Aluminum Enclosure Tutorial
This tutorial is designed to help you become more comfortable with the MDA cnc machining system. This tutorial will be going over some basic, yet very powerful ideas, which will allow you to make a variety of different parts.
MDA Precision deems the below information to be correct, but holds no responsibility for user error, or misprints.
First we must draw the part in CAD program. I drew my part in Rhino, but any CAD program can be used. The dimensions of this part are: 1.5" by 2.25" by 0.5".
Save the 2-D contours of the part and open it in BobCAD-CAM, or draw the part in BobCAD-CAM to start with. Below is a shot of the imported dxf file from Rhino.
The first thing we have to do is offset the inside contour by about 0.003" torwards the inside to allow for a finishing cut at the end. This can be done by firstly clicking on the inside contour while holding the shift key to select the chain, then going to the "Other"menu and choosing "offset".
Now we are ready to pocket. Select the offset contour if is not already selected by clicking on the contour while holding the shift key down. Now go to the "other" menu again and choose "pocket" then select "spiral" enter the tool diameter, then enter the radius of the tool at the "distance between lines" box, make sure that "Contour is first path" is NOT selected and click OK. You now can follow the instructions on the bottom left hand side of the BobCAD-CAM window, since we have no islands you only have to press enter and the tool paths appear.
Leave the tool paths selected and go to "Special/NC Cam" - "Insert NC" then choose "MACH2 MILL". The NC window appears. On the left side of the NC window there are various icons, click on the tool depth settings button. This window allows you to control the following: the top of the material, what height rapid movements will take place at, how deep your tool will go, how deep each cut should be, and your feed and plunge settings. Remember to be conservative with your feed settings for now as you can always increase them while the program is running in Mach2. The feed should be set to around 10 and the plunge to 2(At this feed the motor RPM can be around 3000).Also enable "Automatic Roughing" and Max depth each Cut should be about 0.1". Now click "OK" and go to the "Machine" menu and select "Auto" the G-code for the selected tool path will be created according to the tool depth setting you just entered.
Go back to the drawing window and press the delete key to delete the tool paths. Now it is time to create the finishing pass. Select the original inside contour and offset it inward by the radius of the tool. Go to the tool depth settings in the NC Window and deselect the "Automatic Roughing" option. Now go to the "Machine" menu again and select "Auto", the G-code is produced and pocketing complete. Save the G-code file by selecting "file" in the NC window and "Save a copy as", name the file and make sure it is in the ".tap" format.
Now start up Mach2 Mill and choose the MDA Precision Profile. Go to "File" then select "Load G-code" choose the file you just saved in BobCAD-CAM. Below is what you should see.
Before you start the program you must center your end mill on the lower left corner of the work piece. You may use a electronic or mechanical edge finder to do this. Once you have found an edge zero it's axis. Once both of these edges are zeroed move to a safe Z. Now go to the MDI(F2 key) window in Mach2 Mill here you can directly input commands to the machine. Click into the large yellow box at the bottom of the page and enter G00 X"Radius of edge finder" then press enter, G00 Y"Radius of edge finder" then press enter. Go back to the "Program Run"(F1) window and zero the X and Y axis.
Finding the edge in the Y axis.
 The Z axis can be zeroed by loosening the spindle and lowering it till it just barely touches the surface of the part then tightening the spindle securely again.
End mill centered in X, Y, Z.
Turn on the spindle in Mach2 Mill "Spindle CW" and make sure the RPM is correctly set. You will want to lubricate and cool the tool during this pocketing procedure, if you don't have a coolant unit use some cutting oil or WD-40. Now to start the program click "Cycle Start Alt-R" the program will began. The above process may seem long when described in words, but with a little practice it will only take you only minutes to complete this whole process.
Pocketing in process.
When the pocketing is finished we can proceed to drilling the holes.

Proceed to next Section