Hey there, Maker!

Welcome to the CNC series of Snapmaker Academy. The previous five episodes focus on the CAD and CAM processes. Now, it's time to dive into practical machining.

We already understood that CNC machining works by removing material from a solid workpiece to achieve the desired geometry. The toolpath (or G-code) instructs the cutting tool (aka bit) on how to move, while the cutting tool engages with the workpiece to produce the outcome.

Just like you wouldn't use a dagger to chop ribs, various cutting tools are designed to cut out different geometries. Choosing the right cutting tool is critical to your project's efficiency and even success. Therefore, this article aims to introduce the basics of cuttings tools and walk you through some of the most commonly used router bits.

First, let's get to know the major features used to categorize a cutting tool.

Basic Terminologies

Flutes/Teeth

Teeth refer to the cutting edges, and flutes are the grooves formed between teeth. As the bit rotates, teeth are responsible for cutting materials off, while flutes help evacuate the chips (namely removed materials) from the workpiece. Though not to be taken as the same thing, these two terms are usually interchangeable since they are always identical in number.

Number of Flutes

The number of flutes on your router bit impacts the work speed and the surface finish of your product. Having more flutes offers two main advantages. First, it adds to the strength of the bit, which means the bit can be fed into the workpiece faster and work on harder material. Secondly, bits with more flutes tend to give a better surface finish.

Bits of different numbers of flutes

However, this doesn't mean you should try to go for as many teeth as you can. To explain this, we need to introduce a new concept: chip clearance. Flutes serve as the passage for chips to evacuate, and chip clearance is the amount of space that a single flute takes up. When the number of flutes increases, chip clearance (i.e., the passage) gets smaller, hence the more difficult for the chips to be evacuated. Yet, if you can't get the chips out in time, the heat produced during cutting will build up, eventually destroy the bit and even lead to burning. This is especially the case for materials like aluminum which produces large and sticky chips. That's why you should try to find the balance when deciding the number of flutes.

Type of Flutes

There are two common types of flutes: straight and spiral.

• A straight flute is parallel to the shank of the bit, striking the surface of the material perpendicular to the rotation direction. Straight bits are stronger than spiral bits and can be used at higher speeds. On the other hand, they produce less smooth surface finish on the workpiece since such design brings more chatter. They are commonly used for slotting and cutting straight contours.

Straight flutes vs. Spiral flutes

• A spiral flute goes along the shank of the bit spirally, staying in constant contact with the material surface. Such design allows less chatter and leaves the finished surface smoother, making these kinds of bits ideal for trimming surfaces. However, spiral bits are weaker when held against straight ones and cannot cut too deep into the material or work at very high speeds.

Geometries

Shape of Tip

Router bits come in a variety of tips, each creating different shapes of cuts as they engage with the material. Some of the most common types you will find are flat, ball-nose, and chamfer.

• A flat (or square) tip got a nearly 90-degree angle between its circumference and the end surface.
• A ball-nose tip has a sphere-shaped end, as its name suggests.
• A chamfer tip is a sharp conical tip. Chamfer bits are also called V-bits for their tips looking like the letter "V".

Upcut vs. Downcut

Spiral flutes can be further divided into two categories: upcut and downcut. The differences between the two types of spirals are crucial because they determine the direction in which chips are evacuated.

The spiral flutes of an upcut bit wrap around the body of the bit clockwise, pulling chips away from the workpiece being cut. An upcut bit tends to leave a rough surface finish on the top of the workpiece and a smooth surface on the bottom.

A spiral downcut bit, however, pushes chips down as it's cutting, with the flutes wrapping around the bit counterclockwise. Conversely, a downcut bit leaves a cleaner cut on top but a fuzzy surface at the bottom.

It's worth noting that you should always use an upcut bit for plunging operations unless you know what you're doing, especially for thicker materials. The reason is when a downcut bit plunges straight down, the chips have nowhere to go but to grind against each other as the bit spins, which is going to create friction and even start a fire.

Center Cutting vs. Non-center Cutting

Router bits are either center cutting or non-center cutting. The cutting edges of a center cutting bit go all the way into the center, whereas those of a non-center cutting bit leave a hole in the center. Center cutting bits can plunge straight down into the material, while non-center cutting bits cannot.

If a non-center bit were to plunge into the material, the material engaging with the hole in the cutting edges remains uncut, which can break the bit and lead to burning. To use these bits, you need to drill a pilot hole or use ramp plunge moves. Perhaps the only good reason to buy non-center bits is they are cheaper.

Size

Basically, size determines what you can do with any given router bit. Large ones are good at cutting a lot of material, but it comes at the cost of details. Smaller bits provide higher resolution in detail, with a trade-off in strength and machining efficiency.

Overall Length

The overall length is the distance between one end of a bit to the other. Longer bits are able to reach down deeper into the material. Now, you might believe that having longer bits sounds like a safe bet since they offer more choices. Unfortunately, that's not the case.

This brings us to a concept called "stickout". Stickout refers to the distance from the end of the collet (i.e., tool holder) to the bit's tip. It's this part of the bit that works without support. The more stickout, the less rigid a tool is. If it sticks out too far, the bit is prone to be bent by the cutting force.

Cutting Length

As we can see, cutting edges (or flutes) cover only a portion of the bit. The cutting length (also called "flute length") of a bit determines how deep it can cut into the material. Note that the cutting depth should never exceed the flute length of your bit. Otherwise, chips won't be pulled out properly, and your bit could be damaged by the heat accumulated.

Shank Diameter

The shank diameter is the width of the non-cutting end of the tool. This is the diameter that will go into your collet. Common shank sizes are 3.175 mm (1/8 inch) and 6.35 mm (1/4 inch).

Cutting Diameter

This is the diameter of the cutting end of your router bit. It is often the first thing to look for when choosing a tool for your job, as it determines the resolution of cutting.

When cutting, the cutting edge will leave a circular profile in every internal corner, with a radius equal to half its diameter. Also, it is impossible to cut out features that are smaller than the cutting diameter because bits are cylinders (except for V-bits). Say, you can never have a slot that is 2 mm wide using a typical bit with a cutting diameter of 3.175 mm.

On the other hand, a bigger cutting diameter makes your bit more rigid, allowing deeper cuts. Besides, bits with a larger cutter diameter can remove more material per unit of time, which means you can do the same job faster.

Common Router Bits

There are literally tens of thousands of tool types and variations available for CNC machines. Covering every type and use is beyond the scope of this article. We will introduce the most commonly used router bits.

Before diving in, we need to clarify the differences between milling bits and drill bits. Milling bits, including end mills, face mills, and v-bits, are designed to cut with their cutting edges as they move laterally through the material. By contrast, drill bits are intended to be used for drilling holes, plunging straight down into the material.

End Mill

End mills are designed to cut with their cutting edges on the circumference of the bit, but they do have cutting edges on the end surface too. Though center-cutting end mills are capable of plunging straight down, such operations could be demanding for them and should be avoided if possible.

Flat End Mill

With a nearly 90-degree angle between its circumference and end surface, a flat end mill is going to create neat square corners at the bottom and a flat surface anywhere it passes over the top of. They are great for removing large amounts of material, widely used for everything from roughing to cutting pockets and 2D contours.

Flat end mill

Ball-nose End Mill

The circumference and the end surface of a ball-nose end mill form a rounded corner. The radius of that round corner equals the cutting radius (i.e., half of the cutting diameter). These mills excel at creating curvature or detail-rich 3D shapes like relief.

Ball-nose end mill

Since their tips are round, cutting out a perfectly flat surface is challenging for these bits because they will leave scallops on the workpiece.

Bull-nose End Mill

You can see bull-nose end mills as a transition between flat and ball-nose ones. The radius of its round corner is smaller than the cutting radius. Since they combine a flat bottom with round corners, they can create flat-bottomed pockets with rounded corners at once without changing tools.

Bull-nose end mill

Roughing End Mill

Roughing end mills have many serrations on the cutting edges to quickly break up chips, which is great for efficiently removing a large amount of material. The thing with roughing end mills is that they will leave a poor surface finish with corncob-looking tracks on your workpiece, and that's why they are often referred to as corncob end mills. Hence, roughing end mills are for roughing only.

Roughing end mill

Face Mill

Face mills are designed to cut with their cutting edges on the end surface of the bit. They often come with multiple cutting edges that are replaceable, which allows removing more materials at higher speeds. These kinds of mills need powerful spindles to push them.  These mills are mostly used for creating a large and smooth flat face on the surface of a plate or bar workpiece. 

Face mill

V-bit

V-bit, also known as chamfer mills, are used for chamfering, deburring edges, and letter engraving. They are not so good at cutting profiles or carving out pockets since they'll leave a sloped surface on the workpiece.

V-bits are available in many sizes and angles, although 90, 60, and 30 degrees are most common. A smaller angle often comes with a smaller cutting diameter, supporting shallower cuts while retaining more details. A bigger angle allows wider cutting diameter and deeper cuts.

V-bits in different sizes

Drill Bit

Drill bits are designed to bore straight down into the material with their pointed tip. Unlike milling bits, their flutes only function as the passage for chips to be pulled out. They are often used for pre-drilling holes for screws.

Drill bit

Summary & Next Up

This article introduces some of the most commonly used router bits on top of explaining the basic terminologies used to describe cutting tools. And that is the foundation for us to look into setting parameters for cutting jobs in the future. We hope it could be helpful for you!

In the next episode, we are going to introduce some of the most common features of a model that you might encounter and then exemplify how to choose the right router bits for a CNC project. Please stay tuned!

Hey there, Maker!

This article breaks into two parts. In part 1, we learned the concepts of CAD, CAM, post processor, and firmware, as well as the CAM workflow of Fusion 360 in detail.

In this part, we will continue with other CAD/CAM software picks: FreeCAD, Aspire, and Carveco Maker (formerly ArtCAM). We will also briefly introduce two easy-to-use CAM software picks: Snapmaker Luban and MeshCAM.

CAM Software

 This article only focuses on the CAM features of the software introduced. To learn more about their CAD-related features and highlights, see CAD for CNC: Eight 3D Modeling Software Picks to Visualize Your Ideas.

FreeCAD

FreeCAD is a free 3D modeling software with a strong suit for designing solid models. Once a model has been created, you can switch to Path Workbench to generate the toolpath and G-code.

 If you're using FreeCAD to design models for the first time, you need to download and import the post and tool library to ensure that the G-code that is to be generated can be successfully exported to Snapmaker CNC Carving Module for further processing. 

• To import the post, copy the .py file to the Mod\Path\PathScripts\post folder in the installation directory of FreeCAD.
• To import the tool library in the latest FreeCAD 0.19, perform the following steps:

1. Click Edit > Preferences > Path > Job Preferences > Tools. Select Use Legacy Tools, and click OK.
2. Switch to Path workbench. Click  > Import. Select the .json file in the FreeCAD folder of the post and tool library and click Open.

Import a tool library in FreeCAD - 1

Import a tool library in FreeCAD - 2

Click  to set up the basic configurations of your carving job. In the Output tab of the Job Edit panel, you can enter a name and extension for the G-code file to be generated and select the post in the Processor bar. In the Setup tab, you can define the dimensions of the stock in relation to the model and the location of work origin. In the Tools tab, you can select the tool for your carving job.

 The extension for G-code files that Snapmaker CNC Carving Module can recognize is .cnc.

After performing these basic configurations, you can select different features of the model in the tree diagram on the left and apply different machining strategies to generate separate toolpaths for each of them. For example, for the outer profile of your model, select a strategy that can quickly cut through the material, whereas for sunken areas, opt for a strategy that can efficiently remove the material. While generating toolpaths, FreeCAD allows you to preview how the tool moves and what the finished product looks like, so that you can make adjustments in real time.

Simulation in FreeCAD

If you know your way around G-code, you can click  to inspect the G-code content of a path and view or directly edit the G-code in the text box that appears. Once everything is set, click  to post process the selected job and generate the G-code specific to Snapmaker CNC Carving Module.

Here are two great tutorial videos that you can check out: FreeCAD - The Powerful Path Workbench for CNC Machining and G-code and Ultimate Free CNC CAM tutorial with FreeCAD.

Aspire

Aspire is a reputable wood relief design software with powerful CAM features.

With Aspire, the first step of modeling is setting the coordinate system and the stock parameters. When creating a project, you need to specify Job Type, Job Size, work origin (i.e., XY Datum Position, and Z Zero Position), and Orientation in the Job Setup pane first. Aspire supports four-axis CNC carving. To work with Snapmaker Rotary Module, just select Rotary in Job Type.

 If you're using Aspire for the first time, you need to download and import the post and tool library to ensure that the G-code can be successfully exported to Snapmaker CNC Carving Module for further processing.

• To import the post, open Aspire, click Toolpaths > Install Post Processor..., and click the .pp file in the Aspire folder of the post and tool library. (There are two files with the .pp extension in the folder, one for three-axis machining and the other for four-axis machining. You can import only one post at a time.)

Import a post in Aspire

• To import the tool library, open Aspire, click Toolpaths > Tool Database, and click Import. Then, open the Aspire folder of the post and tool library and select the .tool file.
  

Import a tool library in Aspire - 1

Import a tool library in Aspire - 2

After you finish modeling, click on the top left to proceed to set up toolpaths by configuring the parameters in the Toolpaths pane that appears on the right. You can modify the previously set stock parameters in the Material Setup panel at the top.

Next, you get to choose appropriate machining strategies for different features of the model. In relief carving, for example, we apply rough machining to carve out the general outline and then use finish machining for the details. In these two rounds of machining, different tools and machining strategies are required, which are to be generated as corresponding toolpaths. In the Toolpaths pane, click Select to pop up the Tool Database window, where you can select the tool to use. Click Edit to set machining parameters such as spindle speed, feed rate, and stepover. When you’re done with setting the parameters, click Calculate to generate toolpaths.

After the toolpath is generated, click Preview Selected Toolpath to visualize how the tool moves and what the finished product looks like. Should you need to adjust the toolpath, the operation is pretty easy. Double click the toolpath on the right, and the parameter setting window then appears.

Simulation in Aspire

When all is set, click  to generate the G-code. The post that you have imported earlier will appear in the Post Processor bar. Click Save Toolpath(s), and the G-code customized for Snapmaker CNC Carving Module will be generated.

As a top choice for CNC relief design, Aspire comes with well-made official training videos. You can also find many videos made by users on YouTube and other platforms, such as Vectric 3D Carving & Toolpath Tutorial for Vcarve & Aspire and Basic Guide to CNC with Vectric Vcarve Pro / Aspire Profile Toolpath.

Carveco Maker

Our last guest is Carveco Maker created by the team behind ArtCAM. If you're familiar with ArtCAM, you will quickly pick up on Carveco Maker, as it draws heavily from its predecessor.

In Carveco Maker, two separate steps are required to set the stock dimensions. The width and height are defined when you create a new project, whereas stock thickness is defined in the window where you configure toolpath parameters. By default, the work origin is the center of the stock. You can modify it by clicking Model > Set Position (P) in the top navigation bar. After you finish modeling, click Toolpaths in the tree list on the right to start setting the machining strategies and toolpath parameters.

 If you're using Carveco Maker for the first time, you need to download and import the post and tool library to ensure that the G-code can be successfully exported to Snapmaker CNC Carving Module for further processing.

• To import the post, copy the .con file in the ArtCAM folder of the post and tool library to the postp folder in the installation directory of Carveco Maker.
• To import the tool library, after you finish modeling in Carveco Maker, click Toolpaths in the Project panel and then click in the Toolpath Operations panel to enter Tool Database. In the pop-up window, click Import.., select the .tdb file in the ArtCAM folder of the post and tool library, and click Open.
  

As with the previous software, different machining strategies are needed for different features of the model in Carveco Maker. After you select a feature, choose the way you want it to be machined by clicking the corresponding button on the Toolpaths pane to the right. In the pop-up window, you can select a tool and set its machining parameters, such as feed rate, stepover, and cutting depths. As mentioned previously, this window is also the place where you can define stock thickness. After finishing setting, you can run a simulation to view the processing results.

Simulation in Carveco Maker

After you finish configuring toolpaths, click Toolpaths in the tree list of the Project panel. Then, in the Toolpath Operations panel below, click  to save your toolpath. In the pop-up window, select the post processing method that has been imported in the drop-down list of Machine file format, and click Save to export the G-code. Now, we can send the G-code to the CNC machine for carving and simply wait for the finished product.

The Carveco Maker team has already made a series of official training videos, such as Carveco Maker - Designing A Plaque (part one) and Carveco Maker - Machining A Plaque (part two), covering the most common basic operations. The two videos here use the example of making a plaque to demonstrate the entire procedure, from designing a sketch to setting the toolpaths and exporting the G-code. Also, ArtCAM users have made a large amount of tutorials resources that are helpful for using Carveco Maker, as the two pieces of software practically share the same working logic.

Snapmaker Luban & MeshCAM

That's all for our introduction to CAD/CAM software picks. Sometimes, we have already finished the model design and simply want to turn it into toolpaths. This is where software dedicated to CAM comes in. So, let's take a look at two CAM software picks: Snapmaker Luban and MeshCAM.

Snapmaker Luban is free and open-source CAM software developed by the Snapmaker team. Tailored specifically to Snapmaker 3-in-1 3D Printer, it is designed with user-friendliness in mind around three major functions: 3D printing, laser engraving and cutting, and CNC carving. Needless to say, the CAM features of Snapmaker Luban match Snapmaker hardware with perfection. The toolpaths and G-code that it generates can be directly used by Snapmaker CNC Carving Module. In addition, it also supports the preview of tool movements and the finished product. If you simply want to carve out the finished product based on an existing model file, Snapmaker Luban is without doubt one of the best candidates.

MeshCAM is one of the most popular CAM software on the market, with excellent ease of use as its main highlight. Thanks to its straightforward workflow and simple operations, even those new to the world of CNC without machining knowledge can easily master it. Automatic toolpath configuration is one of the things that make MeshCAM great. Simply choose the tools and the desired quality level, and MeshCAM will automatically calculate the appropriate parameters. The built-in post processor of MeshCAM does not support Marlin yet. Some additional steps are required to translate the G-code into a format recognizable for Snapmaker.

Summary

The CNC workflow begins with CAD, where imaginations are transformed into designs. Next, CAM connects design and manufacturing by transforming designs into toolpaths for CNC carving machines. The first three articles of our CNC series focused on CAD and introduced eight CAD modeling software picks along with 12 recommended websites for modeling resources. In the fourth and fifth articles, we moved forward along the CNC workflow, clarified some key concepts in CAM, including post processor, firmware, and CAM workflow, and presented four integrated CAD/CAM software picks with their respective work process. Now, we have learned the complete process from CAD to CAM. We hope that these articles can help you get started with CAD and CAM for CNC!

Snapmaker Academy will continue to offer more CNC carving resources and information. So stay tuned! If you are interested in any topic, please feel free to let us know by leaving a message in our community or sending an email to support@snapmaker.com.

Disclaimer

Snapmaker recommends the software and videos to you in no particular order and for resource-sharing purposes only. Snapmaker does not in any way endorse, control, or assume responsibility for the content, views hosted on, and services provided by the developers of the software or individuals.

Hey there, Maker!

Welcome to Snapmaker Academy! This is the fourth episode of our CNC series. The three previous episodes focused on CAD and introduced some practical modeling software and websites of modeling resources. Now, let's turn to CAM and check out four CAM software picks suitable for CNC carving.

Photo by Fakurian Design on Unsplash

Before jumping right into CAM software, let's go through some basic concepts. First of all, what are CAD and CAM?

CAD vs. CAM

We already know that, in the CNC workflow, three steps are required to turn an idea into a finished product. First, obtain the model file. Second, transform the model file into commands that CNC machines can execute. Third, import the commands into a CNC machine to start carving till we obtain the finished product.

Computer-aided Design (CAD) refers to the first step in this workflow. It covers aspects related to model designing, such as conceptualization, detailing, modification, etc. Computer-aided Manufacturing (CAM), on the other hand, corresponds to the second step, through which models are transformed into commands (toolpaths and the corresponding G-code) that tell the CNC machines what to do. Usually, it also includes operations like simulation and error check to minimize the risk of going wrong.

For example, you want to build a toy car. First, you need to turn the imaginary toy car in your head into a model file, which is essentially a collection of geometrical data. This step is called CAD. Next, you use software to transform the model file into G-code. The toolpaths in the G-code tells the machine what to do in order to carve the geometric forms depicted by the model, such as round corners, bosses, and grooves of the toy car. With simulation and error check, you can preview the path of the tool on the material surface and judge if the carving will go smoothly. This step is called CAM.

Photo by Tool., Inc on Unsplash

In a nutshell, with CAD, we transform ideas into designs, and with CAM, we manufacture real products based on the designs. The two processes complement each other and are equally indispensable.

Post Processor & Firmware

Now, it's time to move on to two new terms: post processor and firmware.

As mentioned before, your design can become G-code thanks to CAM software. But in order to successfully carve out the finished product, a crucial step is to make sure that your machine can effectively recognize the G-code output by the CAM software.

You can think of G-code as a collection of different "dialects". Post processors translate the dialects into the one that your specific CNC carver can understand and execute. The file that post processors use for such translation is called a "post". A post processor can be either stand-alone software or integrated into CAM software.

Firmware is a special kind of software that is embedded in hardware, resembling the operating system of your computer. For 3D printers, firmware is responsible for transforming G-code into control commands that tell your CNC carver what to do. The firmware of your CNC carver determines the type of G-code it can read. This means that you need to know what language your machine speaks (i.e., its firmware type) first and then select a translator (i.e., a post processor) that works for it.

Products made with Snapmaker CNC Carving Module

Marlin is one of the most popular 3D printing firmware. Other widely-used firmware includes GRBL and Klipper. The firmware of Snapmaker 3-in-1 3D Printer is developed based on Marlin. Currently, we provide posts for ArtCAM, Aspire, FreeCAD, and Fusion 360. After downloading the file, simply import it to the software to generate the correct G-code for your Snapmaker CNC Carving Module.

 To learn more about Marlin, see What is Marlin?.

CAM Workflow

Before delving into each CAM software, let's go through the overall workflow of CAM briefly. This can help us better understand the logic of using each software. A typical CAM workflow consists of the following six steps:

1. Import the model to CAM software;
2. Set the coordinate system and define the position and work origin of the stock (i.e., the material to be carved);
3. Specify stock parameters, such as its dimension and orientation;
4. Select the machining method (for example, three-axis machining or four-axis machining) and the tool (for example, flat end mill or ball end mill) being used;
5. Preview the toolpath in simulation to visualize in advance how the tool moves and what the finished product looks like;
6. Perform post processing and export the G-code.

Now that we have understood the role of CAM in the CNC workflow and the CAM workflow, it's finally time to get down to business. Let's look at some excellent CAM software!

CAM Software

CAD and CAM are two independent procedures, and a lot of software focuses on one of the two. However, due to our pursuit of convenience, more and more software now integrates both CAD and CAM features to enable an all-in-one design process.

One big advantage of this type of CAD/CAM software is the elimination of data format conversion, which occurs when you import a model file from CAD software to CAM software. CAD/CAM software works with the same data files from sketch design to the generation of G-code. What's more, it is easier to edit model files because you do not need to switch between different software. This article will introduce four pieces of CAD/CAM software with a focus on CAM: Fusion 360, FreeCAD, Aspire, and Carveco Maker (formerly ArtCAM).

To learn more about their CAD-related features and highlights, see CAD for CNC: Eight 3D Modeling Software Picks to Visualize Your Ideas.

Fusion 360

The CAD part ends as you finish the sketch design in the Design Workspace of Fusion 360. You can then click to switch to Manufacture Workspace for performing CAM operations.

 If you're using Fusion 360 to design models for the first time, you need to download the post and tool library first and then import them to Fusion 360. The video How to Model & Setup CAM for CNC in Fusion 360 shows you how to do it. As mentioned before, the post ensures that Snapmaker CNC Carving Module can understand the G-code that will be generated by Fusion 360. The tool library tells the software which type of tool we intend to use so that the software can calculate the corresponding toolpath.

Preparations are now done. We can proceed to the manufacturing process! The first step is setup. In this step, we define the coordinate system and the work origin for the stock. By specifying how the stock is placed on the work platform of your CNC carver, this step associates the virtual coordinates in the software with the actual ones in manufacturing.

Now, the software knows the data of the model file, the size and orientation of the stock, and the tool type. It's got everything needed to calculate and generate the toolpath that instructs the tool on how to move. In addition, Fusion 360 supports real-time simulation. It shows the path of the tool in animation to let us visualize the final machining effect in advance. We can edit the toolpath while conducting simulations to optimize the carving result.

Simulation in Fusion 360

With the post imported previously, we can now directly convert the toolpath into the G-code specific to our Snapmaker CNC Carving Module. Then, we import the G-code to the machine and start carving. Now we just wait for the finished product.

Fusion 360 has a great number of users. Its CAM tutorial videos are also easy to find. There are official videos like Fusion 360 CAM Basics and videos made by users like How To Get Started with CAM Within Fusion 360 — Tutorial.

Next Up

Limited by length, this article breaks into two parts, and this is the first part. In the next part, we will continue with other CAD/CAM software: FreeCAD, Aspire, and Carveco Maker (formerly ArtCAM). We will also briefly introduce two pieces of CAM software: Snapmaker Luban and MeshCAM. So, make sure to stay tuned!

Disclaimer

Snapmaker recommends the software and videos to you in no particular order and for resource-sharing purposes only. Snapmaker does not in any way endorse, control, or assume responsibility for the content, views hosted on, and services provided by the developers of the software or individuals.

Hey there, Maker!

This article breaks into two parts. In Part 1, we introduced four pieces of artistic relief modeling software suitable for creating relief models that allow for more free-formed shapes and typically serve visual expression.

In addition to decorative relief, CNC carving is also commonly used to manufacture products with a more regular form or involving assembly, such as phone stands and toy cars. Strict with dimensions, these products should better be designed as solid models of higher accuracy to ensure smooth output to CNC machines. This is where we need to use industrial design modeling software.

Photo by Fakurian Design on Unsplash

In this article, we will take a look at the best of the best in industrial design modeling software for CNC solid modeling—Fusion 360, FreeCAD, SolidWorks, and SketchUp.

Industrial Design

Fusion 360

Price: $60/month, $495/year, or $1,335/3 years (By subscription)

Supported System: Windows, macOS

Highlights: One-stop work platform, Intuitive interface, Cloud storage, Massive supporting resources, One-year free trial

When it comes to solid modeling, we have to mention Autodesk Fusion 360, one of the top modeling software picks in recent years, especially all the rage among makers.

Fusion 360 boasts three benefits. First, it is not only a piece of modeling software, but also a versatile work platform providing a complete suite of tools from model design to manufacturing. It is easy for DIY hobbyists to learn.

Second, it connects modeling with manufacturing. Photorealistic rendering, product simulation testing, and a set of built-in CAM tools to directly generate toolpath and G-code enable a seamless transition from design to manufacturing in the CNC workflow.

Third, the software highlights excellent ease of use on top of its powerful features. Its intuitive interface is user-friendly and easy to get started with. Many users find Fusion 360 more productive than other equivalents when completing the same model design.

Fusion 360 has more to offer. It is one of the first CAD work platforms to support cloud storage. Users can synchronize personal files across multiple platforms and easily retrieve the change records, and collaborate with each other in real time.

In addition, thanks to the huge user base, related instructional videos are everywhere on YouTube, and third-party plug-ins and other resources are also abundant. Snapmaker Academy has previously produced a Fusion 360 tutorial on how to create a model, set up toolpaths, and use the Snapmaker 3-in-1 3D Printer to carve out a finished product.

Fusion 360 CAD & CAM Tutorial Video 

Of course, as a typical Autodesk product, Fusion 360 is available in Education and Personal editions, both of which are free for one year.

FreeCAD

Price: Permanently free

Supported System: Windows, macOS, Linux

Highlights: Open source, Cross-platform, Parametric modeling, Integrated CAM tools

FreeCAD is a piece of free and open-source 3D modeling software used to design solid models of any size for personal projects and fields such as industrial product design and architectural engineering.

The software is designed for parametric modeling, which means the shape of an object is defined by parameters, and all shape changes are recorded to maintain a precise modeling history. You can modify any feature of the models by changing the corresponding parameters. Moreover, changes to individual features can be synchronized to the final model by simply setting the constraints, eliminating the need for repeated operations.

FreeCAD is separated into workbenches. A workbench is a collection of tools suited for a specific task. The Part Workbench and the Part Design Workbench are commonly used in CNC carving. You can produce any geometry by building multiple 3D parts and connecting or assembling them.

FreeCAD can read and write files in various formats, including STEP, IGES, OBJ, STL, DWG, DXF, SVG, IFC, and DAE, basically covering all major 3D models and image files. Highly customizable and extensible, it can be augmented with various plug-ins to support more file formats. Tutorials on the software are easily accessible, such as How to model an easy part for CNC machining in FreeCAD.

In addition, it also provides CAM tools to help you link your design up with manufacturing. Once a model has been created, you can switch to the Path Workbench to generate toolpaths and G-code.

SolidWorks

Price: $3,995/license + $1,295/year by subscription (Standard version)

Supported System: Windows

Highlights: Parametric modeling, Powerful functionality, Easy to learn and use, Cloud storage, Integrated CAM tools

SolidWorks, a piece of CAD software developed by Dassault Systemes, is one of the top solid modeling software picks at present. Dassault Systemes provides 3D design and product development solutions in a wide range of fields such as aerospace, machinery and electronics, and energy materials. Boeing 777—the world's first 100% digitally designed jetliner—was modeled using the company's modeling software.

Like FreeCAD, SolidWorks uses parametric modeling to help you visualize your design precisely, and changes to individual features can be updated in real time to the final model. The modeling method is much the same as in FreeCAD, i.e., creating surfaces and then truncating or stretching the surfaces to get the model you want.

SolidWorks also provides rendering, simulation, manufacturability check, and CAM tools to help users reduce potential errors in the design process and achieve "manufacture-oriented design." In terms of data management, the software supports cloud storage and real-time collaboration. It boasts excellent expandability and compatibility, as it can be used with many plug-ins and other modeling software.

Among the four pieces of solid modeling software, SolidWorks provides the most powerful and comprehensive functions, allowing you to design complex parts and assemblies easily, and satisfy advanced modeling needs. Moreover, it is easy to use, intuitive, and quick to get started. As the software has millions of users, it is easy to access supporting resources from their official community, YouTube channel, and Reddit community. Technical support is covered in the annual subscription fee included in the price of the software.

SketchUp

Price: Free version and three paid versions available

Supported System: Windows and macOS for Desktop version and all operating systems for Web version

Highlights: Easy to use, Cloud storage, Web client available, Free model library

SketchUp is a piece of easy-to-use 3D design software, dubbed as the "pencil" to generate digital designs, which is widely used in interior and architectural design. If you are not sure which modeling software is right for you, SketchUp is a good choice to start with.

To build a model, you simply create 2D shapes by drawing lines and then extrude them into 3D objects. This is the most common method for architectural modeling and can also be used for CNC solid modeling of regular parts. You can also use SketchUp to break down the 3D structure to be assembled into vector graphics for CNC cutting. However, it does not provide CAM tools, and you need to install plug-ins or use other CAM software to generate toolpaths and G-code.

SketchUp is available in one free version and three paid versions. The free version is web-based, so it cannot be used offline. SketchUp Shop is the cheapest of the three paid versions and it is also web-based, so it is suitable for DIY modeling. The other two versions—Pro and Studio—can run on both web and desktop.

SketchUp supports a wealth of plug-ins and offers mobile apps for iOS and Android devices, allowing you to view your 3D models on your mobile device at any time. Its 3D Warehouse is a free online open library where anyone can upload or download materials and models. A lot of official tutorial videos are available, such as Top Tips for Fabrication and Prepping Woodworking Projects for LayOut in SketchUp. SketchUp also has an active community forum, which is worth visiting.

Summary

In this article, we introduced four pieces of industrial design software for solid modeling, namely Fusion 360, FreeCAD, SolidWorks, and SketchUp. The former three provide built-in CAM tools. Fusion 360 is known for its one-stop work platform and intuitive interface. FreeCAD is a piece of free open source software that can run on all platforms and support various extensions. SolidWorks is a powerful tool that can meet advanced modeling needs. SketchUp is the easiest to use and offers a free version.

Snapmaker Academy will continue to offer more CNC carving resources and information. So stay tuned! If you are interested in any topic, please feel free to let us know by leaving a message in our community or sending an email to support@snapmaker.com.

Disclaimer

Snapmaker recommends the software and videos to you in no particular order and for resource-sharing purposes only.

Snapmaker does not in any way endorse, control, or assume responsibility for the content, views hosted on, and services provided by the developers of the software or individuals.

Hey there, Maker!

In the previous article, Going from Art to Part: Models, Designs and Videos for CNC Carving, we explained that model files are the first step in the workflow of CNC carving and introduced several websites that offer ready models. But, what if you're looking to turn your unique ideas into reality?

A relief carving of your cat, a wooden tray sized to fit snugly into your corner cabinet, a spectacle frame tailored to your face shape ... If you've ever thought of making something like that, now's the time to take a step further.

New to 3D modeling or not sure how to choose modeling software? Snapmaker Academy is here to help! In this article, we will walk you through eight practical CNC modeling software picks for creating your own 3D models from scratch.

Photo by Fakurian Design on Unsplash

It's worth noting that we're touching on modeling software for CNC carving purposes only and do not intend to involve detailed software tutorials.

How to choose CNC modeling software?

The thing is that the dozens of modeling software on the market often come with distinctive operating logic and functional features. Considering the cost of learning, it's definitely wise to do your homework in choosing the right one. Here are some key factors worth considering:

• Purpose of Use

  
  The software you should use when designing something to be CNC machined depends greatly on what you are trying to make. For beginners, powerful or comprehensive functions may not be necessary. On the contrary, advanced functions can be intimidating until you become proficient.

• Function & Feature
  The usage of 3D models determines how they should be designed. That's why modeling software varies in function, feature, and expandability for specific fields.

• Price
  The vast majority of modeling software is charged with prices ranging from a few hundred dollars to several thousand dollars. Before placing your order, make sure you understand what is included in the service.

• Ease of Use
  The ease of use relates directly to the cost of learning the software. A helpful reference is how intuitive the interface is. Shortcuts can also be a time-saver when making repetitive operations. 

• Support Resources
  Support resources include official technical support, user communities, and relevant UGC. These resources are the channels you can resort to when encountering a problem. The larger the user base, the stronger the user community, which is especially important for beginners. Having the guidance of someone who has been there before can be sheer bliss when you're scratching your head over a particular feature.

• Trial Availability
  At the end of the day, one trial outclasses ten introductory articles in interpreting how the software works. Given the high pricing of most modeling software, an available trial version is probably the greatest virtue.

CNC Modeling Software

Solid Modeling VS Surface Modeling

First, notice that there is a fundamental difference between 3D models used for different purposes. For industries like machinery and mold manufacturing, 3D models require high dimensional accuracy and must form a closed space, so we call them solid models. For industries such as film and games, however, surface models are commonly used, which focus more on an object's external. They allow for more free-formed shapes and do not necessarily make up a closed space. Such models typically serve visual expression only, including animation character design, product display videos, etc.

Closed Space VS Open Space

An imperfect analogy would be a comparison between engineering drawings and art paintings: while one corresponds to real objects and must be precise to the length of each line and the size of each angle, the other is visually oriented and thus can go wild to display structures that cannot exist in reality.

Actual Structure VS Surreal Structure

（Photo by Autodesk Fusion 360 on YouTube & 8385 on pixabay）

Accordingly, 3D modeling software can be divided into three categories based on modeling mechanism: solid modeling, surface modeling, and solid + surface modeling. In CNC carving, surface modeling is appropriate for creating ornamental reliefs or parts with lots of irregularly curved surfaces. Instead, products involving complex assembly or parts consisting of regular shapes like rectangles, round holes and straight lines are suggested to be designed as solid models.

Next, let's get to the point — modeling software for CNC carving. Note that the following software may support both kinds of modeling but is here divided into two categories — artistic relief and industrial design — based on the modeling mechanism it is known for.

Artistic Relief

Aspire

Price: $1,995  (Perpetual for a specific version, including free minor updates)

Supported System: Windows

Highlights: Relief design, 2D to 3D, 4-axis CNC carving, Integrated  CAM

Aspire is a one-stop CNC software solution developed by Vectric. Featuring relief design, it allows simple and quick conversion from 2D images to 3D relief models. Here's how it works: after importing a 2D image, the software assigns a height difference to the image based on the shade of color to create a 3D relief model. The darker the color, the smaller the corresponding Z-axis height value, and the deeper the carving. For this type of conversion, a grayscale image works best. You can also start with a sketch and expand it into a 3D model step by step by operating manually.

Aspire offers a set of handy tools and a rich library of resources for relief models. You can use filters to remove the noise in the image to create a smoother surface, or manually increase the Z-axis carving depth to further spotlight its three-dimensionality. What's more, the software comes with hundreds of free 2D graphics and 3D relief models to add to your creations.

Support for 4-axis CNC carving is another bonus. You can either design your own 4-axis models or import third-party models. Aspire's rotary job setup and auto-wrapped simulation allow you to visualize your job. Combined with Snapmaker Rotary Module, you're ready to create in a new dimension.

Cases made with Snapmaker Rotary Module

After modeling, the next step is to turn your model into commands that will instruct your CNC machine on how to move, which is also within the cover of Aspire. Aspire is capable of calculating 3D roughing and finishing toolpaths to accurately carve out your model, saving the trouble of using another CAM (computer-aided machining) software.

It's recommended to try out the built-in cases in the trial edition before purchasing. You can find tutorial videos for the cases on their official website. There are also many useful videos made by Aspire users, such as the one by Roger Webb, demonstrating the whole process of making a relief plaque from importing a grayscale image to setting toolpaths.

Carveco Maker

Price: $15/month or $180/year (By subscription)

Supported System: Windows

Highlights: Diverse relief editing tools, Broad range of supported file types, Integrated CAM

You may not have heard of Carveco, but you're probably familiar with ArtCAM, one of the oldest software devoted to CNC. In fact, ArtCAM is the predecessor of Carveco. The software was acquired by Autodesk and then discontinued in 2018; that's when Carveco Ltd. was formed with the purpose of delivering continuity of access and service of ArtCAM. Carveco Maker is the elementary variant of the Carveco software range.

Just like ArtCAM, Carveco Maker is powerful and easy to use, making it popular among woodworkers, sculptors and makers. Besides the regular 2D sketch design and 3D modeling tools, it also includes multiple features customized for relief models, such as conversion from grayscale or vector image to relief, embossing STL model to relief, one-click smoothing of relief, and more. You get to control the final presentation and fineness of the finished product at your own pace. Its relief clipart library contains more than 600 exquisite relief models, all free to use in your CNC projects.

Carveco Maker's Relief Clipart Library

Carveco Maker works easily with different types of graphics, 3D models, and CAD (computer-aided design) files. Integrated CAM is also one of its strong suits, enabling choices over machining strategies, tool configuration, toolpath generation, and real-time simulation of the final look of your design.

The Carveco team has produced a series of well-made instructional videos covering key tools and features such as Reliefs from Images. In addition, ArtCAM's existing large user base and tutorial videos are also available resources for Carveco Maker since the two pieces of software are basically the same. Carveco does not offer a trial version but a 14-day money back guarantee on the software is available.

ZBrush

Price: $39.95/month, $179.9/6 months, or $895/perpetual

Supported System: Windows, macOS

Highlights: Digital sculpting, Modeling with brushes, Intuitive operation

ZBrush is a leading software package in digital sculpting software, endeared to film studios, game developers, and illustrators globally. One of the major games made with ZBrush is Assassin's Creed. As the name suggests, digital sculpting is like sculpting some digitized clay through manipulating geometric shapes by pushing, pinching, chiseling and slicing with brushes. Compared to traditional 3D modeling, its operating logic is far more intuitive, reproducing the natural feeling of working with a real-life object.

It is ideal for creating detailed surface models with sophisticated and irregular shapes, powerful in presenting realistic shadows, textures, and creases.

When used for CNC modeling, ZBrush is competent in both creating 3D models from scratch and collaborating with other modeling software to add more details to your relief models, such as softening joints, adjusting partial height difference, adding textures, etc. The software is also great in real-time rendering that provides instant feedback. However, to generate toolpaths and G-codes, you need to use plug-ins or import your model into CAM software.

Plentiful sculpting brushes in ZBrush

Thanks to its intuitive logic, ZBrush is easy to get started, and tutorial videos abound. Its trial version has no restriction on features, which lasts 30 days.

Blender

Price: Free

Supported System: Windows, macOS, Linux

Highlights: Open source, Cross-platform, Free interface layout, Integrated digital sculpting

Blender is open source software for all platforms, providing 3D creation pipelines from modeling, rigging, animation, simulation, rendering, to video editing. As the only mainstream modeling software that is free for life, it is a public project hosted by the Blender Foundation, with the mission to bring 3D technology as tools in the hands of artists everywhere in the world.

Beyond polygon modeling, Blender also integrates digital sculpting, empowering fast and free detailing using brushes. Though not comparable to ZBrush in this regard, it is qualified. As with ZBrush, the generation of toolpaths and G-code requires additional CAM plug-ins or software since it does not specialize in CNC.

Sculpting brushes in Blender

A typical workflow in CNC relief modeling is to import a 2D image, trace the profile with polygons, expand it into a 3D model by operations like stretching, and then smooth the edges and corners with subdivision tools, including sculpting brushes. You can find many related videos on YouTube, such as Decoration Modeling in Blender 2.9 Part 1.

Being free and open source does not equate to a lack of support resources, at least not with Blender. Donations from users, developers, and companies keep the foundation and their official technical team running. Also, Blender's growing community is very helpful and ready to come to your aid when in trouble.

Summary & Next Up

This article introduces four pieces of artistic relief modeling software: Aspire and Carveco Maker, which specialize in CNC and excel at relief modeling with CAM tools included; and ZBrush and Blender, which allow users to create or optimize relief models through digital sculpting.

Limited by length, this article breaks into two parts and this is the 1^st part. In the next part, we will introduce Fusion 360, FreeCAD, SolidWorks, and SketchUp for solid modeling.

Disclaimer

Snapmaker recommends the software and videos to you in no particular order and for resource-sharing purposes only.

Snapmaker does not in any way endorse, control, or assume responsibility for the content, views hosted on, and services provided by the developers of the software or individuals.

Hey there, Maker!

You probably already know that makers' world is full of possibilities. On top of that, as the owner of the Snapmaker 3-in-1 3D Printer, with its three interchangeable functions – 3D printing, laser engraving and cutting, and CNC carving – you're empowered with more than one key to unlock the door from imagination to reality.

So, what do you want to create with your Snapmaker CNC Module?

Here are 11 resources websites that will inspire you and provide access to model files, complemented by a series of tutorial videos. Hopefully, this article will help you in taking the first stride.

To begin with, let's go through some basic concepts of CNC machining.

What is CNC machining?

CNC stands for "Computer Numerical Control". CNC machining is a common subtractive manufacturing technology. The process involves removing material from a solid workpiece with cutting tools to achieve the desired shape. Compared to 3D printing, aka additive manufacturing, CNC machining is fundamentally different since it chips material off a blank workpiece instead of adding material to build a part.

Cases made with Snapmaker CNC Module & Rotary Module

What can you do with a CNC machine?

CNC machining can work with a wide range of materials, including plastic, wood, jade, and metal. Technically, you can even build a house through CNC machining with quite some assembling, not to mention toy cars, ukulele, PCB…

Next, let's look at the workflow of CNC carving. Typically, it takes three steps to turn an idea into a finished product:

1. Obtain a model, either by modeling yourself or downloading from model repositories.
2. Turn the model file into a G-code using CAM software (such as Snapmaker Luban and Fusion 360). The G-code will instruct the machine on how to move.
3. Export the G-code to your CNC machine. Start carving on your machine and then wait for your job to be done.

Now that you've recognized what a CNC machine can do and how it works, let's get down to the gist. In the following CNC resources websites, you can indulge in inspiring ideas from all over the world or directly download model files and carve them out.

CNC Resources Websites

 On the 3D model files provided in the following websites, except for those specified with compatibility of CNC machines, take care in identifying whether a particular model is suitable for CNC carving.

Thingiverse

Being one of the world's largest and most active 3D model file repositories, Thingiverse boasts three million users and over two million models. From regular household items, ACG character figures to mind-blowing gadgets, there's something for everyone. While models for 3D printing predominate, it's not hard to find models for CNC carving.

In this community, you can also follow people from all walks of life. If you're interested in CNC woodcarving, ZenziWerken is definitely one of the must-see accounts. It was created by Daniel, a German who loves woodworking. He has been sharing hundreds of woodworking cases designed and made all by himself over the years for free. Each case is exquisite and practical, with detailed instructions.

Since you can 3D print a 3D printer, be noted that if you simply type "CNC models" in the search bar, the results will mostly be parts for CNC machines. This might often be the case with the following websites as well. Therefore, it is best to search with specific keywords, such as "CNC toy cars". Thingiverse's search filters support only a few categories, which makes the right keywords even more critical.

GrabCAD

GrabCAD has more than 9 million users and nearly 5 million model files, all available for free download. The site focuses mainly on models for specialized fields such as automobile, mechanics, architecture, and industrial designs, distinguishing GrabCad from other 3D model repositories. However, you can also find numerous models suitable for CNC carving. For example, the keyword "chess" will return some nice matches.

In addition to filtering by model category, GrabCad's search filters also support specifying file format and the software used to generate the model. To locate the model you need quickly, use precise keywords combined with appropriate filter criteria.

MyMiniFactory

MyMiniFactory is one of the most popular 3D model marketplaces with more than 160,000 models. Although not known for its volume, many of the models come from professional designers, and the average quality is excellent. All of the models have been tested by the community to ensure that they can be used for 3D printing, and some of them are also compatible with CNC milling.

MyMiniFactory focuses on paid models from art and pop culture fields such as games, anime and movies. If you're a pro in designing or modeling, this is a great place to cash in on your talent.

MyMiniFactory also provides a small selection of free models. The site highlights easy-to-use search filters, which allow you to refine the results by category, pricing and complexity of the models, as well as the model of the 3D printer used. A direct search for "CNC" returns less than ideal results, and it is best to enter more specific keywords, such as "relief".

Cults

Cults is another designer-rich 3D model repository featuring delicate models. The site has over 3 million users and close to 420,000 models. Both paid and free models are available. If you're good at creating 3D models, you can upload your work to Cults and price it in just a few steps.

Surprisingly, searching directly for "CNC" on Cults leads to quite a few models designed for CNC carving. A more precise keyword will undoubtedly return more satisfactory results, though. On an account called "STLFILESFREE", you can find dozens of beautiful models for wood relief carving, all for free.

TurboSquid

TurboSquid models are used by game developers, architects, visual effects studios, advertisers, and creative professionals around the world. You've probably seen TurboSquid models hundreds of times and didn't know it. A majority of the one million models uploaded here are priced.

Most of the models on the site are not for 3D printing or CNC processing, but you can filter by STL format and enter specific keywords, such as "relief". You can also filter out free models, although the results may be numbered.

Instructables

Unlike the model repositories introduced above, Instructables is a community where DIYers share their creations. Each case contains detailed step-by-step instructions, accompanied by pictures, animations and videos; each step allows other users to add hints or ask questions, allowing sufficient interactions.

From electronics, mechanics, woodworking to cooking, Instructables offers cases of just about anything. On the Workshop subpage, there are separate sections for 3D printing, laser cutting and CNC. The CNC section is definitely a mine of information for experienced CNC players. In addition, the site has a Teachers section, thoughtfully divided by grade level, to encourage teachers to apply DIY cases in their classes. Search directly for "CNC" plus keywords, such as "CNC toys", and you'll likely find some fascinating results. Not every case comes with ready model files, but all cases are available as a packaged PDF file for download.

Maker Union

Maker Union supplies free DXF files of high quality with a simple and easy-to-use interface. DXF is a vector image format that is well adapted to CNC machining, which acts as 2D patterns that guide your machine on where to cut. Processing DXF file with CNC machines will not leave black edges as opposed to laser engravers. The finished products are perfect for decoration.

The site features theme-based display of files, where a set of beautiful DXF files can be downloaded as a package in a click. Although the number of themes is just over 240, there are on average 6–8 files under each theme, all of which are ready-to-cut for CNC machines. Maker Union supports keyword search of themes, and you can choose to display the search results by popularity, release date, etc.

MakeCNC

MakeCNC offers only paid models of high quality, covering categories such as architecture, vehicles, ships, mazes, animals with a total of more than 1,400 models. Each model consists of a set of vector graphics that can be used directly for CNC machining. Assembly is usually required, and a detailed assembly manual is hence included in the files downloaded. While cutting a single vector graphic poses little challenge, milling complex curved surfaces and carving assembly parts do require more experience in CNC machining.

STLFinder

As you can tell by its name, STLFinder is a search engine for 3D models in STL format. Thingiverse, GrabCAD and MyMiniFactory are some of the major 3D model libraries included in its index. The total number of models indexed is huge, with 159,316 results returned for the keyword "wall art" alone. It only supports filtering by paid or free models.

Etsy

Etsy is a marketplace focusing on handmade items and craft supplies. Apart from physical goods, there are also paid models under a broad range of categories, including home decor, toys, art, as well as tools; both 3D models and 2D patterns are available. Here you get to see buyers' reviews and photos of finished products on the page of each model file. You can also open your own store on Etsy and price your creations.

Go straight for "CNC file" in the search bar, and you'll find hundreds of 3D models for CNC machining, ranging from woodcut Star Wars calendar to world map relief. The site supports filtering by keyword match, price range, release date, etc. In addition, the search bar provides access to recently viewed items.

Craftsmanspace

Craftsmanspace comprises a wealth of free 3D models and 2D patterns. In addition to the two sections dedicated to model files, the Free projects section collects cases uploaded by users along with instructional PDF files. The site also has a Knowledge section full of information, including a comprehensive introduction to woodworking joints completed by illustrations and terminologies.

Pinterest

Pinterest is one of the largest image-sharing platforms in the world. Thanks to its volume, searching with CNC-related keywords, such as "CNC cutting design", returns a considerable number of results, including many masterpieces. Browsing through the designs can be a great source of inspiration. Note that only images of finished products are available here rather than source files for CNC machining.

CNC Tutorial Videos

Whether it's to stimulate your own thinking with others' designs or provide model files that your CNC machine can work with, we hope the above websites have helped you in leaping from ideas to models.  

Now, let's proceed to turn models into solid parts. Here are several tutorial videos on using Snapmaker CNC Modules and software, namely the Snapmaker Luban and Fusion 360.

Tutorial Videos by Snapmaker

Snapmaker 2.0: How to Use the CNC Function

The Snapmaker 2.0 comes with an ER11 collet, an MDF wasteboard, and dust-resistant Linear Modules. The CNC Module is easy to use and supports various types of materials. Check out this step-by-step tutorial on Snapmaker 2.0 CNC function and give it a shot.

How to Use CNC Function with Rotary Module

Follow along this video to see an entire 4th-axis CNC machining process with the Rotary Module. We've added new features of Origin Assistant and Bit Assistant to the Touchscreen and realized full support in Snapmaker Luban. 

Intro to Snapmaker Luban 4.0 for 3-axis CNC Carving & Intro to Snapmaker Luban 4.0 for 4-axis CNC Carving

Learn how to use the 3-axis and 4-axis CNC with Snapmaker Luban 4.0 with a brand new interface, improved workflow, and some useful newly added features.

Fusion 360 CAD & CAM Tutorial for CNC Beginners [Snapmaker Academy]

Follow this video to design a 3D model in Fusion 360 and carve it out with your Snapmaker. The whole process could be much easier than you would have expected.

Tutorial Videos by Users

Snapmaker Tool Changes: Fusion 360 3D Relief Milling

Rodney Shank made this video for anyone who wants to know how to mill a relief on wood using Fusion 360 and the Snapmaker 2.0. In this video, you will be guided through the whole process step by step, including changing tools from rough to finish carving.

4 Axis CNC Machining with Snapmaker 2.0
In this video, Nikodem Bartnik tests and reviews the Rotary Module of Snapmaker 2.0. He succeeded in milling some cool stuff like SpaceX model out of epoxy tooling material and wood while failed with aluminum.

Snapmaker 2.0 - E04 - Using the CNC

In this project of Koka-Bora Creations, the author demonstrates the process of carving an SVG image onto a piece of wood relief using Snapmaker 2.0. In addition to the practical steps, he also explains how CNC relief works, the pros of working with SVG greyscale images, and some other principles.

Armed with the above resources, you're well-prepared to try it out now. Just get your Snapmaker CNC Module going and bring your creative sparks to life!

In the future, Snapmaker Academy will continue to provide you with helpful CNC resources and knowledge, so STAY TUNED!

If you are interested in other topics of 3D printing, feel free to contact us at support@snapmaker.com, or leave your message in our community.

Disclaimer

Snapmaker recommends the websites and videos to you in no particular order and for resource-sharing purposes only.

Snapmaker does not in any way endorse, control, or assume responsibility for the content, views hosted on, and services provided by these websites or individuals.

Design & Manufacture

This is a newbie's guide on 3D modeling and CAM setup for Fusion 360. In this video, you will learn how to create a sketch, create a solid body, import tool library, set 2D pocket, set 2D contour, and post-process you design in Fusion 360, and finally carve it out with Snapmaker 2.0.

The tools and material needed:

[Tool] Snapmaker 2.0: https://shop.snapmaker.com/collection...

[Software] Autodesk Fusion 360: https://www.autodesk.com/products/fus...

[Material] Beech Wood Board (150mm×150mm×10 mm)