done on the Shapeoko forums:

Note that CONTROL clicking with the mouse will add or remove clicked on geometry from the current selection (as opposed to Shift-click which is the typical interface convention) --- the instructions below show accomplishing this task w/o that feature.

Please compare with the official video:

Tool creation

It is necessary to have an appropriate endmill tool setting to select. If one doesn't, consult the manufacturer's specifications, and then add a tool:

  • Toolpath
  • Edit Library
  • Add Tool
  • double-click on the new tool to go into edit mode
  • edit as needed
  • Ok
  • close window

Df engraving text toolpath toolcreation.jpg

(The endmill in question is the #301 0.50" V-Bit Cutter - 90° from Carbide 3D)

Note that Carbide Create uses taper angle, not the typically reported V-angle, so one must divide by 2, so the 90 degree bit is reported as having a 45 degree taper.


Okay, trying again, let's do this step-by-step w/ detail suitable for a tutorial:

- first find a suitable image.
- selected the vector .pdf: -- the 3D shield versions are likely needlessly complex and the b/w version doesn't afford all the educational opportunities of the colour one.

Open the .pdf in a suitable vector editor (I selected Inkscape) and switch to outline view --- View | Display Mode | Outline

(optional, Inkscape affords an option to automatically set the page size to match the drawing, File | Document Properties | Resize page to drawing or selection --- this was done here to make for a consistent sizing and placement of the image)

Cc vcarve df importandsetup.jpg

Note that there are a number of instances of over-lapping elements --- these must be addressed so that the image can have toolpaths applied w/o interfering with other elements.

When selected, the image is a Group --- ungroup until the image is composed of nothing but paths --- there should be 42 of them.

Then, select paths which overlap, duplicate the one which you wish to subtract from the other, select the second path and Path | Difference until all such overlapping is eliminated. When viewed in Normal mode, the appearance should be much the same as the original:

Cc vcarve df fullcolour.jpg

However, when viewed in outline mode, one sees only that geometry which one would wish to have cut:

Cc vcarve df outline.jpg

At this point, the file is usable for V-carving, if there is no need to consider the matter of how wide the V-bit is, and how deep it will cut (the piece would be very small), or if the CAM program used for V-carving has a facility to limit the depth to which it will cut. That is not the case with Carbide Create, so some additional planning, math and geometry are necessary.

The first thing to do is to decide what elements will be cut to what depth:

  • the outer gold, and the blue letterforms will be left full height
  • the white surrounding the letters may be a normal V-carve (if sized so that the bit can plunge fully into the piece to cut the widest element
  • similarly the gold of the feet will be left at full height
  • the black of the talons will be left at full height, but pierced by a simple V-carve
  • the grey will also be left at full height
  • the white areas will be recessed to half the intended cut depth
  • the inner blue areas of the shield will be cut to the full cut depth, and the sharp corners and inner edges will be will be V-carved so as to increase their definition --- this will leave some areas which will need to cleaned up w/ a chisel

Then, we must decide:

  • what size the piece will be cut to
  • what the thickness of the stock will be
  • what the greatest depth to which we will be cutting
  • what angle V-bit will be used

For this tutorial:

  • 5" wide
  • 1/4"
  • 1/8"
  • 90 degrees

The first thing to determine is what width a 90 degree V-bit will cut at a depth of 1/8" --- this is easily determined using trigonometry, or may be determined by drawing up the relevant geometry, or realized easily when one notes that the projection of a 45 degree angle at a given depth results in one-half of a square, so the width offset is the same as the depth to which we will be cutting, which greatly simplifies the math.

At this size, there is no need to depth limit the space around the letters.

V-carving text with a field

First, create or import a suitable geometry. It must have internal text, and a pair of paths (inner and outer) to define the border.

Df engraving text import.jpg

One must be able to select only the afore-mentioned paths --- some complex files such as the sample below will require complex selections which may be made easier by moving elements temporarily out of the way (alternately, control-click on elements which you wish to add to the current selection). Select each in-the-way path and change its coordinates so that it is out of the way --- in the image below, we have selected the outer path and added 5 to the Y coordinate and clicked Apply:

Df engraving text clearingforselection.jpg

Repeat for each path which interferes with the selection, then select the text and the inner path:

Df engraving text selectinnerandtext.jpg

Click on Toolpath and then V Carve:

Df engraving text toolpath vcarve.jpg

The toolpaths will then be calculated, which reveals another limitation of Carbide Create's (current) implementation of V-carving. Only the outermost pair of paths will have the V-carve operation applied to them.

Df engraving text toolpath vcarve inner text.jpg

One must then zoom in and select the innermost countours (counters in typographic parlance) which one wishes to have engraved and apply toolpaths:

Df engraving text toolpath vcarve letters.jpg

Repeat applying toolpaths to each counter, naming each appropriately:

Df engraving text toolpath counters.jpg

Interestingly, since in the current implementation, Carbide Create does not consider Toolpath creation to be an undoable operation, one may restore them by simply undoing 3 times:

Df engraving text toolpath originalpositions.jpg

Lastly, select the outermost path and select an appropriate endmill and operation to cut it out. Note that if one wishes the piece cut out with a V-bit, one must manually offset the path or add geometry to allow V-carving all the way around the object. In this instance, we will simply cut with a round endmill and use a file to clean up the pair of internal radiuses:

Df engraving text toolpath outline.jpg

One may then click on "Show simulation" to preview the file:

Df engraving text toolpath preview.jpg

If all is okay, click on "Save GCode" to create the .egc file for cutting.