Fab Academy 2017

The CAM process

To prepare the job for cutting, one needs to make the cam file. This is a calculation of the pathways the cuttinghead makes to cut the pieces, so there are a good deal of settings to look at.

Initially one needs to define the basic setup, where the zero is on the job. In this case I used the edges for the top of the desk as the X and Y, and used what would be the bottom left corner for defining the origin.

Setup - Tab: Setup

Operation type: Milling
Orientation: Select X&&Y Axes
X Axis: Selected Edge
Y Axis: Selected Edge
Origin: Selected Point
Model: 3 Bodies

With these one can define what edges of the piece are the axis used in making the command file. With this you also define the XYZ origin for the piece. Through here you also define which pieces are to cut, by selecting the model bodies.

Setup - Tab: Stock

Mode: Relative size box
Stock Offset Mode: No Additional Stock

With these you can tell the program how big the piece is, and how big the stock material is. In simple 2D CNC cutting its not necessary for the machine to know if there is extra stock around the piece. You just set the zero properly before starting the job.

In general with our machine it is a good idea to define the top of the piece as the origin so all the Z value will be negative, and if the origin is also in the bottom left corner for the piece all X and Y figures will register as positive.For our machine the X is the shorter axis.

Once the origin point is properly defined, you need to define the material size. In this case I used relative box size, so that the program uses the furthest points of the model as the corners for the stock.

Now that the basic setup is done, and the sotware knows its origin we can begin defining the job further. For this run I used the simple 2d contour.

2D Contour setup - Tool

Tool: #6 - 6mm flat
Coolant: Disabled
Spindle Speed: 15000rpm
Cutting Feedrate: 5000mm/min
Plunge Feedrate: 100mm

These values dictate how fast the CNC machine can move while cutting the material. How fast the bit has to spin, how fast the head should move. Cutting Feedrate dictates the XY axis movements while the Plunge feedrate dictates the speed for Z axis.

If you plan to run a lot, you will want to make your own tool definition, that has all these values bound to it. Otherwise these values get reset as soon as you close the program.

2D Contour setup - Geometry

Contour Selection: 8 chains.
Tab Shape: Rectangular
Tab Width: 6mm
Tab Height: 1,5mm
Tab Positioning: By distance
Tab Distance: 48mm

Through here you can define what edges are cut as 2d countours. in this case I had 8 edges or, 8 chains to cut. also I used tabs, that are little bridges left behind on the bottom of the cuts, they hold the pieces in place while they are being cut.

First we need to define the tool used, we use the 6mm flatheaded tool for these runs. The machine also needs to know how fast it should run so we also need to define the feed and speed settings. When picking the tool, each tool already has a set of predefined settings, that then can be edited for the job. If you need these settings to stick permanently you can define your own tool, and input the settings there.

For the geometry, you need to pick the bottom edges of each of the piece or feature you want to cut. Tabs are useful to use, their purpose is to make sure the piece stays in place while it is being cut. Otherwise the piece could move and lodge into place and cause damage by breaking the tool or cause other issues.

2D Contour setup - Heights

Clearance Height: 10mm - From_ Retract Height
Retract Height: 5mm - From: Stock top
Feed Height: 5mm - From: Top height
Top Height: 0mm - From Stock top
Bottom Height: 0mm - From: Selected contours.

The next tab for the 2D contour settings is the heights, in general these do not need to be messed with, unless you have a extraordinadely uneven piece that exceeds the default distances.

2D Contours setup - Passes

Maximum Roughing Stepdown: 2mm
Rough Final: True
Order by Islands: True

Another important setting to check is the multiple depths, without this the machine will try to cut the piece with just one run. From here you can set the depth for single pass, and the program will automatically calculate how many passes it need to make to make the cut. If you need to do fancy work, you can define finishing stepdowns and how deep they are made.

2D Contours setup - Linking

High Feedrate Mode: Preserve rapid movement
Allow Rapid Retract: True

These settings allow you to tell to the machine if it needs to slowdown, or if it can keep going on high speeds, and if it needs to be careful in pulling the bit up or not.

Leads and transitions lets you tell the machine if it can plunge right down when starting a jog, or if it needs to slide down into or out of it the material. These depend more on the material and its needs.

Once these settings have been done, you can simulate the run, to see if there are any issues, but usually with the 2d runs there wont be that many. The simulation also gives you an idea of how long the run will take, and you might want to go back to the settings to speed things up if it seems like a really long run.

Now that you are happy with what you have, you can make the post processing, which is a translator that takes the toolpath you designed, and turns it in to the dialect of G-code the machine understands.

Each machine has its own postprocessing instruction code, you need to take the file you have, and put it into the configuration folder. Copy-paste is your friend.

Then the program sees the post config file and you can choose it from the list.

You will want to give the program a name so you know what is the file you made. Finally let the program open it in an editor so you can inspect the file, for things like if the Z goes below the value defined as thickness. Such oddities would indicate you have a problem in the setup.

The paperwork

Assesment

Have you Explained how you made your files for machining (2D or 3D)?
Have you,Shown how you made something BIG (setting up the machine, using fixings, testing joints, adjusting feeds and speeds, depth of cut etc)?
Have you, Described problems and how you fixed them?
Have you, Included your design files and ‘hero shot’ photos of final object?