Search the Knowledge Base
CNC Workflow Using Vectric VCarve / VCarve Pro for CNC
1.0 Introduction
The CNC (Computer Numerical Control) workflow is a systematic and highly precise process that transforms digital designs into physical objects through automated machining. This advanced manufacturing method offers unparalleled accuracy, repeatability, and efficiency, making it a cornerstone in industries ranging from aerospace and automotive to prototyping and custom manufacturing.
This manual provides an overview of the initial phases of the CNC workflow i.e. CAD (Computer Aided Design) and CAM (Computer Aided Manufacturing) using Vectric VCarve / VCarve Pro. This manual will help you to kickstart your CNC machining journey using Vectric VCarve / VCarve Pro and will demonstrate the use of this tool to create a 2.5D model (CAD) and toolpaths (CAM) of a coaster.
1.1 Vectric VCarve / VCarve Pro
Vectric VCarve / VCarve Pro is a software package designed for CNC machining. It’s primarily used for creating 2D and 3D models and generating toolpaths that carve or cut intricate designs into various materials like wood, metal, plastic, and more.
The user interface (UI) of Vectric VCarve / VCarve Pro is straightforward to navigate. Upon opening the software, you’ll encounter a screen similar to the one depicted in Figure 1.
Click on the image(s) to expand
Main Window:
Toolbar: The main window has a toolbar at the top, through which a user can access different menus such as File, Edit, Machine etc. The toolbar is indicated by a red rectangle in Figure 1.
Browser: A browser tab (marked by the blue rectangle in Figure 1) on the left, that allows a user to create a new project, open any existing projects and access video tutorials and resources.
Job Setup Window:
Job Setup: To start a new project click on Create a new file and a Job Setup window will appear, as shown in Figure 2. In this window a user can set the outer dimensions, thickness of the material/workpiece. The job setup window is indicated by the orange rectangle in Figure 2. After the job setup has been completed, click on OK and the drawing canvas indicated by the blue rectangle in Figure 2 will adjust to the job size.
Click on the image(s) to expand
Click on the image(s) to expand
Part Design Window:
After the job setup has been completed, a part design window will pop up indicated by the red rectangle as shown in Figure 3. This window contains different tabs such as Drawing, Modelling, etc that enable a user to create 2D Sketches and generate 3D models. To the top right-hand side of the same window is another tab called Toolpaths (indicated by a black rectangle in Figure 3) that enables a user to create toolpaths for the desired part.
2.0 Workflow
The CNC Workflow is divided into three main phases:
- Design Phase: Designing and creating a CAD (Computer Aided Design) model of the desired part.
- Program Phase: CAM (Computer Aided Manufacturing), creating Toolpaths/G-Codes for the machining of the desired part.
- CNC Phase: Using a CNC machine to cut the designed part from a workpiece.
This manual will discuss and demonstrate the first two phases i.e. Design and Program using Vectric VCarve / VCarve Pro to make a coaster, details of which are shared below:
2.1 Design Phase: Designing and CAD Modelling
The process starts with the designing of the intended part by specifying the dimensions and features of the part. This manual uses the example of a coaster that has a Maker Store logo in the centre, to demonstrate the CNC Workflow using Vectric VCarve / VCarve Pro. The coaster is shown in Figure 4 below.
Click on the image(s) to expand
The dimensions of the coaster are:
- Length = 100mm
- Width = 100mm
- Thickness = 12mm
- Corner Radius = 10mm
- Material = Wood – Pine
Follow the below steps to design the above coaster in Vectric VCarve / VCarve Pro:
Step 1: Open Vectric VCarve / VCarve Pro and under Startup Tasks click on Create new file. Please see Figure 5 for reference.
Click on the image(s) to expand
Step 2: Enter the job dimensions and other parameters as shown in Figure 7 and click on OK. Please see Figures 6 & 7 for reference.
Click on the image(s) to expand
Step 3: Under the Drawing tab, select the Rectangle icon highlighted in red. See Figure 8 for reference.
Click on the image(s) to expand
Step 4: Select the top left corner in the Anchor Point tab. Choose Corner Type as Radiused External and enter the radius as 10mm to create the rounded edges. Under the Size tab, enter Width and Height = 100mm. Click on Create and then Close. See Figure 9 for reference.
Click on the image(s) to expand
Step 5: Under the Drawing tab, click on Text. In the rectangle created on the canvas, click at any desired place you want to place the text (near the top edge). In the Text window on left, type in MAKER as the text. Select your desired font and set the Text Height = 10mm. Click on Close. See Figures 10 & 11 for reference.
Click on the image(s) to expand
Step 6: Double click on the MAKER text vector on the canvas and under the Edit tab in the toolbar select Align Selected Objects. Under this menu select Center Horizontally in Material. This will align the selected text horizontally. See Figure 12 for reference.
Click on the image(s) to expand
Step 7: Create the text STORE near the bottom edge of the rectangle by repeating steps 5 & 6. See Figure 13 for reference.
Click on the image(s) to expand
For the next step, you will need the Maker Store Gear Logo for the coaster. For your convenience, a vector file of the logo has been provided. Please download and unzip the Maker Store Gear Logo vector by clicking on the blue Download button below.
Step 8: Click on File on the toolbar and select Import → Import Vectors. Select the Maker Store Gear Logo file downloaded earlier and click on Open. See Figures 14 & 15 for reference.
Click on the image(s) to expand
Click on the image(s) to expand
Step 9: Resize the gear logo by double-clicking on the logo and dragging one of the corners. Place the logo in the centre of the rectangle. Align the gear logo in the centre of the rectangle by pressing the F9 key on your keyboard. See Figures 16 & 17 for reference.
Click on the image(s) to expand
Step 10: Click on File tab in the toolbar and select Save. Choose the desired location, name the file and click on Save. See Figure 18 for reference. If you are working on a larger project it is recommended to save the progress of your work often.
Click on the image(s) to expand
Congratulations, you have completed the Design and CAD Modelling phase of the CNC Workflow using Vectric VCarve / VCarve Pro.
2.2 Program Phase: CAM (Computer Aided Manufacturing)
CAM (Computer Aided Manufacturing) is the second phase of the CNC Workflow, wherein toolpaths/G-Codes are generated. Toolpaths are cutting instructions that are provided to the machine via the controller. The toolpaths are stored in the form of codes called G-Codes (Geometric codes). A translator also known as a post-processor is used to translate the toolpaths into the correct G-Code format.
The post-processor to be used depends on the controller being used. For example, if you are using a Grbl-based controller, such as the xPRO V5 controller, then you have to use a Grbl post-processor. If you are using an AXBB-E controller, you will be using the UCCNC post-processor. Different controllers will generally require different post-processors.
This step of the workflow requires the use of tools (end mills) and a post-processor. All the information about tools is stored in a tool library. Maker Store has created a tool library for all its tools which have pre-set speeds and feeds to get you started with CNC machining.
Please download and unzip Maker Store’s Vectric Tool Library here.
Please download and unzip Maker Store’s Vectric Post Processor for Grbl here.
The above tool library and post processor will work with all the Vectric softwares.
To create toolpaths for the above-modelled coaster, follow the steps mentioned below:
2.2.1 Importing Maker Store Vectric VCarve / VCarve Pro Tool Library
Step 1: After you have downloaded the Maker Store Vectric tool library from the above-mentioned link, click on the Toolpaths tab in the toolbar. Select Tool Database. See Figure 19 for reference.
Click on the image(s) to expand
Step 2: Click on Import a tool database button at the bottom of Tool Database window. Select the downloaded Maker Store Vectric Tool Library file and click on Open. See Figures 20 & 21 for reference.
Click on the image(s) to expand
Step 3: Next click on Merge. The imported tool library will appear in the Tool Database window. See Figures 22 & 23 for reference.
Click on the image(s) to expand
Congratulations, you have successfully imported the Maker Store Vectric VCarve / VCarve Pro Tool Library.
2.2.2 Importing Maker Store Vectric VCarve / VCarve Pro Post-Processor
Step 1: Under Machine tab in the toolbar, select Post Processor Management. See Figure 24 for reference.
Click on the image(s) to expand
Step 2: Click on the Install Post Processor to custom Post Processor directory button at the bottom of Post Processor Management window and select the downloaded Maker Store Vectric Post Processor file. Next click on Open. See Figures 25 & 26 for reference.
Click on the image(s) to expand
Step 3: A new message window will appear saying if you would like to make this post processor as the default post processor. As per your liking select Yes or No. Next click on Close. See Figures 27 & 28 for reference.
Click on the image(s) to expand
Congratulations, you have successfully imported the Maker Store Vectric VCarve / VCarve Pro Post Processor.
2.2.3 Creating Toolpaths
In this section, we will generate the toolpaths and select the appropriate tools for carving the coaster design. Vectric has a range of toolpaths that can be used. Each toolpath type is unique and corresponds to the features on the workpiece.
It is important to note the order of operations that you must undertake to machine the part to reduce tool changes and therefore machining time. In this project, we will use the V-Carving tool path first to carve the text with a V-Shaped tool. We will then cut the gear pocket with the Pocketing toolpath and cut the coaster out of the stock using the Profile toolpath. In total it will be two tool changes.
Step 1: Hold the Shift button on your keyboard and select the two text vectors “MAKER” and “STORE“. Click on Toolpaths tab at the right side of the window and select V-Carve/Engraving Toolpath. See Figure 29 for reference.
Click on the image(s) to expand
Step 2: Under the Tool section of the V-Carve/Engraving Toolpath, click on Select. Next, in the Tool Database window under Maker Store Vectric Tool Library, select V-Bit (90° – 22 mm Diameter) #188 endmill. Click on Select. See Figures 30 & 31 for reference.
Click on the image(s) to expand
Step 3: Under Project toolpath onto 3D model section, type in Name (name of toolpath) as Coaster Text 188. This name will help in easy identification of the end mill required for the operation. See Figure 32 for reference.
Click on the image(s) to expand
Step 4: Next, a window will appear in the 3D view tab. Hold and move around the Left mouse button to rotate the 3D model. You can see the simulation of the V-carve / Engraving operation by clicking on the play button. After viewing the simulation, click on Close. If you wish to edit the sketch, click on 2D View tab. See Figure 33 for reference.
Click on the image(s) to expand
See the simulation of the V-carve / Engraving operation below:
Step 5: In the 2D View Tab, select the Gear Logo vector. Under the Toolpaths tab, click on Pocket Toolpath. See Figure 34 for reference.
Click on the image(s) to expand
Step 6: Under the Cutting Depths section enter Cut Depth = 3mm (as per the design). In the Tools section, click on Select. Next, in the Tool Database window under Maker Store Vectric Tool Library, select 2 Flute Down-Cut 6mm – #100 end mill. Click on Select. See Figures 35 & 36 for reference.
Click on the image(s) to expand
Step 7: Select the Cut Direction as Climb. Tick the Ramp Plunge Moves and set the Distance = 5mm. Name the toolpath as Coaster Pocket 100. Next click on Calculate. See Figure 37 for reference.
Note: Contrary to plunging, ramping makes the tool engagement with workpiece to be gradual which prevents blunting of tool. Climb milling is the most favourable method of milling as it provides a better finish and generates less heat in the tool.
Click on the image(s) to expand
Step 8: To play the simulation click on the play button. See Figure 38 for reference.
Click on the image(s) to expand
Step 9: In the 2D View tab, select the rectangle vector. Under Toolpaths tab, click on Profile Toolpath. See Figure 39 for reference.
Click on the image(s) to expand
Step 10: Under the Cutting Depths section enter Cut Depth =12.5 mm. In the Tools section, click on Select. Next, in the Tool Database window under Maker Store Vectric Tool Library, select 2 Flute Down-Cut 6mm – #100 end mill. Click on Select. See Figures 40 & 41 for reference.
Note: Since wood is a natural product, the thickness generally varies even though it will be stated as 12mm. In order to account for this variation, the cut depth is selected as 12.5mm in the above operation.
For this toolpath we are using the same end mill as the previous toolpath to minimise the number of tool changes resulting in an efficient workflow.
Click on the image(s) to expand
Step 11: Click on the Edit Passes button and change the Number of Passes to 4. Click OK. See Figures 42 & 43 for reference.
Click on the image(s) to expand
Step 12: Under the Machine Vectors section, select Outside / Right. Select Direction as Climb. Tick the Do Separate Last Pass and set Allowance (A) = 0.15mm. Tick the Reverse Direction. See Figure 44 for reference.
Note: The Reverse Direction under last pass executes the last/final pass in opposite direction which results in a better finish.
Click on the image(s) to expand
Step 13: Tick the Add tabs to toolpath. Enter Length = 6mm and Thickness = 3mm. Click on Edit Tabs. See Figure 45 for reference.
Click on the image(s) to expand
Step 14: Under Specify tabs set Constant Number as 2. In the Placement section select Avoid corners and curved regions, and click on Add Tabs. In the 2D View tab click on the two points on rectangular profile as shown in Figure 46. Click on Close.
Click on the image(s) to expand
Step 15: Tick Add ramps to toolpath and set Distance = 5mm. Enter Name as Coaster Profile 100. Click on Calculate. See Figure 47 for reference.
Click on the image(s) to expand
Step 16: A warning message will appear regarding the depth of cut being more than the material thickness. Since we are using a sacrificial board underneath our workpiece, it won’t damage the machine bed. Click OK. See Figure 48 for reference.
Click on the image(s) to expand
2.2.4 Post Processing
The final phase in generating the toolpaths is post-processing, which involves using the Post Processor downloaded earlier to create toolpaths/G-codes.
Step 1: Under the Toolpaths section, all the created toolpaths will be visible. You can drag/drop to change the position of toolpaths. However, the sequence of the toolpaths is very important.
Select the first toolpath i.e. Coaster Text 188 and click on Save toolpaths button. Under Post Processor select Maker Store Vectric Post Processor Grbl and click on Save Toolpath. See Figure 49 & 50 for reference.
Click on the image(s) to expand
Step 2: Choose the desired location and name the file as Coaster Profile 100. Click Save. See Figure 51 for reference.
Click on the image(s) to expand
Step 3: To view the simulation of all the operations together, select all the toolpaths and click on Preview Toolpaths. Next click on Reset Preview and then select Preview All Toolpaths. See Figures 52 & 53 for reference.
Note: If you wish to make changes to your model, click on 2D View tab and edit the sketch/model. and then right-click on any of the toolpaths and select Recalculate → Recalculate All.
Click on the image(s) to expand
Click on the graphic below to view the final simulation:
Step 4: Next, select the next two toolpaths, first Coaster Pocket 100 and then Coaster Profile 100 (sequence is important). Under Post Processor select Maker Store Vectric Post Processor Grbl and click on Save Toolpath(s). Next, choose the desired location (same folder as the first toolpath), name the file as Coaster Pocket & Profile 100 and click Save. See Figures 54 & 55 for reference.
Note: To create an efficient workflow, deciding the order of operations is essential, as it will save time and money. The Coaster Profile 100 toolpath needs to be executed at the last as this is the piece that holds the part with the workpiece. Moreover, the Coaster Profile 100 and Coaster Pocket 100 toolpaths use the same end mill, i.e. 2 Flute Down-Cut 6mm – #100, so it is logical to execute these toolpaths one after the other and for the same reason their Toolpaths have been combined. The Coaster Text 188 uses end mill Ø22mm 45° (90° V-Router Bit 22mm) – #188 and hence will be executed first. Therefore the order of operations will be:
- Coaster Text 188 (V-carve / Engraving)
- Coaster Profile 100 (Pocket)
- Coaster Profile 100 (Profile)
Click on the image(s) to expand
Congratulations, you have successfully completed the CAM phase of the CNC workflow.
Support
For any questions or concerns, please contact us at [email protected]
Australian customers: For more project ideas and solutions, please visit makerstore.com.au
North American customers: For more project ideas and solutions, please visit makerstore.com.cc
UK and European customers: For more project ideas and solutions, please visit makerstore.co.uk
Credits
- Maker Community.
- Our fantastic customers, whose feedback constantly helps improve our proceses and guides.