Carbide Create User Guide
Carbide Create was designed to be a fully functional 2.5D CAD/CAM program to help users, without an existing CAD solution, get started using their CNC machine right away.
This document will take you through the features of Carbide Create and show you where to go to get started creating your own designs.
Here is a small sample of the projects you can make with Carbide Create
Woodworking: Cabinets, Embelishments, Custom Tool Holers, Inlays
Engraving: Plaques, Logos, Nameplates, Jewelry Boxes
Prototypes: Fixtures, Jigs, Functional Products
Customized Gifts: Coasters, Picture Frames, Key Rings, Knives, Tools
Sign Making: Businesses, Houses, Clubs, Offices
Carbide Create is not a 3D CAM package. 3D file formats (STL, STEP, IGES,) are not compatible with Carbide Create and require a different CAM package all together.
Carbide Create can make 2D and 2.5D parts by either drawing natively in the program, or importing existing design files from programs such as Illustrator, Inkscape, AutoCAD, or CorelDraw.
This software can import the following file formats: DXF and SVG.
Carbide Create has a clean interface which makes creating or modifying designs and toolpaths simple and straight forward. The program is broken down into 4 main parts
1.) The Menu Bar provides access to the traditional ‘open’ and ‘save’ commands. The Reset View button recenters the canvas on the screen.
Enabling Snap to Grid will force all control points to snap to the closes grid point.
2.) The Job Setup section is represented by the cog icon and provides access to change settings specific to each job, such as material size and type.
3.) The Design tab provides general drawing tools for design modification, sizing, alignment etc. prior to machining
4.) Toolpaths are created and edited through the Toolpath tab.
5.) The Canvas area of the screen represents your material and the 2D design you will be machining.
Access the Job setup pane by clicking the cog icon located by the top left corner of the screen. The Job Setup section provides access to change the specifics of your job. From here you can configure the material size and type along with setting the zero points of your job.
Define the stock size by inputing the actual size of your raw material or a known size for your design. Units entered here can be inches or millimeters, and are defined at the bottom of the job setup screen.
Stock Thickness defines how thick your material is. Utilize best practice by actually measuring your material and entering the actual value measured.
Set the Z-zero location by selecting ‘Top’ or ‘Bottom’ from the dropdown menu found in the Stock Thickness pane. Unless you have a specific reason, or know what you’re doing, always set z-zero to the top of the material.
Set the starting point of your job by selecting from teh dropdown menu in the toolpath zero section. Note the zero point of your job will be represented by the red/white circle shown here in the bottom left corner.
Set the machine and material by using the dropdown boxes. Selecting the appropriate material will allow Carbide Create to produce accurate speeds and feeds. Selecting the correct machine will define how large of a piece you can design, along with setting the automatic feeds and speeds correctly.
The retract height text box defines how high above the material the machine will retract in between toolpaths. If you have clamps or a special case where more (or less) retract is required, enter that value here.
From here you can change the grid size and gives you the option of importing a graphic as the background.
The units for grid spacing will be the same as the units you select on the main Job Setup screen.
Pro-Tip: Loading an image for a background is a quick and easy way to use an image as a reference to build a part or design by tracing. Once imported, the image can be scaled and the opacity can be increased or decreased to help aid in tracing or referencing.
Clicking this button will clear the canvas completely. You’ll be prompted to confirm, but if you click yes, there is no going back!
The design pane allows you to draw or modify your designs through the use of the vector shapes and tools. All designs are comprised of a combination of the available vector tools (described below). Each of these tools have different properties and options that can be selected and modified individually, at any time.
Circles can be created by clicking the circle icon in the design pane. Once clicked, you’ll be prompted to click the center point location of the circle, then drag out to define the diameter. Pressing escape will cancel the operation and send you back to the design pane.
Once the circle has been created, you can edit the circle by selecting the object with the cursor. Once selected, you can edit the circle’s properties by changing the values in the edit menu.
Elipses are not currently supported in Carbide Create
The move property allows you to position the circle on the canvas with absolute coordinates. You can position the circle by any of it’s quadrants or center point.
Click OK to apply the changes.
Squares and rectangles can be created by clicking the rectangle icon in the design pane. After clicking the rectangle icon in the design pane you’ll be prompted to click the target center point of the rectangle, then dragging out and up to define the rough size of the rectangle.
Once the rectangle is created you can edit the size (width and height) along with reposition the rectangle with absolute coordinates.
Dragging the rectangle on the canvas is a valid way to move the object as well. Notice as you drag the rectangle, the absolute coordinates will be updates in real time.
Rectangles can also be rotated to any angle after they have been created. Select the rectangle and under the orientation pane, enter the degree which the rectangle should be rotated. Click OK to apply the changes.
A polyline is a tool to create shapes by connecting straight lines at different points. Clicking the polyline icon will prompt you to click the first point on the canvas, then continue clicking on new points to create new segments of the polyline.
Pro-Tip: The color of the line is a visual indication of the status of the object you are creating. When the line is purple, the object is ‘open’ and cannot have a toolpath applied to it.
Afer the polyline shape is created, the shape is technically a polygon and can be edited by selecting the object and changing the values of the available properties in the edit menu.
The curve tool is similiar to the polyline tool with the added functionality of creating a curve between points. After clicking the curve icon in the design toolbox, you’ll be prompted to click the first point on the canvas. Just like polylines, move to and click the second point of your object - to create a curve, hold down the click and drag away from the point.
After creating your curve, click again to begin the next segment. Continue this process until your shape has been created.
Curves and Polygons have the a special editing tool called ‘node editing’. The node edit tool, available after selecting an existing curve or polygon, allows you to manipulate the individual nodes of a curve or polygon. Simply click on any node and drag to desired location.
Pro-Tip: Pressing escape on the keyboard will exit you from any of the edit modes.
Similiar to node editing, the curve edit mode allows you to adjust/modify existing curves. Select an object that has a curve, click the ‘node edit’ button to initiate node editing, then click the curve edit mode button to bring up editing handles for each of your curves.
Clicking the handles and pulling or rating the curve will allow you to redefine your curve. Press esc on your keyboard at any time to exit curve editing.
Regular polygons are the building blocks for most designs. Create a polygon by selecting the polygon tool and following the wizard to place your initial object.
Once placed, you can edit the object be changing the parameters in the edit pane on the left side of the screen. Polygons can be rotated, scaled, or placed by absolute coordinates, along with the typical drag and drop funcitonality found across all edit modes.
A special edit feature of polygons is the ability to change the number of sides. For example, entering a value of 3 will result in the polygon changing into a triangle, entering a value of 8 will create a traditional hexagon, etc.
Text can also be used in any of your designs. The full library of truetype fonts installed on your computer are available through the text design pane.
Once created, text can be adjusted by defining Height or Width, with the program keeping the other proportional when scaling.
Pro-Tip: applying a boolean operation to text will result in ‘exploding’ the characters into individual components!
Selecting more than one object will activate the Alignment Tools button on the left pane. After clicking the alignment tools button, you’ll presented with an entire pane of alignment options.
The bottom of the pane allows you to chose your reference point: align to stock material or align to the last object selected.
Pro-Tip: You can determine which object was the last object selected by looking at the highlighting. The last item will always be highlighted with a dashed orange line, where a typical selection is a solid orange line.
Carbide Create has 3 boolean options to help create accurate non-traditional shapes by combining regular shapes.
Union Combines two objects into one, leaving only the unique elements. Union can be performed on two or more objects. Also, objects that have already been union can be union again.
Intersection Uses the second object selected (with the dashed line) to cut through the first object, leaving only what is left from the first object after the cut.
Subtraction Only the features that overlap will remain. This is the opposite of the union feature.
The scaling operation can be used to proportionatly change the size of any object, or any group of objects. In the scale edit menu, you can adjust by entering a percentage value (1=100%, 2=200%, etc) or by adjusting the width or height.
Pro-Tip: Scaling comes in handy when importing files. If you DXF or SVG does not import at the correct size, use the scale feature to adjust accordingly.
The toolpath engine is the heart of Carbide Create. Within the toolpath view you can create and edit toolpaths which will turn your design from a simple 2D sketch into an actual part.
The word “Toolpath” is a term only found in CAD/CAM software and has little in terms of analogies in everyday life. A toolpath is basically the map the cutting tool will follow when making your part on the CNC machine.
By creating toolpaths, you are effectively creating the map.
There are 4 basic types of toolpaths to chose from within Carbide Create. Each type serves a different purpose and should be used in specific instances. We will go over the 4 types of toolpaths below and show examples of what they produce.
Pro-Tip: When creating toolpaths, it is helpful to keep in mind what you are doing: telling the bit where to cut. If you keep that in mind, and also remember that the bit (also referred to as a cutter or endmill) has a diameter that has to be offset, it will be easier to keep track of what you are doing.
Inside Cut - An inside cut will move the cutting bit to the inside of the object. Inside cuts are generally used for internal shapes and features. That is, if you are cutting a circle from the center of your part and want to maintain the the circle’s dimensions, you would want to select inside cut.
Outside Cut - An outside cut moves the cutter to the outside of the object. This is effectively the opposite of an inside cut and will result in the cutter being offset ot the outside of the line around the entire perimeter of the shape.
Outside cuts are generally used as profile cuts to cut away the perimeter of your part from the stock material.
Pocket - The pocket operation clears the internal area of a feature.
Pro-Tip: With Carbide Create, you can select multiple objects inside of an area to be pocketed. The toolpath engine will pocket around those objects. The features that are left over are referred to as islands
No Offset - The no-offset strategy is the equivalent of engraving. The center of the bit will be placed on the center of the line, no offsetting will occur. Your bit will follow the center of the line around the entire perimeter of the shape.
Visual Guides and real-time recalculating
Carbide Create places blue lines around the features that will be machined. The blue lines represent where the center of your cutting tool will travel while your job is running. You can see the blue lines after switching back to the design view.
While in design view, if you were to modify any of the shapes within the design, there is no need to re-calculate the toolpaths, Carbide Create will take care of that for you.
When you are in the toolpath section of the program, the toolpaths have already been created will be represented by shading. Toolpaths that cut deeper into the material will be shown as darker and shallow cuts will be lighter. Where white is a cut that barely cuts through the surface and black is a cut that goes all the way through the material.
- Inside Cut
- No Offset Cut
- Outside Cut (2 examples in images)
The image above shows all 5 types of toolpaths, the 4 defined earlier plus v-carving, which is talked about in detail in a following section.
Notice the 3 Circles in the center of the design. All 3 of the circles were drawn to be 1” in diameter.
- The circle on the left (3) is an inside cut
- The circle in the center (4) is a no offset cut
- The circle on the right (5) is an outside cut
If you look at the shaded lines that represent where to tool will cut, you will notice that the circles are increasing in size! The cuts where the bit is not on the inside will create a circle that is larger than 1” in diameter.
Here is the 3D preview of the same part, it is clear to see that the circles 4 & 5 are going to be larger than the intended 1” diameter because of the toolpath type that was selected.
Each toolpath (with the exception of v-carving) allows you to set the max depth of that specific operation. The max depth tells the program how deep you want to cut the feature.
Pro-Tip: If your feature goes all the way through the material, you can select ‘Use Stock Bottom’ to autofill the thickness of the material.
Feeds and Speeds
Not only does Carbide Create have a powerful toolpath engine, it also contains pre-defined speed and feed information for more than a dozen materials!
Part of setting up your job requires you to select the material you’ll be using. Selecting the correct material (or closest) to the material you’ll be using is important for both vizualization AND to properly calculate the speeds and feeds.
The second component to the calculation is the cutting tool you select.
By clicking EDIT under any of the toolpath menus you can access the feed and speed settings. Although Carbide Create calculates these automatically, you can override the auto calculations and run the machine at your own feed and speed settings.
Carbide Create has a pre-defined tool library containing all of the most common cutters.
These cutters are numbered to match the numbering system we use for the cutters sold through the Carbide3D online shop.
- The 100 series cutters have a 1/8” shank
- The 200 Series cutters have a 1/4” shank
- The 300 Series cutters are v-bits and other specialty shapes
Adding new tools
Although the library is full of commong cutters, you may eventually find the need to add your own. To do so, click the ‘Edit Library’ link found below the endmill selection dropdown box. This will pop open a new window containing the details of your library.
To add a new tool click the Add Tool button at the lower left corner. This will populate your library with a new tool
To define the parameters of your new tool, double click the new tool name. After you double click the name, your new tool will become editable and you can fillin the appropriate details for each property.
Pro-Tip: You must double click the tool (or right click->Edit) to actually change the values of the tool. After changing values, click the OK button to submit the changes to the library.
Simulation / 3D Preview
Carbide Create comes with built in 3D preview functionality. Once you have a created at least one toolpath, you can cselect a representative material from the Toolpath Simulation menu and then click the ‘Show Simulation’ link to generate a full 3D preview of your part!
Once the preview is created, full manipulation is available through the mouse. You can rotate, zoom, and pan the preview.
- Left Click - Hold and drag to rotate
- Scroll Wheel - Zoom in / Zoom Out
- Right Click - Pan
- Reset View - Will reset the 3D in preview mode.
Click the hide simulation button to go back to 2D mode.
V-carving is a special type of toolpath that uses v-shaped bits to create features that vary in width and depth.
To create v-carving features, select an object on the screen and under the toolpaths menu, select v-carving. Make sure you have a v-carving bit in your library (or create one) and ensure you have selected this bit as your tool.
The toolpath engine will find the center point of each of your objects and determin the depth based on the width of your feature.