1. Using Surfcam to Produce a Numeric Control (NC) Program
An Introduction to the CAD/CAM Process
Instructions for 3 Axis Programming Using the
D&M CNC Milling Machine
Production processes for the plastic key fob project

2. The CAD/CAM process consists of the following steps:
The production of a drawing using a CAD program.
The identification of the types of cuts to be made and the sequence of the cuts (NC).
The Post Processing that converts the tool path sequences into G-Codes for use by the machine.
Making the part on the machine.

3. To produce the key fob for this exercise you will need to follow these general procedures:
Create a 2d drawing using SolidWorks.
Save the drawing as a .DXF file.
Open the file in Surfcam.

4. Surfcam Instructions Open Surfcam from the desktop on the computer.
Open the file that you need to have converted to G-code by selecting the location, file and file type.

5. Once the file is open you will need to make the following settings
for converting the 2d .DXF data to Surfcam data.

6. Select “NC”, “2 Axis” & “Contour” to begin.
Even though you are using a 3 axis machine for the actual work,
the layout for the process only requires 2 axis .
“Contour” means cutting directly on the line.

7. Select the inner most lines for cutting first
Select the inner most lines for cutting first. Use “Single” to select individual lines, arcs or points by clicking on them. Use “Chain” to select groups of contiguous lines and arcs. Click near the beginning of the group you wish to “chain” and then again near the end of the group. Selected items will be highlighted in yellow. Select “Done” when you have selected all of the items to be included in this process.

8. After selecting “Done” the “Tool Information” dialog box will appear.
Select “Select Tool” to identify the type and diameter of cutter to be used.
In the dialogue box that appears select a 1/8” diameter, 2 flute end mill – this will be the tool used for the cutting of the material in this exercise
.125
After selecting the cutting tool, enter the feed and plunge rates for the process.
For this exercise use a feed rate of 15 ipm and 5 ipm for the plunge rate.
The material selection will be made next.

9. Do not exit the 2 Axis Contour dialogue box yet!
Select “Select Material” and choose “Mahogany”.
Even though you are cutting plastic, the material properties are similar.
Do not exit the 2 Axis Contour dialogue box yet!
Select “Cut Control” to set the remaining features.

10. To control the cuts for this exercise, set all of the parameters as shown to the right.
The “In Z” data includes 2 critical numbers. The “Amount To Remove” is the total depth of the cut. The “Rough Spacing” is the amount of material that should be removed in one pass of the cutter. It is the same number for this exercise.
Once these parameters are set, select “OK” to exit the 2 Axis Contour dialogue boxes.
The NC parameters for the cutting of the letters on the key fob are now complete.
.25

11. The tool paths for the NC program have now been identified
The tool paths for the NC program have now been identified. Red lines will be seen on the 2d drawing indicating cutter travel in the G00 (Rapid Move)mode.

12. To see the all of the tool paths that have been produced, select “View”. In the View dialogue box double click on “Isometric view”.
White lines represent the original drawing data, red lines the rapid (G00) tool movement and green lines the actual contour cuts (G01, G02 & G03).

13. Select “View” again and then “Top” (double click) to return to the top view of the drawing data.
The next NC process will now need to be addressed.
Following the concept that interior elements need to be cut first, select “NC”, “2 Axis” & “Contour”. Select the small circle using the “Single” tool.
At the “2 Axis Contour” dialogue box, leave the tool and material information as previously set.
Select “Cut Control” and change the information as shown on the next slide.

14. .25
These settings represent the total depth of cut (.06) to go through the .55” material and .03 to be removed in a single pass. It will then require 2 passes to cut the entire way through the material. There will be two sets of green lines (contour cuts) shown on the diagram.

15. Repeat this exact same set of procedures to develop the NC data for the outside “slot” component of the drawing. All contour information will be the same as it was for the small hole (both the Tool Information” and the “Cut Control”) . When finished identifying the NC data for the 3 processes the drawing data will appear as shown below.

16. Once you have the NC process data in place, “Save” your file.
Exit from the Surfcam software.
Up until now you have been running the
the “demonstration mode”.
At this point you will need to insert the
“software key” so that you may continue your
work using the full capabilities of the software.
Open Surfcam again.
Open your file.
Go to the operations manager, right click on the NC project
And select “regenerate all”.

17. Next, select “Operations Manager” from the menu.
The “Operations Manager“ screen will appear.

18. The 1st process (the cutting of the letters)
The “Operations Manager” outline is set up to show the following items for this project:
The overall NC Project
The project Setup
The 1st process (the cutting of the letters)
The 2nd process (the cutting of the hole)
The 3rd process (the cutting of the slot) 1. 2. 3. 4. 5.

19. The material size data will now need to be entered.
Right click on “NC Project” in the “Operations Manager” outline.
In the sub-menu that appears select “Edit Setup Information”.

20. In the “Section Information” dialogue box select “Stock”.
“Corner 1” is the lower, front, left corner of the material.
“Corner 2” is the top, back, right corner of the material.
Enter the data shown to the right for this project.
Be sure to indicate the “Z” data for “Corner 1” as a negative number.
Once the data is entered, select “Add” and then “OK”.

21. Save the program at this point.
Select “Toolpath Verification” to inspect the program that has been created.

22. The “Toolpath Verification” screen will appear.
Move the “speed control” slider to the left (slow)and then select “Play” to verify the accuracy of your program. If it appears correct, exit the screen and save your program. If there are errors, see the instructor.
If the program is accurate, the material will be shown in blue. The letters will be shown in yellow indicating that the material has been cut into – but not all the way through. The hole and the slot will show through to the background indicating they have been cut all the way through.
Exit the “Toolpath Verification” screen and return to the “Operations Manager” .

23. Be sure “NC” code is highlighted (blue).
The next step will be to run the “Post” to create the G- code. Set the “axis type” and the “post” as shown below.
Be sure “NC” code is highlighted (blue).
Select “Post” and the contour data will be processed into NC code (G-code) .

24. The “editNC” screen will appear
The “editNC” screen will appear. The code for this program will need to be edited to add two items to make the program rum correctly on the milling machine.
Line N1 will need to be added to allow for the cutter to be lifted off of the material before the spindle is turned on.
Line N1 should read, ”G00 Z.25”.
At the end of the program, prior to the spindle being turned off, the cutter should be returned to the origin.
Enter a line of code that reads, “G00 X0 Y0”.
Save this program.

25. Open the .NCC file for your project in Velocity for an emulation prior to running the program on the milling machine.
Pay close attention to the up and down motion of the cutter to insure that the cutter is above the material surface during all G00 movements.
Inspect the code to be sure that all plunges of the cutter (G01 Z- motions) are listed with a feed rate of 5 IPM.
Inspect the code to be sure that all X & Y motions of the cutter (G01) are listed with a feed rate of 15 IPM.
Verify that the cutter is returned to the start point of the program, X=0, Y=0.
If all is fine, save the file and proceed to the milling machine to cut out your project piece. If not, make the necessary corrections.

26. At the CNC milling machine:
Insert the flash drive into the computer
open the “Velocity 4CNC” software
select “File”, “Open NC Code”
Select your file (NCC file extension)
Run an emulation
Verify that the toolpath is accurate
secure your material on the mill
Turn on the mill
Zero the cutter to the material
Zero the software
Cut the material.