Production of the Body for the Wooden Toy Project An Introduction to the CAD/CAM Process

1. Using Axyz ToolPath to Produce a Numeric Control (NC) Program Production of the Body for the Wooden Toy Project An Introduction to the CAD/CAM Process Instructions for 3 Axis Programming for use with the Axyz Millennium Router

2. In SolidWorks, open the “part” drawing of the body of your toy.

3. Orient the view so that the “part” is in shown in profile (front view).

4. Find and open the “sketch” that includes the “extruded cut” for the axle holes.

5. The diameter of these holes will need to be set to a fairly small diameter so that a contour cut with a ¼” cutter will make the holes have a diameter slightly over ¼” . A diameter of .02” is recommended.

6. Exit the sketch to return to the “part” drawing. The diameter of the holes will be greatly reduced, but remember, the ¼” cutter will be making a “contour” cut and will be following the center line of the drawn circle.

7. Next, use the “Features” function to “sketch” a rectangle around the “part” that represents the perimeter of the material that will be used . Use “Extrude Boss/Base” and “sketch” the material perimeter. Set the dimensions for the rectangle and “center” the “part” in the rectangle by using the dimension tools. Material perimeter

8. Exit the sketch and then instead of “extruding” the material perimeter, exit the “extrude” function. The sketch lines that remain in place will be used to create an origin point for the CNC program that will eventually be produced. If you are producing “pocket” cuts on both sides of the “part” be sure that the “part” is centered precisely side to side inside the perimeter lines.

9. Once the material perimeter is placed around the “part” use “Save As” and save this “part” diagram. USE A NEW NAME AS TO NOT CORRUPT OR CHANGE THE ORIGINAL PART. From this new “part”, select “Make A New Drawing”. Use a totally blank sheet (turn off display format) and insert either the front or back view of the new “part”. No other views are needed. Use “Save As” and save this “drawing” as a .DXF file. This is the drawing that will be imported into the machining software. Exit SolidWorks.

10. If you are producing “pocket” cuts on both sides of the “part” be sure to produce a .DXF file for both sides of the “part”. You will eventually need to produce tool path programs for both .DXF files.

11. Once the .DXF file(s) has been produced, open the Axyz ToolPath software to begin creating the CNC program for cutting out the various elements of the “part”. The various elements that will need to be cut include the axle holes, any pockets and the body of the part.

12. When opening the .DXF file in ToolPath, select the file location, the “Type of File”, the “File Name” . Be sure to have “DXF Files” selected as the “Type of File”. Select “OK” at the prompt for “Available Machines” and “DXF Error”.

13. When the file opens check “Layout” to insure the “part” has been imported in the correct scale and unit type. The sizes listed should match the drawing originally produced. If they are, select “OK”, if not return to SolidWorks to check the “Units” & “Scale” of your part drawing.

14. In the next step, any extraneous drawing elements will need to be deleted from the imported image. If there are none, move to the next slide. If there are, follow these steps: Select “Edit” from the main menu. Select “Erase” from the edit menu. Use the cursor to click on any items that need to be erased and then select “Erase Shapes”. v When finished, return to the “Main Menu”.

15. Next, select “Analysis” to correct or compensate for any potential cutting errors. In the “Analysis” dialogue box click on “Duplicate Shapes”, ”Direction Errors” and “Sequence Errors” buttons. All 4 error indications should now read “0” (there should be no “Open Shapes” in this project.

16. The imported data will now need to separated for each of the individual machining processes that need to take place. Select “Groups” and “Move to Group”. Click on the axle holes, select “To Group” and then “Blue”. Select “Move to Group”, select any items to be pocket cut and then “Green” (if none, skip step). Select “Move To Group”, select the body perimeter and then “Yellow”. Once the “groups” are made, select “Main Menu” to exit.

17. The “Output” parameters for each process now need to be set. Select “Output” from the main menu. Set the parameters for each of the “groups”. Turn the “Machining Path” “Off” for the “White” group (click in the space marked “Forward”). No processing will take place in this group since the only item in the “White” group should be the material perimeter which does not need to be cut. Set the “Depth” of the “Blue” group to the material thickness plus approximately a 1/16” of an inch to be sure the bit cleanly cuts through the material (1.875” + .0625” = 1.94”). Turn on the “Multipass” for the “Blue” group and set the “Pass Depth” to .2”. Since a ¼” cutter is to be used and the depth of cut should never exceed the cutter diameter. If there are any “pocket cut” items, set the “Depth” in the “Green” group to the depth set on your plan and set the “Multipass” for the “Green” group if necessary. Set the “Yellow” group (body perimeter cut) to the same “Depth” and “Multipass” parameters as the “Blue” group.

18. The preliminary “Output” settings are shown below. Your data should be identical in all areas with the exception of the “Green” group.

19. The cut for the body will need to have the tool path “compensation” changed so that the cutter will travel ½ of the bit diameter outside of the line drawn indicating the body perimeter. By changing the “compensation” the body will be cut exactly to the size drawn. Check to see if the “compensation” is “positive” or “negative” (inside or outside the shape). Select “Compensation” in the “Yellow” group. Select “.500” and “+”. Select “Send” from the bottom of the “Output” menu, “OK” from “AvailableMachines” and view the tool path diagram. If it shows a tool path smaller than the body the “compensation” is negative. If the diagram is larger than the body the compensation is positive. Select “Cancel” from the main menu and then “Output” to return to the “Output” menu.

20. The “Yellow” group compensation should now be set to .125” (the cutting bit radius) and indicated as either positive or negative based on the test you did at .5”. A quick verification to check the accuracy of this size and location could be performed at this point using the same process as described on the previous slide. The tool path in the diagram to the right demonstrates the slightly larger, but accurate path that should occur.

21. The final parameter that needs to be set is the “Tab” feature. “Tabs” are small areas of the body perimeter tool path that will not be cut. These areas secure the interior material so that it does not dislodge from its location and become damaged. Select “Tab Width” from the Output menu. Click on “Tab Width” on the dialogue box. Select 7.00”. Enter “2” in the “Number of Tabs” space. Select ”Ok”.

22. This is an example of the final Output menu. There may be differences in the “Yellow” compensation entry and the overall “Green” group settings. Save the program by selecting the “Save Ready File” button at the lower right of the screen.

23. Save the file in an easily accessed location. It will now have a .RDY file extension associated with it. Exit the Output menu by selecting “Ok”. You may now exit the software program.