This page describes the Langmuir Crossfire CNC Plasma Table. This is a 3 foot square table equipped with the 45 Amp Razorweld plasma cutter. It can be used to cut various sheet metals up to 1/2" thick.
- Never cut or weld material with zinc in it. Especially galvanized material. It gives off toxic fumes.
- Always have a little extra material or get your material a little larger for testing before you start your final cuts. Create a simple object such as a small circle to test cut on your material to see how it comes out.
- If you want to see the path the plasma cutter will take and check the positioning of your material without cutting it, leave the plasma cutter off. Only urning on the computer and the controller will allow you to import your code and move the plasma cutter without it actually cutting the material.
- The plasma cutter requires the same eye protection as if you were welding. There are welding glasses available.
The general workflow for using the CNC plasma is as follows.
- CAD Design
- CAM toolpath creation
- Machine Setup and Control
There are many different software options that can be used to make it through this workflow. Langmuir provides extensive video tutorials that cover the full workflow using Fusion 360. This entire method can be followed on the Caroline computer, which has a Fusion 360 license. The most common workflow used at Vector Space is Inkscape -> SheetCAM -> Mach3.
There are a lot of options for creating 2D CAD drawings. Inkscape is the easiest, there's also FreeCAD and libreCAD.
The purpose of the CAM process is to provide the tool with instructions on how to create the CAD drawing. In the case of the plasma cutter, this typically means how to follow the lines, and at what speed. The three programs we've successfully used to do this are SheetCAM, FreeCAD, and pyCAM. Each is discussed below, but SheetCAM is recommended for beginners and can be found on the Caroline computer.
The step-by-step instructions below assume that you have already created your object and are ready to improt it into SheetCAM to prepare the code for cutting with the plasma cutter.
Import your drawing
To begin a new project, Click the File menu – New Part. If you want to import a previously designed object from another program (dxf, svg, etc.), in the pop-up menu that opens, choose Yes when it asks if you want to Import a drawing, and then select your file from the explorer menu.
- Under the drawing options, pay special attention to Scaling and Position
- Scaling: Default is set yo 0.5 which is roughly half the size of the imported drawing. If you want it full size, change this to a “1”.
- Position: Default is set to the bottom left corner. This setting or any of the other corners would work best depending on if you have a blank piece of material. If you set the position to center, the plasma cutter will always start from the bottom left corner of your material and move to the object. If you are working around previous cuts, this makes the job much more difficult to position on the plasma cutter.
- If you did not import a drawing file, you can create your object using the SheetCAM controls.
Creating and assigning layers
Once you have completed your design or finished adjusting settings for the imported object, you can create different layers for objects if you want them cut in a certain order. For example, you may want the plasma cutter to cut the holes out first, then cut the rest of the design afterwards. To do this the program has the ability to assign objects to different layers.
When choosing to create your layers, be sure to choose them in the order that you want them to be cut. For example, choose the “Holes” layer first, and the rest of the design second. Think about how each layer will affect the rest of the project. Cutting the design first will probably drop it out of the material, so then it would be difficult to cut the holes after this happens.
- The program will assign all objects to one layer initially.
- To assign objects to a new layer, click the Mode menu and select Edit Contours.
- Left click and hold, then drag the mouse over one or more objects and then release the button.
- Right click on any of the selected objects. In the pop-up menu click Move to Layer, New layer (you will name it) or choose an existing layer to assign the object to a previously created layer.
- To edit the options for each layer:
- Click the Operation menu, Plasma Cut
- Pay attention to the following options in the pop-up menu:
- Contour method: Do you want the cutting to happen on the inside, outside, or middle of the path lines. For example, you may want the holes to be cut on the inside, but the rest of the design on the outside.
- Layer: Make sure you have selected the correct layer for the parameters you are setting.
- Feed rate: The default for this is set to inches per minute (ipm), so if you wanted 20 mm/s, 40 ipm would be close to the same speed (47 ipm would be the exact same).
- Click “OK”. The path setting will now show up under “Operations” on the left sidebar off the program. You can double click to edit them later if necessary.
- When you have finished editing your object and adjusting settings for the layers, you can process the object to be run on the plasma cutter.
Processing your object
Once you have imported your object and adjusted the layers, it is time to process the image and create the code that will tell the plasma cutter how to cut the object. The code you create here will be imported into the Mach3 program installed on the plasma cutter computer.
- Click the File menu, choose Run post processor
- Name your file and save as a G-code (XX.tap) file. Note: Even if you try to add “.nc” to the end of this file type, it will still only be recognized as a “.tap” file.
- You will now be able to inspect the G-code at the bottom of the program window. If processed correctly, there should be X and Y coordinates in this code along with many G-code commands. SheetCAM will add in the start and stop commands between objects automatically and display the cutting path with lines and arrows.
- You will need to open the “.tap” file in notepad/mousepad and then click File, Save As and rename the ending of the file to “.nc” so that the Mach3 software on the plasma cutter computer will easily recognize the commands without issues. If you load the “.tap” file you may experience issues where the cutter will stop due to some elements of the code. Using and loading the “.nc” type file seems to eliminate any issues, even though the code is identical and unaltered.
If the 2D CAD drawing is created in FreeCAD, the tool path generation can be created directly using the Path workbench. There are a number of good video tutorials available on using the path workbench; however, almost all of them assume that a 3D object is being created on something like a milling machine. The process for a 2D plasma cut is even simpler, and can in most cases be accomplished by creating a contour path of your sketch.
Import Existing 2D design
- Import dxf or svg into FreeCAD
- Select all shapes, draft workbench, convert bidirectionally between draft and sketch
- Select all sketches, Sketch workbench, merge sketches creates new sketch
- Delete all other shapes and sketches
- Path workbench
Create Original 2D design
- Use sketcher to create design
- Change to path workbench
- Set output file name and change processor to linuxcnc
- Edit default tool for 80 in/min horizontal, 20 in/min vertical, click OK
- Create profile based on edges. Add edges using Geometry tab.
- Preview toolpath using simulator button
- Export .nc file using the post-process button
- Manually add stop (M05) and start plasma (M03 S1)
3. Machine Setup and Control
Set nozzle above workpiece with 1/8in shim
Jog the cutter where you want it and set x and y zero in Mach3
Test the programming by clicking cycle start
Speed and Power
The following table has been developed in-house. Please add to it with any experience you have.
|Material||Thickness||Speed (inch/min)||Amperage (Amps)|
|Carbon Steel||1/8 in||75||45|
|Stainless Steel||1/4 in||30||45|