CNC FLIP-PART SETUP
composed by Mathieu Pung
PART I 3d Software
1. Bring your Model into Rhino, SolidWorks, Alias, etc! I do most of the setup in 3d software since the
machining software might change depending on which FabLab you are working in.
2. Pick all objects (I usually group them and center the pivot). Rotate* your part to be machined correctly. It
needs to lie on the XY plane.
*When rotating it helps to type in manually increments of 90 degrees.
3. With your pivot point in the center of your object(s), use Transform > move your part to the origin – just
type 0 if you have that mode. The flip part is not like single sided machining!
4. Let’s make the posts!! In side view, I use a Primitive Cube. Cubes are faster to machine over than
cylinders. Here I use 2 to 4 of them generally but you could use as few as 2 or as many as 100! Depends
on how much sanding you want to do afterwards. As a general rule, make them the same thickness as
the mill bit you are using. You want to place them at the line of tangency (not necessarily the center of your
object – here it is a little below center). Don’t worry about their length right now. Also, try to place them on
the flat spots on your model so it is easier for sanding later (This example doesn’t have any).
5. Create a plane at the origin. Scale the plane to encapsulate your part. This represents the area that will be
machined. I place a small sphere the size of the bit just for reference to make sure it will fit. Next, trim your
support bridges back to the edge of the plane (Image 2).
6. Move your plane down slightly past the tangency line since you will be machining with a ball end bit.
end. Place a cube that represents exactly your block in size (especially the thickness!) - make sure the
block will have about a 25mm frame around your machining plane. Center the block at the origin. Now,
move up or down your block to center your object.
8. Trim the top surface of your block with the machining plane. This step depends on your 3d software. This
is also how everything will look when it machines your part. Again, make sure the block has a 25mm frame
around your machining plane.
9. Export this as the ‘TOPSIDE’.STL. Our machining software uses STL files, but yours may use igs files.
NOW, for the SECOND SIDE.
10. Very Important**: Group all of your objects (including the surrounding box) as one. Place the pivot at the
origin.
11. Select the entire group and Rotate it 180 degrees around the Y axis.
12. Now, since you flipped it, you might have to Trim the top of the block again.
13. Move the plane down slightly past the line of tangency since you are using a ball end bit.
14. Export this as the ‘BOTTOMSIDE’.STL. Our machining software uses STL files, but yours may use igs
files.
CNC FLIP-PART SETUP (cont’d)
PART II Machining Software – this demo uses DeskProto 5.0
Regardless of your software, the steps and general strategy is similar.
15. File > Start Wizard. Choose 3d milling. Now, if everything looks ok with regards to scale, just hit next on
the next 2 steps.
16. When asked which part of the segment, “use whole geometry”. You may think to use just “half” but we
have already placed a plane which will limit the geometry being cut. In the next window, choose your
milling bit. Make sure it is long enough to make it halfway through your material!! Otherwise, the collet
will hit your material when machining.
17. You may hit “Calculate Toolpaths”, but do not write the NC file just yet. Just hit Finish.
18. There are several issues that we have to correct.
19. Look on the left toolbar and click “Part Parameters”.
20. On the Support tab, we don’t have to do anything since it has been done in 3d already. And again, just
leave it at “whole geometry” in the Segment tab.
21. Here are the important things to change!!!
a. On the Ambient Tab, click “Equal to top level of segment”.
b. On the Translation Tab, click “Make Centre of part Zero” for XY & “Make top of part zero” in Z.
22. You should have this. Notice the machining doesn’t try to go outside and down the frame. Also, the origin
has moved to top center.
23. Now, look on the left toolbar and click “Operation Parameters”.
24. Click the “Segment” Tab, and click on “Custom Rectangular” and “Set Graphically.”
You’ll have to click on the wireframe icon to be able to see anything.
Then, you’ll click on the marquee tool to draw a rectangle that sits inside your frame as shown below. This will prevent the software from machining the border frame.
25. Click the “Borders” Tab, and click on “Cutter Stays within segment” – this way it stays within the framed
border.
26. You should now have this. Notice the toolpath stays inside the frame border.
27. You’re done with the first side! Go to Create > Write NC – Program File and save it out as TOPSIDE
28. NOW, GO BACK TO STEP 15 and rerun the wizard (** Don’t try to rotate your geometry in the machining
program). When finished, save out your file as BOTTOMSIDE.
CNC FLIP-PART SETUP (cont’d)
PART III Machining Setup
You’re ready to get machining!
29. Place your material down on a substrate of mdf or something similar. Make sure the table surface is flat
and secure. I usually use a dab of wood glue the size of a fingernail on each corner of the block. Do not
rely on double-stick tape.
30. Take a ruler and a pencil and draw an “x”on the top center of your block. Zero the xyz at the top center of
your block.
31. Machine the first side using the TOPSIDE NC FILE. **Important: The very first pass will be very difficult
on the bit as it will plunge all the way down. Be quick, and SLOW DOWN THE FEED RATE to about
25% before it starts cutting. You may resume to 100% when the first pass is complete.
32. Now, using the Spindle on button and jogging the bit, Plunge 2 holes (about 2-3 cm deep) in the frame of
your material. You do not have to go all the way through the material.
Put those holes at a simple xy coordinate. For instance, here they are at x = 0, y = 125mm,
and x = 0, y = -125mm.
33. Now, wedge a paint scraper into each corner and a hammer out the glue. This should be fairly easy if
done right. Move your part to side (without forgetting its orientation).
34. This is the essential step. You need to repeat step 32, but this time, do it directly into the substrate on the
cnc machine. Do not machine into the aluminum!!!
35. Cut and place two wooden dowels (that are the same diameter as your drill bit) into the holes on the
table. (Here I used old drill bits since I didn’t have wooden dowels).
36. Use a dab of wood glue the size of a fingernail on each corner of the other side of the block. Flip your
block over 180 degrees around the Y-axis of the table and line it up using the dowels as a guide. Push it
snugly on the cnc table while the glue dries.
37. Machine the bottom side using the BOTTOMSIDE NC FILE. **Important: The very first pass will be very
difficult on the bit as it will plunge all the way down. Be quick, and SLOW DOWN THE FEED RATE to
about 25% before it starts cutting. You may resume to 100% when the first pass is complete.
38. That’s it. Now, wedge a paint scraper into each corner and a hammer out the glue. Use a hand saw to
cut the supports, take the part out, and start sanding!!
Download the tutorial as pdf file: