Bracket Arm 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.
This tutorial will be on machining a bracket arm, which could be used for many applications.
The as part drawn in Rhino it is 4" long and 1.5" wide at it's widest section, and 0.125" thick. As you can see this part can only be held in a vice when being cut out of a piece of flat stock if the finishing pass is skipped. So I will make a simple jig using a clamping plate to hold the part allowing for finishing work.
1) Flat stock cut to rough dimensions, add an extra 0.25" to the length for good measure. 2) Drill holes in the center of each arc (3" apart on my bracket). Be careful that these holes are the same distance apart as the holes in you clamping plate grid. On my plate the holes are in 0.5" increments.
3)Aligning flat stock to clamping plate with machinists square. Spacers are underneath each screw to lift up the stock a little.
4)Flat stock attached to V4 F1210E high speed machine table.
DXF. Contours imported into BobCAD-CAM.
Select the outer contour while holding down the "shift" key this will select the entire "chain" instead of just one segment of the chain. Then go to the "Other" menu and select "offset" (Go to page 229 in your BobCAD-CAM Training Guide to learn about offsets more in depth). The offset distance should be half of the tool diameter plus about 0.003", since this is a roughing cut.
Below you can see the generated offset. The direction that the little arrows on the contour is pointing is the direction that the tool will go when milling. To change the direction of the chain hold the "shift" key down and put your pointer on the side of the contour in which the arrow is NOT pointing and click on the chain . The direction of the chain should change, this way you can choose between conventional or climb milling.

Leave the tool path 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. Your Rapid height MUST be above the screw heads that are holding the bracket. 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 at 2 (At this feed and with a 0.125" end mill the motor RPM can be around 4000).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.
The selected tool path should now be deselected, and the same offset as before should be made from the original contour, but only offset by the radius of the tool. Also climb milling could be used here since this is a finishing cut. Go to the tool depth settings and uncheck automatic roughing then do the process described before to produce the G-code.
Now you must offset the inside contours. Since they both have to be offset the same direction and distance we can select both of them, then preform the roughing offset, and generate the G-code(remeber to look at the tool depth settings window to make sure that automatic roughing is on for the roughing cuts and off for finishing cuts. Remember that the offsets must be toward the inside this time.
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 open the "File" menu and select "load G-code" find your file and load it. Now it is time to finish setting up the machine.
Turn on the spindle and make sure the motor is at about 4000 RPM (If you do not have a high speed model just lower your feed rate with the feed rate override in Mach2 once the program starts to about 8 IPM. Press cycle start and the machine should start cutting chips.
Use the edge finder on the lower screw head in order to get the center of the end mill aligned with the center of the screw. Once aligned zero the X and Y axis. Move the tool a little away from the screw and move the spindle down manually till it just barely touches the surface of the stock (method described in the Enclosure tutorial). Zero the Z axis.
Outside contour machined.
Part complete.
The finished part!!!!!