CNC file preparation (CAD)
This page is still a work-In-Progress. If you have any feedback or suggestions on things that need more or better explanations, please let us know by filing an issue here on Github or send an e-mail to cnc@fellesverkstedet.no! Your input makes this wiki better! :-)
On this page we explain how to prepare your digital files for cutting by using the Shopbot at Fellesverkstedet. A large part of preparing your files will depend on your specific project but below are a few general guidelines. Preparing files for CNC-milling has 2 steps: First you design your file in CAD-software and then you use CAM-software to generate the files that will run the machine (CAD stands for Computer Aided Design and CAM stands for Computer Aided Manufacturing). Below we'll talk about the CAD part of preparation.
(Note: The software Fusion 360 is both CAD and CAM-software in 1 package but currently you're more on your own in terms of preparing the CAM-file, since we don't have much experience at Fellesverkstedet in using Fusion 360)
Go to:
-
- Filetypes & software
- File-prepping
- Precision, units & tool variables
- Lay out pieces to be cut
- Hold down circles
- Bonus: layers
- Going from 3D to 2D
The first thing to consider is whether you will be cutting a 2D file or a 3D file. In general 2D files have quicker production and preparation time in CAD in comparison to 3D files (although there are exceptions). 2D files are often used for cutting out pieces out of flat plates that can be assembled afterwards or for engraving text or a logo, or both. 3D files are mostly used for making 3D shapes like sculptures, molds or landscapes for architecture models.
comparison of 3D vs 2D cutting. The red lines show the way the machine will run. In this case it obviously makes more sense to do 2D cutting
Click to expand!
The important part about 2D cutting is that you need to have a vector file as a .dxf (.svg works as well) that we can import into v-carve. You DON'T need a 3D file, but in certain cases it is possible to retrieve 2D vector file information out of 3D models. Also make sure your file doesn't get crazy large (>50MB) or the CAM-software might have issues dealing with them.
Dxf files can be exported from most 2D vector-based software like illustrator, inkscape, etc or using most 3D CAD-software like Rhino3D, Onshape, Fusion 360, Autocad etc. (if you use Affinity designer it's also possible to export as .svg)
Note: importing a non-vectorised image into a vector-based software and exporting that image straight to a dxf does not result into a correct vector file. There are however ways to automatically convert images to line drawings in Inkscape or Illustrator. Search for "Image Tracing" + the software you will use to get guides on how to do this.
In your drawings you will need to consider the different operations you want to execute with the machine. These operations are called toolpath operations and the 3 most common are Drilling, Pocketing and Profiling (= Cutting).
- DRILL (requires a closed curve) will make a hole in the center of your curve with the diameter size similar to the milling bit. You can choose if it drills all the way through the material or only to a certain depth.
- POCKET (requires a closed curve) will clear away everything inside the curve to a specified depth.
- PROFILE (can be both open or closed curve) cuts on the outside or inside of a curve and compensates for the diameter of the milling bit. This is used for cutting out pieces and is therefore the most common operation.
comparison of different types toolpaths, as described above, to the same geometry. The blue line is the geometry where the toolpath is applied to, the red lines show the way the machine will run with the milling bit.
When you prepare your drawing you place curves according to how things will be cut out. The most important things to remember is that you will get round off inside corners due to the milling and that you will need some spacing in between pieces to fix materials to the machine.
Prepare your drawings in mm, as this is the unit system we will use later in VCarve (CAM). The shopbot has a precision of 0.05 mm so if you have pieces that slot into each other you'll need to be precise with drawing. Joints can be drawn without tolerance as we can add that later in Vcarve.
For cutting through materials the shopbot uses a milling bit. The diameter will greatly depend on the material and thickness you are trying to cut and an important thing to be aware of is that inside corners will get round off to the radius of the milling bit. This is something the milling machine does automatically, so no need to add this to your drawings, just something to be aware of.
However, if you would like to engrave something with precise corners, it is possible to use a v-bit in combination with the V-carve engraving toolpath in Vcarve. The V-bit will then move up in the corners to the tip of the bit.
To lay out the pieces for cutting, you first draw a shape with the dimensions of your material. (Most common full sheet size is 2440 by 1220 mm).
Then position the pieces that will be cut inside the material. Leave enough space from the edges of the material as you will need space to screw the material onto the machine later. 25 mm from the edge is safe when using a 6 mm diameter bit.
In case you have multiple pieces to cut, leave enough space between the parts as the diameter of the bit needs to pass in between them. Having 25 mm between the pieces is safe for a 6 mm diameter bit, since then we can place holes for screwing in the material.
Note: both these distances can be pushed to a certain extent but require more attention when preparing the files in the CAM-software and during the milling process.
Before milling into the material you'll need to make sure that the material is fixed to the machine. We do this by screwing down the sheet onto the sacrifial layer. It's important to not hit those screws when milling and the solution for that is to use the machine to mark where to put the screws by drilling into the material. If you draw circles with a diameter of 25 mm around your parts, you can use these to drill in the center of that circle and mark the position of the screw (this also explains why we have 25 mm as a suggestion of space to keep between the pieces as written above here). More explanatory images on this topic will follow.
This step is not necessary but will make things easier when setting up the job later in Vcarve. Put the curves that have different operations onto different layers with their own colors.
In a lot of cases when trying to make cabinets & furniture you'll want to create 3D objects out of flat sheets of material which you can assemble after cutting out. Often, but not always, the easiest way to do this is to actually draw the objects in 3D so you can double check if sizes and location of possible joinery is correct. Then you lay these pieces flat and convert them to 2D lines which can then be exported as .dxf.
It is however possible to skip the step of drawing things in 3D and just draw it straight in 2D, but by seeing how things are in 3D there's less room for errors. In either technique it's important to be very precise in you drawing: If you have joints that need to fit perfectly together, drawing 0.1 mm wrong can cause things to not fit together afterwards in some cases.
Click to expand!
For 3D milling you will need an .stl file of the object you want to mill. In case your object is bigger than the material you have OR bigger than the max thickness we can mill (6 cm), you will need to split up the model into separate pieces. Each piece then becomes a separate .stl file. Make sure to not have too big files that are hard to import (>500 MB)
Since we only have 3-axis machines at Fellesverkstedet, you'll want to avoid undercuts. Undercuts are cavities that the milling bit cannot reach because of the limit of the axes, as shown in the image below.
However, there are ways to split up your 3D model into separate parts which can then be milled and afterwards glued together as shown in the image below.
Depending on the shape or model you are trying to create, this can get quite complex, so if there's the opportunity, try to simplify what you are tying to do as much as possible.
With 3D-milling, things can sometimes get a bit complicated as there's more factors to consider then with 2D/2.5D-milling (though not always). If you're using a ballnose milling bit there's no way to create perfect sharp corners, as shown in the image below. Note: this is only the case for inner corners. Outer corners shouldn't provide an issue.
The diameter of you milling bit will also decide the detailing that you're capable of milling. At the same time, the diameter decides how much time it takes to mill so you need to find a balance between how much detailing you would like and how much time you would like to spend milling. In some cases it is possible to use a smaller diameter milling bit in the areas where the bigger big cannot reach, but this is often hard to get perfect due to a different tool deflection of a different bit.
Click to expand!
The next step is importing your vectors into VCarve and setting up the toolpaths that will run the cnc-machine. This step you can do at Fellesverkstedet, or try to prepare at home by downloading VCarve (PC only):
IMPORTANT: The makerspace license that's connected to the master license at fellesverkstedet is 22965-DCBF2-A242E-5E47B-46AAF-40E3B-21D3C. You will need to enter this license into Vcarve or else you won't be able to open your vcarve file at Fellesverkstedet. This license provides all Vcarve functionality except for exporting the toolpaths to Shopbot Code (which runs the machine). This final step you'll need to do using the pc's at Fellesverkstedet which run the master license of VCarve.
Download the free trial edition of VCarve Pro on this link and activate it with the license code above. No license code means you won't be able to use the vcarve file at Fellesverkstedet. Also license codes from other organizations will not work with Vcarve at Fellesverkstedet. See image below to find out where to enter the license code
//
For getting access to the same milling bits as at Fellesverkstedet you can download our tool database here and import them into vcarve (see image below on where to find the button to import the database).
If you cannot get it to work, no worries, just prepare your files with one of the standards bits that come with Vcarve software and remember to change the speed settings at Fellesverkstedet before exporting the toolpaths.
Click to expand!
Nesting: In the Top plane, draw a sheet in the size of your material and position your separate pieces to be cut into this sheet, using the guide lines described above. If you don't know how to lay pieces flat, check out this video which explains the process.
Exporting: After you prepared the sheets which you will be cutting with the pieces positioned inside, create a new sketch in top view and project the faces that you will be cutting (so both pockets and cutouts) into this sketch. Now you can finish sketch and export the dxf by right-clicking on the sketch and pressing "Save as Dxf". You will then be able to import this dxf ino Vcarve where you will define what needs to happen to the different lines.
Click to expand!
If you have a hand draw sketch which you would like to digitize and turn into a vector drawing for cnc-milling or laser-cutting you'll first need to make a picture of it. You can either do this with a camera but the best it to use a scanner as this will give better results when converting it to a vector drawing in a later stage. What you want to end up with is either a .jpeg, png, bitmap, etc (pdf might work as well). When you have this continue to the next step below:
Click to expand!
There's a bunch of software that can convert images containing pixels (jpeg, png, bitmap, etc) into a vector which can be used for cnc-milling or laser-cutting. Most commonly used software doing this are graphic design softwares like Illustrator or Inkscape(free) but there are also some online converters that do it in the browser (although we've never tested these). The process is called image tracing in case you'd like to google if you can do it with the software you work with. Below are a few links explaining the process in different software but there's probably a lot more video explanations on youtube.
http://write.flossmanuals.net/start-with-inkscape/tracing-an-image/
After you converted your image to a vector drawing you can export your file to dxf for using at the cnc.