|
. |
Part 9 - Machining - continued.
The next step is to specify the cutting tool geometry. The first pass will be a rough cut with a larger tool. Select the Cutting Tool Type "Ball". In the "R" (radius) field, enter 0.2 . Leave the "O" field set to zero. In the "H" (height) field, enter 0.15 . In the "D" (maximum cutting depth) field, enter 0.3 . Press the "Enter" keyboard key in any of these fields, and the spinning tool profile is drawn in the Cutting Tool window. Note that if "R" does not equal "H" for a "Ball" tool type, then the tool tip shape is actually elliptical. The "O" (offset) value must be less than the "R" value. It can be used (when greater than zero) for specifying bullnose bits and other specially-shaped tools. If the tool type is "Ball Taper", then the "O" parameter specifies the radius of the tip.
The final step to generating a tool path is to specify the tool path parameters. All of the Cutting Path types key off of the data coordinate scale origin. For example, the "Radial" path type uses the data coordinate 0,0 as the center point for the radials. Leave the Cutting Path Type set to "Traverse Horizontal". Machining can be performed on the entire surface, or it can be limited to an area specified by the current region. Leave the Cutting Path area mode set to "Entire Surface". The "Step-Over Spacing" field specifies the distance, in data coordinates, between each traversal. For a radial path type, this field is for specifying the angle, in degrees, between each radial. Enter a "Step-Over Spacing" value of 0.25 . The "Maximum Path Depth" field specifies how deep into the existing material the tool can go on this pass. This is measured from the original uncut surface heights. VS3D will never drive the tool deeper into the current (calculated) machined surface than the tool's specified Max Cutting Depth "D" parameter. Enter 0.25 in the "Maximum Path Depth" field.
Note that VS3D versions 1.4 and newer include additional tools for specifying the "climb" or "descend" direction of the tool path. Use the "CW / Climb" setting. Click on the "Make Cuts / Add To Protocol" button. If you are currently running a licensed version of VS3D then a form will appear for specifying details of the output file, including feed rates, spindle RPM, etc. The available settings will vary depending upon the "Machine Type" chosen for the protocol. Leave all of the default settings unchanged and click on "Ok". You will also be prompted to enter the name of the file to save if not running in DEMO mode. If you are running in unlicensed DEMO mode, all file output is disabled and no output file is saved, but the predicted results of the machining pass will still be displayed.
|
