Concrete Printer RSS feedConcrete Printer on FlickrWatch Us on YoutubeLike us on Facebookhttps://twitter.com/ConcretePrinter

Design Your Engraving

We recommend using Vectric’s VCarve toolpath design software to create the design for your engraving. This tutorial goes through the fundamentals of engraving your first job. More info and tutorials about using VCarve (and the stripped down version – Cut2D), as well as purchase information, can be found at Vectric’s website.

  • Step 1 - Create Job Size
  • Step 2 - Import Vector File
  • Step 3 - Select All Vectors
  • Step 4 - Size the Artwork
  • Step 5 - Center the Artwork
  • Step 6 - Open Toolpath Toolbar
  • Step 7 - Create Pocket Toolpath
  • Step 8 - Set Toolpath Cut Depth
  • Step 9 - Select and Set Tool
  • Step 10 - Clear Pocket
  • Step 11 - Preview the Toolpath
  • Step 12 - Save the Toolpath
  • Step 13 - Save VCarve File

Click image for larger view.  For smaller screens, click the expander icon in the top right of the pop-out window for the full size view.

Step 1 – Create Job Size and Position

    • Open VCarve and click ‘Create New File’.  The Job Setup Box will appear.  Set your job size – use the dimensions of the Concrete Printer’s engraving area – 36inches wide x 24 inches tall.
    • Next, make sure the thickness is set somewhere above .5 inches.  If its set lower than your cutting depth the file will not render an engraving toolpath.
    • On XY position click the center mark.  Your machine will register this as the ‘zero point’ of your engraving.
    • Click ‘OK’

 

Click image for larger view.  For smaller screens, click the expander icon in the top right of the pop-out window for the full size view.

Step 2 – Import Vector File

    • Click ‘File’, then ‘Import’, then ‘Import Vectors’
    • Find your EPS, AI, PDF or other vector art file and open it.

 

Click image for larger view.  For smaller screens, click the expander icon in the top right of the pop-out window for the full size view.

Step 3 – Select All Vectors

    • With cursor over the artwork, right click and select ‘Select all Vectors’

 

Click image for larger view.  For smaller screens, click the expander icon in the top right of the pop-out window for the full size view.

Step 4 – Size the Artwork

    • With the artwork selected (Pink dashed lines), left click on the selection. Little square edit nodes should appear around the compass points of the artwork.
    • Place your cursor over one of these nodes and ‘pull’ while holding down the left mouse button
    • Try experimenting with pulling the node while also holding down the Shift key
    • Next experiment pulling while holding down the CTRL key
    • Next experiment pulling while holding down the Alt key

Holding down Shift, CTRL, or Alt allow you to scale artwork in various ways.

HINT
Undo: You can ‘undo’ your steps with ‘CTRL’+'Z’ (‘CTRL+Y for redo) or use the undo/redo arrows in the ‘File Operation’ area shown here

 

Click image for larger view.  For smaller screens, click the expander icon in the top right of the pop-out window for the full size view.

Step 5 – Center the Artwork

    • Once you’ve enlarged your artwork you can center it within the job by clicking the ‘Center in Material’ icon

Click image for larger view. For smaller screens, click the expander icon in the top right of the pop-out window for the full size view.

Step 6 – Open the Toolpath Toolbar

    • Open the Toolpath toolbar by clicking the tab in the top right corner

HINT
To keep the toolpath toolbar open, click the pin to keep the Toolpath toolbar open

Click image for larger view. For smaller screens, click the expander icon in the top right of the pop-out window for the full size view.

Step 7 – Create Pocket Toolpath

In this instance we will create a pocket toolpath.  The selected areas will be engraved.

Click image for larger view. For smaller screens, click the expander icon in the top right of the pop-out window for the full size view.

Step 8 – Set Toolpath Cut Depth

Set the toolpath Cut Depth to .2″ to .25″. Its important to realize this isn’t the actual depth your bit will cut. This is amount of depth the floating head on your machine will follow to as it moves across the job area. Typical variance of a patch of concrete can be anywhere from 1/8 inch to over 1/2 inch!

You want to engrave the entire project without gouging the high spots in order to skim the low spots (without the floating head that would be your only option). The spring loaded action on the floating head is light enough that it won’t gouge the high spots, yet it will push down the bit into the low spots to ensure they are engraved.

For pockmarked concrete or very uneven concrete, you may need to come back to your VCarve file, select parts of your design that were not engraved or only slightly skimmed and create a new toolpath with a deeper cutting depth and save as a separate file to load into Mach3.  As long as you don’t move the machine, you will be able to go back over missed spots using this method.

Click image for larger view. For smaller screens, click the expander icon in the top right of the pop-out window for the full size view.

Step 9 – Select and Set Tool

  • Click the ‘Select’ button under ‘Tool:’

Here in our pop-out window we find a large number of different bits for applications that your Concrete Printer is fully capable of tackling. With concrete, we are dealing with different animal. The bit is constantly changing as it wears down while it engraves. If we are using a V-shaped concrete bit, the flat end area of the bit (the part of the bit will be actually touching the concrete) is also constantly changing in diameter (getting larger as it wears). Fortunately, the effect needed is also less precise than, for example, an engraving in wood or aluminum, so we will need to ‘lie’ to the software to compensate for these changes and allow the software to calculate the toolpath.

  • Set the bit diameter to .25 inches
If you are using a new V-shaped bit, the tip is useful for engraving smaller details, but keep in mind that the smaller the tip diameter, the faster the bit will wear. We will be using a new V-bit for this project, but knowing the tip point will wear relatively quickly, we will tell the software that its diameter is .25 inches.

Even if the bit we are using is worn to a diameter greater than .25 inches, we may need to tell the software that the diameter is smaller than it actually is. Giving the bit a larger diameter setting (that may be more accurate) might prohibit the software from calculating a tool path in areas narrower than .25 inches (for example, the decorative horizontal line above ‘Landowski’

  • Set the stepover to about 30%
The stepover is the amount the bit travels over its preceding pass. A lower percentage will produce a smoother engraving area. A higher percentage will leave ridges along its engraving path. Of course, the more stepover (lower percentage) the more bit wear and vice versa.
  • The spindle speed is irrelvant. You will engrave concrete with maximum RPM on your spindle. For engraving wood and other materials, you will use the included speed controller to adjust speed
  • Set the feed rate at 4-7 inches/sec
The slower the feed rate (the rate your bit will move across the toolpath), the more bit wear and the deeper your bit will engrave toward cut depth (the spring action on the floating head will have more time to ‘drill’ into the concrete)
  • Set the plunge rate between 1-3 inches/sec
Again, the slower the rate (lower number), the longer your bit will dwell on one point as it lifts then lowers onto the next part of the toolpath – and improperly set plunge rate will create ‘drill marks’ where the z-axis (up and down axis) lowers into a new part of the toolpath before moving across the surface.
  • You can change the name of your tool if you like, or just click ok and remember which tool you edited.

Click image for larger view. For smaller screens, click the expander icon in the top right of the pop-out window for the full size view.

Step 10 – Clear Pocket Settings

There are two different methods how the machine can clear the engraving area:

  • Offset will follow the shape of the area to be engraved from the outside in (if it were a circle to be engraved it would follow the edge and spiral to the center). This method gives the bit a shorter engraving path and a shorter engraving time, but the effect on concrete isn’t as desirable in our opinion
  • Raster creates a sweeping motion, zig-zagging back and forth inside the shape to be engraved, then (if set to ‘last’) makes a final pass around the edges (‘Profile Pass’).
  • Click the Raster radio button
  • Set the Raster Angle to 45 degrees (setting it to zero or 90 might be more desirable if you project has thin horizontal or vertical lines)
  • Set the Profile Pass to ‘Last’
  • Pocket Allowance will help you ‘cheat’ your toolpath.
Many times your bit (‘Tool’) diameter will be too wide to hit details smaller than the diameter of your bit. When this happens the software will simply skip that area to be engraved. Rather than compensating for this by creating a multitude of toolpaths with different bit diameters for different parts of your design, we’ve found using a negative number between -.01 to -.09 of the Pocket Allowance will usually allow your toolpath to created and hit all areas of the design.
  • Click ‘Calculate
The Pocket Toolpath settings will now close and the toolpath will render.The blue lines are the path that your bit will follow to engrave. The red lines are where the z-axis will lift the spindle and travel to the next area to be engraved.

If there are areas of your design where the toolpath did not register, double click the Pocket under ‘Toolpath list and either change your pocket allowance settings (many times just -.01 increments will change the effect) or lower your bit diameter setting under ‘Tool’>'Edit’. Click ‘Calculate’ again to recalculate the toolpath.

Click image for larger view. For smaller screens, click the expander icon in the top right of the pop-out window for the full size view.

Step 11 – Preview the Toolpath

After clicking ‘Calculate (Step 10), the Preview options will appear. Experiment with the different options to get different previews

  • Click ‘Preview Toolpath‘ or if you’ve created multiple toolpaths for different parts of your design, click ‘Preview all Toolpaths’

The engraving preview will render with the options you’ve chosen. If you need to edit something in the toolpath, double-click the toolpath name (in this case ‘Pocket 2′ under Toolpath List and repeat previous steps to tweak your toolpath. You can then click Reset Preview to clear the current rendering.

With your cursor over the preview image, hold down the left mouse button and move your mouse – you can rotate the preview image to see it from any angle. Hold down CTRL and scroll your mouse wheel to zoom in and out. Hold down CTRL and the left mouse button to pan the image.
  • Click ‘Save Preview Image‘ if you need to send a rendering to your customer for their approval.

HINT
Clicking the checkbox next to your toolpath will show the toolpath within the preview image

Click image for larger view. For smaller screens, click the expander icon in the top right of the pop-out window for the full size view.

Step 12 – Save the Toolpath

  • Click the ‘Save Toolpath’ icon
  • The Save Toolpaths interface will appear
  • Usually you will simply check ‘Output all visible toolpaths to one file
  • Set the Post Processor setting – Select ‘Mach2/3 ATC Arcs (inch) (*.txt)
This setting will now remain each time you use VCarve and will not need to be changed.

 

  • Click ‘Save Toolpath(s) to File
  • Name and save your filepath
This is the file (txt file) that you will open in Mach3.
HINT
Stay organized! Develop a filing system on your computer to ensure you know exactly where to find files and who they are for. Haste will make waste when you need to pull up a file and don’t remember where you put it or what you called it.

Click image for larger view. For smaller screens, click the expander icon in the top right of the pop-out window for the full size view.

Step 13 – Save the VCarve File

  • In the upper right under File click ‘Save As’
  • Name and save your file
Saving the file will allow you come back later and edit the toolpath, or create new toolpaths for different parts of the design
slide