In this skill builder you will become familiar with creating simple 2D drawings in VectorWorks (CAD), creating basic cutting operations in MasterCAM (contour cuts and pockets), and running a job on the CNC router.
You will need
1/4″ straight endmill
Flat sheet material
Eyes and ear protection
Create a 2D drawing in VectorWorks.
Make sure your drawing is in the top right quadrant of the XY Axis. This is a good habit to get into, it will save time at the CAM station.
Export as a DXF/DWG file and save to a thumb drive.
Before you begin the CAM, you must first know what type of end mill(s) you will be using and the thickness of your stock material. Measure material thickness using digital calipers. For this skill builder I am using a 1/4″ straight end mill and 0.475″ thick plywood.
Open the DXF file in MasterCAM at the CAM station located in the shop. You can view the grid by clicking F9.
Select the correct Machine Type, Techno Generic 4X Router.
Select the first Toolpath, Contour
Select the shape(s) you wish to perform the operation on.
If choosing multiple shapes, hold shift while selecting.
Inside or outside of the shape. If the arrow is pointing in a clockwise direction, the mill will cut on the outside of the shape. If the arrow is pointing in a counter clockwise direction, the mill will cut on the inside of the shape. Clock out, count in.
Select the tool
From the Select library tool, choose 1/4″ straight bit. If you don’t see it, un-click the “filter” checkbox.
Select Depth of Cut. Remember the rule of thumb: the depth of each pass should be no greater than the radius of the end mill you are using. We are using 0.25″ diameter end mill, so a depth of cut of 0.125″ is what we want.
Select if you want Break Through or not. For contour cuts, you typically want Break Through turned on.
In Linking Parameters, select the depth of the operation. The depth will never be greater than the thickness of the material being cut. Remember, the depth will always be negative. I have set the depth at -0.475″, the thickness of my material.
Select the second operation, Pocket
Select the shape(s) you wish to perform the operation on. If choosing multiple shapes, hold shift while selecting. Pocketing can be performed between two shapes.
Select the tool, 1/4″ straight bit again.
Select the depth of cut. Again the depth is 0.125″.
Select if you want Breakthrough or not. Typically for pocket operations, breakthrough is turned off.
Select the depth of the operation. For our pocket depth we only want to go down a depth of 0.35″. Remember, the depth will always be negative.
Cut out the outer shape using a contour operation. Select 1/4″ straight bit for the tool, 0.125″ depth of cut, and -0.475 for overall depth. The only thing different is you want the direction of the arrow to be clockwise for a cut outside of the line.
Order of operations is important. You do not want to cut out a part and then perform more operations on the part. For example, if you are cutting a wheel, you do not want to cut out the wheel and then the center axle hole. The wheel could move between the operations and the center hole could be off center. If the axle hole is cut first, then the wheel is cut out, the axle hole will always be centered.
Animate the Operations
Click the Toolpath Group and the the animate button.
Click the play button to see the simulated operations.
When you are happy with your operations, create the G-code and save it to your thumb drive. The file created will be a .nc file.
Bring your g-code to the CNC work station in the shop. Open up Techno Router Interface.
Open up the file by clicking “File”. Find your file on the J drive.
Set the Cut Speed and Plunge Speed for the intended material. 55 cut speed and 45 plunge speed are standard settings for plywood. And click Preprocess.
A run time estimation will be created (7 minutes and 22 seconds). You can preview your operations by clicking Preview button.
If everything looks good, you can close the view window.
Secure Your Material
Mount your material to the CNC spoil board using screws. Make sure the spoil board is clear of dust and not too chewed up. Secure the material so it lays flat.
Install the end mill
Select the proper collet and snap it into the collet nut. Thread it onto the spindle. Insert the end mill into the spindle and tighten using the two wrenches.
Once the material is secured and the end mill is in place, you have to set the X, Y, and Z origin. Using the X and Y jogging controls on the Techno Router Interface, move the end mill into the desired position. Bring the jog speed down to very low, and begin to position the Z origin. You want the mill to be very close to the surface of the material, but not touching it. When the mill is in place, click the “Zero” button and select “All”. Origin is now set.
It is a good idea to move the Z position up a few inches after setting origin.
Turn on Vacuum
Before you begin cutting, make sure the vacuum is turned on. You will need to wear eye and ear protection at this point.
Begin the Job
You begin the job by clicking the “Start” button on the interface. The button will then read “Resume”, click again, the spindle will come up to speed, and the job will start.
Be aware of where the pause (black buttom on the right), start (green button on the left), and emergency stop (red button in the middle) buttons are. You NEVER leave a job unattended. A job can be paused and restarted, but if you hit the emergency stop the job is lost.
When the job is over, let the spindle come to a complete stop and jog it back to the home position (back left corner). Remove the end mill, collet, and collet nut. Return all tools and equipment to their proper places. Unscrew and remove the material from the CNC bed. Vacuum up any dust created in the shop, especially the CNC bed.