1 Read This First - Safety Information
1.1 General Safety Information
- Always operate this machine indoors on a solid horizontal table or workbench.
- Do not expose this machine to rain or wet conditions.
- Keep children and bystanders away while operating this machine. It requires the supervision and assistance of an adult when children use this machine.
- Stay alert, watch what you are doing and use common sense when operating this machine. Do not use this machine while you are tired or under the influence of drugs, alcohol or medication.
- Do not reach inside the machine or touch the moving parts while the machine is still in operation. An injury may be caused by its moving parts.
- Do not leave the machine unattended while it is still on.
1.2 CNC Safety
- Age Recommendation: For experienced users and users age 18 and above.
- Put the machine into an enclosure and wear the CNC Safety Goggles.
- Always have the material securely clamped. Never attempt to hold the workpiece with your hands throughout the CNC carving process.
- Always unplug the machine before performing maintenance or modifications.
- If the bit or workpiece become jammed or bogged down, turn off the machine immediately. Wait for all moving parts to stop and unplug the tool, then work to free the jammed material.
- Do not touch the bit or collet after use. After usage, the bit and collet are too hot to be touched with bare hands.
- Some dust created by CNC carving and cutting contains chemicals known to cause cancer or other reproductive harm. To reduce your exposure to these chemicals: work in a well-ventilated area and work with safety equipment, such as those dust masks that are specially designed to filter out microscopic particles.
2 Set Up for First Use
Read the product Quick Start Guide and Guide for CNC Carving (https://snapmaker.com/product/snapmaker-original/downloads) to check the included parts, assemble the machine, and set up the machine for the first use. You can also watch the video tutorials on our website (https://support.snapmaker.com/hc/en-us/categories/360000327114-Snapmaker-Original) to learn how to use the machine.
3 CNC Carving Workflow
4 Prepare Files
Design: You can design a 3D model using modeling software such as Fusion 360 and AutoCAD. You can also design a 2D image for cutting only.
Take a Photo: You get a 2D image of scenes or objects in real life by taking a photo with your smartphone. It can be used for relief.
Download: You can find free CAD files from the website like grabcad.com/library.
5 Generate G-code
G-code is a programming language that the machine understands and is a series of commands that tells the machine what actions to perform - where to move, what speed to use, what temperatures to set, and much more. Before you start CNC carving, you need to download the software Snapmaker Luban from our website (https://snapmaker.com/product/snapmaker-original/downloads) and install it. And you need to generate the G-code file from a model or image.
5.1 Generating G-code Workflow
The workflow of G-code generating is:
Select the CNC G-code Generator -> Upload model file (Or enter text by clicking T) -> Configure
the parameters in Editor -> Select the CNC bit in Process -> Configure the parameters in Process -> Generate G-code.
Note 1: Make sure you have selected the correct machine model Original in the top left corner.
Note 2: You can generate several model files into a single G-code to do carving all at once.
Note 3: Left click the image to modify the parameters, and right click it to pop up the operation menu.
Note 4: Three modes are available in the software, including:
Relief: You need to upload greyscale images, and the layering effect is based on the different shades of color on your original images. You can use Carving V-Bit in Relief mode.
Vector: This effect is used for carving vector graphics, which is applicable to pocket milling and 2D profile cutting. You can use Flat End Mill in Vector mode.
Text: You can select the font and enter the text as you need. You can also upload your own fonts. You can use Caving V-Bit, Flat End Mill, and Ball End Mill in Text mode.
Note 5: Auto Preview is enabled by default, which shows the dynamic preview after you modify the parameters. When Auto Preview is disabled, you need to click Preview to check the current status.
Note 6: You can also generate G-code by Fusion 360 if you have more requirements for the CNC functionality or want to carve your own design.
5.2 How to Generate G-code in Vector Mode
This section explains the steps of generating G-code in Vector mode and the meaning of each parameter. And this is an example of acrylic cutting with an SVG image.
1. Select the CNC G-code Generator .
2. Click Open File to upload an SVG image.
3. You can adjust the image size, rotate or move the image as needed. After configuring the parameters in Editor, click Process.
4. As this is an example of acrylic cutting with an SVG image, the proper CNC bit is 1.5mm Flat End Mill.
5. Select the Carve Path. 3 types of carve path are available: On the Path, Outline and Fill. We choose On the Path in this case.
On the Path: The CNC bit carves along the shape of the image. The carve path is marked in blue lines.
Outline: The CNC bit carves along the contour of the image. The carve path is marked in blue lines.
Fill: The CNC bit carves away the inner of the image. The carve path is marked in blue.
6. Set the Target Depth. To carve through the material, the target depth should be slightly larger than the thickness of the material. As the acrylic board used in this case is 3mm thick, the target depth can be set at 3.2mm, for example.
7. Set the Step Down. Each type of material has an appropriate depth of every carving step, exceeding the depth range may lead to breaking of the CNC bit or other risks. For acrylic cutting, the recommended step down is 0.4mm (Since the target depth is 3.2mm, it takes 8 steps to carve through the material).
8. Set the Jog Height. Before the machine switches among the carving routes, the CNC bit will be lifted to a certain height, which is called jog height. In this case, we set it at 2mm.
9. Set the Stop Height. It means the distance between the CNC bit and the material when the machine completes carving. In this case, we set it at 10mm.
10. Set the Tabs if necessary. Tabs refer to the connecting structure among the material and the carved objects, which help with fixing the independent parts of the carving and improving the success rate. You need to set the Tab Height, Tab Space and Tab Width.
Tab Height: Now that the material is 3mm thick, when the tab height is set at -0.5mm, the height of the connecting structure is 2.5mm.
Tab Space: The distance between any 2 tabs. In this case, the tab space is 24mm.
Tab Width: The width in this case is set at 2mm, as shown in the figure below.
11. Set the Print Order. When caving multiple images with a single G-code file, this parameter determines the order of carving. When the orders are the same, the image uploaded first will be carved first.
12. Set the Jog Speed. It determines how fast the CNC bit moves at the jog height when switching to another carving route. The jog speed for this case is 3000mm/min.
13. Set the Work Speed, i.e. the carving speed. For this case, the speed is 400mm/min.
14. Set the Plunge Speed. It refers to the lifting / sinking speed of the CNC bit, which is set at 400mm/min in this case.
15. After configuring the parameters in Process, click Generate G-code.
5.3 How to Generate G-code in Relief Mode
This section explains the steps of generating G-code in Relief mode and the meaning of each parameter. And this is an example of wood carving in which a relief will be made.
1. Select the CNC G-code Generator .
2. Click Open File to upload a greyscale image.
3. You can adjust the image size, rotate, move or flip the image as needed. After configuring the parameters in Editor, click Process.
Invert: You can invert the shades of color on the image, which means the primary light-colored parts will be dark-colored. The darker the color is, the more it will be carved.
4. As this is an example of wood carving in which a relief will be made, the proper CNC bit is Carving V-Bit.
5. Set the Target Depth. The target depth we set in this case is 3mm (P.S. The board is 20mm thick).
6. Set the Step Down. Each type of material has an appropriate depth of every carving step, exceeding the depth range may lead to breaking of the CNC bit or other risks. The step down here is 0.1mm.
7. Set the Jog Height. Before the machine switches among the carving routes, the CNC bit will be lifted to a certain height, which is called jog height. In this case, we set it at 3mm.
8. Set the Stop Height. It means the distance between the CNC bit and the material when the machine completes carving. In this case, we set it at 10mm.
9. Set the Density. Higher density means more carving times. We set it at 6 dot/mm here. Following is a comparison between the actual effects of 2 dot/mm and 8 dot/mm densities.
Note: The density can be set up to 10 dot/mm. To achieve the optimal carving effect, the software may recalculate the density when generating G-code.
Density: 2 dot/mm
Density: 8 dot/mm
10. Set the Print Order. When caving multiple images with a single G-code file, this parameter determines the order of carving. When the orders are the same, the image uploaded first will be carved first.
11. Set the Jog Speed. It determines how fast the CNC bit moves at the jog height when switching to another carving route. The jog speed for this case is 3000mm/min.
12. Set the Work Speed, i.e. the carving speed. For this case, the speed is 600mm/min.
13. Set the Plunge Speed. It refers to the lifting / sinking speed of the CNC bit, which is set at 400mm/min in this case.
14. After configuring the parameters in Process, click Generate G-code.
6 Fix Material
1. Place the material you want to carve on the platform.
Caution: If you need to cut through the material, a spoilboard must be put under the material to avoid damaging the CNC bit and the carving platform.
2. Use the fixtures to immobilize the material. Make sure the fixtures will not collide with any parts of the machine.
7 Attach CNC Bit
1. Insert the CNC bit onto the shank, then use the provided 1.5mm hex key wrench to completely tighten the screw.
Note: If necessary, use the wrench to loosen the screw on the shank of the CNC module before inserting the CNC bit.
2. Remove the CNC bit guard.
8 Check the Spindle of CNC Module
1. Turn on the machine.
Caution: Before you turn on the CNC module, make sure you and any viewers have put on your CNC safety goggles.
Note: It is recommended to use the CNC carver with an enclosure covered.
2. Select Controls on the touchscreen. Turn on the CNC module to make sure the spindle works properly, then turn off the CNC module.
9 Connect to Computer
1. Connect your computer to the machine using the provided USB cable.
2. Enter Workspace in the software. Refresh the Serial Port list by clicking in the Connection section. Click the drop-down button and select the serial port of the machine, then click Connect.
Note: If you can't find the port, unplug the USB cable and try again. You may need to install the driver at:
10 Set Work Origin and Run Boundary
1. Enter CNC G-code Generator , then click Load G-code to Workspace.
2. Find out where the carving will be by setting the work origin. The work origin corresponds to the (0, 0) coordinate origin in the software. For example, if the center of the image corresponds to the coordinate origin in the software, you can click X-/X+/Y-/Y+ to move the CNC bit above the center of the material.
Note: We use another machine Snapmaker 2.0 A150 as an example in above figure.
3. By clicking Z-, adjust the distance between the CNC bit and the material to about 5mm. Then place the calibration card or a piece of A4 paper between the CNC bit and the material.
4. By clicking Z-/Z+, keep adjusting the height of the CNC bit until there is slight resistance when you pull out the calibration card, and it should be wrinkled when you push it forward. Click Set Work Origin.
Note 1: The work origin can only be set on the surface of the material.
Note 2: We use another machine Snapmaker 2.0 A150 as an example in above figure.
5. Lift the CNC bit above the fixtures by clicking Z+, then click Run Boundary to check if the work origin is proper. If not, reset the work origin and run boundary again.
6. By clicking Z-, you can lower the CNC bit to run boundary again at different heights.
Caution: If the CNC bit runs into any parts of the machine, power off the machine immediately. Change the CNC bit if it is damaged.
11 Transfer G-code to Machine and Start Carving
You can use the USB cable or the USB flash drive to transfer the G-code to machine and start carving.
Option 1: Online Carving
If you prefer online carving, you just need to click the Run button in the software. In this way, the computer must be connected to the machine throughout the process.
Note 1: You can adjust Work Speed during the carving progress.
Note 2: If you need to stop carving during the working process, click and .
Option 2: Offline Carving
1. If you prefer offline carving, please disconnect to the Serial Port and unplug the USB cable.
2. Enter CNC G-code Generator , then click Export G-code to file. The extension of the exported G-code file is ".cnc". Save it to the USB flash drive.
3. Insert the USB flash drive into the controller of the machine.
4. Tap Files on the touchscreen. Select the G-code file and tap Start to start carving.
12 Remove Finished Work
1. When the carving process completes, tap Controls -> Jog Mode on the touchscreen.
2. Move the CNC module and the carving platform to a proper position. Remove the fixtures and clean the dust, then you can remove the finished work.
Note: We use another machine Snapmaker 2.0 A150 as an example in above figure.