Maslow CNC Tutorial
In this tutorial we'll cut a Noisebridge sign designed in Inkscape.
- Creating paths out of text objects
- Cut types
- Bit locations
- Z-axis and material depth
- Tabs and router bit width
Quick Basics on CNC
You want to cut something. You have a thing that moves which has a thing that cuts on it. Sometimes you want that tool to "work" aka be cutting, and sometimes you don't, so the machine can move to the next cut. The way the machine knows to what to do and where to do it is location based commands which tell it where to move and how fast. For the Maslow, movement consists of left, right, up, and down. The z-axis for the maslow is the depth which the router bit descends into the material.
If you are using 3/4" wood and you want to be absolutely sure the cut goes through, then you need to specify the cut depth as > 3/4". In this case, 0.80" works great.
Use the text tool to write Noisebridge. Add a line underneathe with the line tool and surround it with a rectangle with the rectangle tool.
Select All and then go to Paths -> Object to Path. This will break each object up and create a set of paths. Paths are required for vector based plotter operations.
Once complete, save the drawing as a plain svg.
It's a web-based application and it's not great. Zooming is goofy, and undo does't work. However, if a mistake is made, it's possible to redo the operation, and at the end of the process, only export the operations you want. More instructions to come using other software but this is a good tutorial and MakerCAM can be to the CNC what Inkscape is to the Laser.
A note about selecting lines, it's best to drag the select square than try to click. Using shift and control to group works fine, just use selection dragging instead of just clicking.
The workflow is to load the file, define what kind of cuts are needed to produce your desired result, calculate the paths, add tabs, and export gcode.
Set the text cut, which will only go partially through. For this sign we want the letters inset, so we will cut the inside of the shape.
- This cut will cut out a complete closed shape, but the side of the cut needs to be determined, e.g. inside or outside the line. Inside and outside only make sense if the shape is closed.
- A follow cut puts the center of the bit on the line.
- A drill puts the router bit in one places and drills a hole to the desired depth.
Cut letters with a Profile Cut
- tool diameter
- the diameter of the router bit. The Maslow should have a 1/4" bit on it but this is Noisebridge so please check.
- target depth
- How far from the front face (e.g. z-axis zero) should the bit drive into the material. In this case, we do not want the bit all the way through, so we pick some reasonable distance into the material.
- Determines which side of the shape we chose will be cut. If we cut "inside the lines" for the text, it will be inset into the wood, which is what we want. If we choose "outside" then the wood around the text will be routed, outlining each letter.
- safety height
- how far to pull the router up. Note this is positive, so it is 0.50" above the zero, which should be 0.50" above the marterial.
- stock surface
- surface of the material in z-height (e.g. the zero on the z-axis) if not actually at the zero'd value for the z-axis
- step down
- the cuts don't go all the way through at once becuase this puts a lot of stress on the router bit. However, if the depth is 0.80" and the steps are 0.05", it's going to take 16 passess to cut. No thanks. This can safely be increased to 0.15" or 0.20".
- feed rate
- how fast the router bit moves laterally when in the material
- plunge rate
- How fast the z-axis moves into and out of the material.
Cut underline with a Follow Cut
The line underneath the letters is not a closed shape. To cut something like this, use a follow cut where the bit will just trace the line.
The options are a reduced set from the profile cut. There's no selection of which side of the line to cut.
Cut the outline with a Profile Cut
To cut the sign out of the wood we use another profile cut. This time we do want the router bit to go all the way through.
The options are almost identical to the first profile except here we cut the outside of the shape and cut to a depth of 0.80", which will cut all the way through the material (which is 0.75" thick).
We cut the outside because if we measured the sign to be 6" by 48", cutting the outside means we get 6" x48". Cutting the inside will subtract the width of the bit from each side, making the sign smaller.
Calculate final paths
Once all the cuts are defined, MakerCAM will calculate the final path. This creates the exact path the tool will follow, where it will drill into the material, how far, etc.
If a completely closed shape is being cut out, for example the entire sign, then tabs should be used as small connective material to keep the sign in place while the cut is performed. If not, then there is a risk the sign will begin to fall, and will mess up the cut.
After calculating all the paths, green and blue lines will be available. Select either for the line you want to tab, which is the outline inn this case.
Use the CAM add tabs to selected menu item.
- tab spacing
- Tabs are defined by spacing, e.g. how far apart they are. Use your best judgement based on the thing you are cutting. It would be nice to say "5 tabs pls" but like whatever.
- tab width
- must be greater than 2x bit width. Let me say that again. MUST BE GREATER THAN 2X BIT WIDTH. 1/4" bit means > 1/2" tab. I use 3x bith width.
- tab height
- the tab does not need to be the entire height of the material. In fact, more tabs with lower height can be easier to deal with when removing the sign. Thick tabs mean you have to work at getting them out vs. just pulling the piece off and sanding it down.
You can move the tabs around if you want. just click and drag.
MakerCAM will provide you a list of all the cuts you created this session. If you want them all, just click all, export selected toolpaths.
If you know you don't want them all, then you can select which ones you want, but honestly it gives no real indication if what they were so like...whatever.
Ok, in Ground Control, click "Actions" and Open the file.
(If you haven't already, click "ports" and select the port the Maslow is running on and then click "Connect")
Ayyyy, there it is. Ok, the red circle with an X is the router. If the router and sign are not aligned at the bottom right corner, hit "Define home". Move the router around using the purple D-pad so the sign is cut where you want it to be. Make sure you hit "Define Home" when you are good, basically like hitting "origin" on the laser.
The dotted lines are the traversals where no cuts will be made.
Solid lines will be cut
Red and Green circles are Pen up and Pen down. You can see where the tabs will be on the outline cut by noticing where the red and green circles are separated.
Ok, all set! Hit the Green Play button and go work on something else for a while, this will take a bit.