Machining the Car Prototype

Bottom Region

General information:

Make sure that there are no undercuts when machining the bottom region of the car. This specifically refers to the wheel well areas.

Use one operation with multiple nc sequences for the bottom region. This is important when creating the manufacturing information file at the end of the task.

Specifically:

Start by creating a work piece that is larger that the body of the car. The work piece should be ½” longer (to allow for ¼” extra on each end), ½” wider (to allow for ¼” extra on each side and ¾” taller (allowing for ¼” extra at the top and ½” extra at the bottom).

The ½” extra at the bottom of the car will be used for fixturing purposes when machining the top side of the car.

Suppress the cuts that were made into the underside of the car to save 3-D printing time and material.

Assemble the car and work piece in manufacturing mode. Make sure that you properly center the car in all three directions according the to extra material that was included in the work piece as defined above.

Use Analysis – Measure – Surface/Surface to get the model properly centered.

Create a detail drawing showing the car assembled to the work piece (full size). Notice that the model is the assembly model for manufacturing mode. Include as a reference dimension the distance from the bottom of the car to the bottom of the work piece. Also include the dimensions for the overall work piece. These are important for creating the physical work piece itself. Print this on B size paper.

The work piece we will start with will actually be larger than is indicated on the drawing. The reason for this is that we cannot make a work exactly to these dimensions, but we can machine an oversize piece to exactly this size. The reason it has to be exact is because we will be turning the part completely over to machine the opposite side, and need accurate touch off locations. Remember, we can not machine undercuts.

*************************** NOTE ***************************

A different coordinate system had to be created after this document was written. The CNC Router has problems with movement along the X axis, therefore a new coordinate system was generated where X is along the short axis of the car, Y is the long axis. All the tool paths had to be regenerated to effect this change. You will notice that the original coordinate system shown in the remainder of this document has X along the long axis.

Make SURE that you have X along the short axis!

**************************END NOTE *************************

Profile the rough block to exact size. Create a mill surface for this operation before starting to create the tool path. You cannot select the sides of the work piece dynamically during the tool path creation process, but you can copy surfaces to create a mill surface.

Use a step depth of 1”, and a feed of 60”/minute. This feed rate can always be over ridden at the controller.

We also need to Face mill the bottom surface as you will find that the foam blocks do not have parallel sided (especially after gluing up pieces). In order to face mill to location 0 in the z direction (which is also the under side surface of the work piece), you will need to create a mill surface to be able to select this surface to mill. From model won’t work. When creating the mill surface, use Copy. By definition, face milling operations lace the tool in the X direction (slow axis on the router). Use the Advanced button under Parameters to set the CUT ANGLE to 90 degrees.

In order to rough mill the underside, a mill volume needs to be created. We need to leave a pedestal under the bottom for fixturing purposes when doing the top side. To accomplish this, sketch a rectangle inside the outside edges of the mill volume. The tool will not machine this area. Offset the outer edges by about .35 from the work piece if you are roughing with a ½” diameter tool.

Mill volume in wire frame. The “bottom” of the volume must be positioned that it encompases any undercut geometry (when machining the top portion of the car), and should extend slight above the bottom of the work piece.

Shaded mill volume region. Note that the tool will leave a rectangular piece in the center of the car.

When creating the tool path, do a rough and profile and use a Rough_Stock_Allow of .125 to avoid any surface gouges with the flat tool. While Vericut appears to report gouges on the right side of the part, Pro/E does not indicate any problems at all (even after doing a gouge check).

Create a surface milling sequence to do the outer body panels from the bottom side. You do not have to worry about Pro generating tool paths for the under cut geometry on these panels. Use what you learned in doing contour surface milling to do this.

Next create the tool path to do the wheel wells.

After running all tool paths in Vericheck:

It doesn’t do any good to save this picture as an In Process model in Vericut. Even though the object can be rotated about the X axis so you think would be able to show the machining of the top portion, you can’t. The reason is because the version of Vericut that is licensed to us cannot deal with multiple coordinate systems.

Produce a mfg.inf file of this entire operation.

Search through this file to get Cutting times for:

Entire Operation XX.XX minutes

Profile (Outside of Work piece) XX.XX minutes

Roughing XX.XX minutes

Surface Mill of Body XX.XX minutes

Surface Mill of Wheel Wells XX.XX minutes