CNC Programming of Robot Base Profile
Design of Robot Base for CNC machiningThe platform is to be cut from plastic (Polycarbonate 4.5mm thick) using a CNC mill. The design incorporates the motor mounts, location of the front wheel and clearance for the drive wheels. A suggested design is shown below. For more information see the webpage Robot CAD.
basic language for controlling a CNC machine is called G&M code.
While programs can be generated directly from 3D models and 2D
drawings, a knowledge of G&M code is helpful needed for analysing
or editing the programs. To start our first program, we need to know
only a handful of G&M codes.
G00 Move the axis at full speed (keep clear of the job!). In other words - "cutting air"
G01 Move the in a straight line (at controlled speed for machining).
G02 Circle Clockwise
G03 Circle Anti-Clockwise
G90 Absolute coordinates
G91 Incremental coordinates
M02 Spindle on CW
M05 Spindle off
M30 End of program
A typical line of code works like this;
G01 X50 Y100
which means: "Using a controlled speed, go in a straight line (from where you are right now) to the point (X50, Y100)".
Now let’s write a program; The centreline of the tool will follow the toolpath below. Coordinates are written with an X, Y or Z before them. Notice that coordinates that remain unchanged do not need to be written. F150 means a feedrate (movement) of 150mm per minute. S1000 means a spindle speed of 1000RPM. I & J are the coordinates of the centre of the circle. This program is written in absolute coordinates.
G00 X0.00 Y0.00
G01 Z0.00 F150
G03 X65.00 Y20.00 I65.00 J10.00
G01 X35.36 Y39.64
G03 X0.00 Y25.00 I20.71 J25.00
that we have not made allowance for the diameter of the tool, so the
actual part will be SMALLER than the toolpath (by ½ the tool diameter).
Before you begin to write the code, take the sketch of the platform and then offset the perimeter by ½ the tool diameter (The tool is 3mm diam, so offset by 1.5mm).
Dimension the drawing so that the bottom left hand corner is the datum point (0,0). You need to know all you dimensions as absolute coordinates. On the platform job, the datum point is the bottom left hand corner of the 191 x 146 mm BLANK. Set this up in SE draft, and make sure all you measurements are based on this point.
Rewrite the above program in incremental coordinates (G91). Write the code as a text file – using Notepad. Use 2 decimal places on all numbers. Display the font as Courier New or some other font that has equal spacing for each character (non-proportional font). Assume the tool begins at the first point (lower left hand corner) at a height of 10mm above the job.
Writing CNC codeGet the CNC Program above (ISEL or BOXFORD versions)
you start CNC programming, you have to convert your Solid Model
(Inventor *.ipt) into a toolpath (1.5mm offset around the drawing
because cutter is 3mm). See Inventor-to-AutoCad
rounded profile and inboard wheels was much more successful in the
maze - the rounded shape reduced the tendency to get caught. It is also
better to have inboard wheels so they cannot be snagged when going
around a corner. Actually, the general shape of a clothing iron seems
to be effective in reducing snagging (on corners) and helps to turn
parallel to the wall.
- Since the cutter is only 3mm diameter, this requires 2 cuts to penetrate the full 4.5mm depth of the polycarbonate.
- Use mirror command for symmetrical shapes. Use copy code to repeat code (e.g. When doing the 2nd cut).
that the blank must have 2 bolt holes drilled before mounting onto the
wooden backing board. The holes are diam 6.5mm and 100mm apart. The
datum point is at the front left of the machine.
- Once the CNC program is complete, save it to disk or memory stick ready for machining on the ISEL CNC machine. Make sure you save the file your file in *.tim format because this is the most reliable. The CNC machine uses the G&M code format.
See the Program settings for bolts positions at (100, 100) and (200, 100) and with an assumed height of 10mm.
Base blank size = 210 x 160 mm (Isel)
BLANK SETUP FOR BOXFORD CNC MACHINE