Using Surfcam to Produce a Numeric Control (NC) Program

Using Surfcam to Produce a
Numeric Control (NC) Program
Production of Wheel Blanks for the
Wooden Toy Project
An Introduction to the CAD/CAM Process
Instructions for 3 Axis Programming Using the
D&M CNC Milling Machine and Cyclone Router
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.
To produce the program for the wheel blanks for this
exercise you will need to follow these general procedures:
1. Create a 2d drawing using SolidWorks.
2. Draw the wheels with a diameter ¼”greater than the
wheel required (compensation for the bit diameter).
3. Include the material perimeter in the drawing keeping
any wheel circumference at least 1/8” from the
material perimeter and each other
4. Save the drawing as a .DXF file.
5. Save the .DXF file on a flash drive.
6. Open the file on a computer running the Surfcam
7. Follow the steps listed on the following pages.
Surfcam Instructions
Open Surfcam from the desktop on the laptop computer.
Insert the flash drive into the laptop.
Open the file that you need to have converted to G-code by selecting
the location, file and file type.
Be sure to have
“AutoCAD DXF Files(*DXF)
selected as “Files of type:”.
The following settings need to be made for
converting the 2d .DXF data to Surfcam data.
The converted DXF data will appear as shown below.
Select “Zoom Out” multiple times until the axis
orientation marker, the origin point and the drawing
data is shown on the screen together.
You will need to delete the extraneous data that has
been placed on the diagram.
To do this, select “Edit”, “Delete”, “Within” and use the cursor to
surround the excess lines/text. Select “Cancel” when finished.
The drawing data will now need to be attached to the program origin.
To move the drawing data, select; “Edit”, “Transform” & “Move”.
Next, select “Location”.
Then, select “Within”.
Click, drag and surround the drawing data.
Select “Sketch”, click on the lower left-hand corner of the
drawing data and then click directly on the origin point.
The drawing data will now be attached to the origin and
the diagram will need to be resized to fit the screen. To
do this select “Display” & “Fit”.
Points for indicating where holes are to be drilled will need to be located on the diagram.
To do this select “Create”, “Point” and “Center”.
Touch the cursor to each of the circles to produce the center points.
Select “Cancel” when finished.
To begin producing the tool paths:
Select NC 2-axis contour auto visible done
Center points in place.
The holes will need to be drilled first in the sequence of cuts that are to be made.
To program the drilling of the holes, select “NC”, “2-Axis” and “Drill”.
Have “Single “ highlighted and then touch off on each of the center points.
Select “Done” when the center points are highlighted.
The “Hole Processing“ dialogue box will appear.
Change “Coolant” to “Off”.
Select “Select Tool”.
Select “Drill” from the drill bit icons.
Scroll through the list and select the ¼” HSS drill (#151).
Select “OK”.
Select “Cycle Control” and set the “Hole Depth” to
Use .55” to drill all the way through .
Use .375” to drill ¾ of the way through the wheel blank.
Select “OK”.
The diagram will now show the “Tool Path” in green.
To see the depth of cut, select “View” and double
click on “Isometric view”.
The view can later be changed back to a top view by
selecting “View” and double clicking on “TOP view”.
The contour cutting of the wheel outline will now need to be completed.
Select “NC” from the menu and then, “2 Axis” and “Contour” .
Select “Single” and highlight each of the circles.
Select “Done” when the circles are highlighted.
Choose “Select Tool” and set the cutter as a 2-flute, 1/4” End Mill”.
Choose “Select Material” and set the material as “Mahogany”.
Set the “Feed Rate” at 50 and the “Plunge Rate” at 10.
Select “Cut Control”.
In the “Cut Control” dialogue box, set the “Amount to Remove” at .55”
Set the “Rough Spacing” to 0 and .2” . Select “OK” twice.
The contouring tool paths are now complete.
The next steps will produce the G-Code for the machine to run.
Once you have the NC process data in place,
“Save” your file to the flash drive.
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
And select “regenerate all”.
The “Operations Manager” should now appear as shown below.
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”.
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”.
Save the program at this point.
Select “Toolpath Verification” to inspect the program that has been created.
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.
Exit the “Toolpath Verification” screen and
return to the “Operations Manager” .
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) .
The “editNC” screen will appear. The code can be edited here, but we
will make any necessary changes in the “Velocity 4CNC” software.
Exit the screen and
select “Done”.
Save your file.
You can now exit
Your NC file should be
saved on the flash
drive with the name of
your original DXF file ,
but with an NCC file
extension .
You are now ready to
proceed to the mill to
cut the plastic.
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)
Open the code editor.
Insert a line of code at the start of the program
before the “M3” line that reads “G00 Z.3”
Insert a line of code at the end of the program
directly prior to the “M5” line that reads “G00 X0
Y0 Z.3”
Exit the code editor.
Run an emulation
Verify that the tool path is accurate
secure your material on the mill
Turn on the mill
Zero the cutter to the material
Zero the software
Cut the material.

similar documents