Milling the Fusion 360 Reciprocating Saw DemoIn part one of our blog on milled surface finishes, we looked at some generic information regarding surface finishes. In this particular blog, we will look at the steps used to mill a scaled-down version of the Autodesk Fusion 360 reciprocating saw demonstration and training part.
Note that this is just one of several methods that can be used to mill the part. Other people will have their own preferences with their own logic behind those preferences. Feel free to share your own tricks and experiences in the comments section.
InspirationThe inspiration for this is the same part, milled full scale, by Titans of CNC to be used as a display piece by Autodesk at tradeshows. Titan's piece is fantastic, with a really good finish, but it also weighs about 60 pounds and is fairly difficult and expensive to ship to all the shows. (See Titan's YouTube video here)
Our goal was to mill a smaller version that could be used as a simpler and smaller showpiece. This was going to be milled on a Tormach PCNC 440, and was scaled down by half to fit into the work envelope of the PCNC 440. The question was whether we would be able to achieve a comparable surface finish to the Haas VF6 SS used by Titan.
Below is an image of Titan's part
RoughingWe utilized an Imco 3-Flute Streaker for the roughing. First a 1/2" diameter cutter (.52 DOC, .05WOC) to remove the bulk of the material, and a 1/4" diameter (.26 DOC, .04 WOC) for re-roughing or rest material roughing.
Here is a slideshow, showing the roughing and re-roughing operations. Full video was difficult as coolant and chips obscured the video capture.
When the 1/2" tool was finished it looked like the picture below. There is extra material leftover inside the pocket for the grip/handle, which needs to be removed by a smaller tool. Also, the stair steps are fairly large for the semi-finishing tools to be used, so it was our goal to smooth those out a little as well.
One can automatically re-rough the leftover material from previous operations.
If you use a second adaptive clearing operation, depending on your parameters and tolerances, you may get some undesired air movements. John Saunders from NYCCNC did a really good video on removing the "whisper cuts", but those tactics do not always work on 3D contoured parts, plus we did want to knock down the stair steps a little.
Alternatively, you run the adaptive clearing just inside the pocket, so that the full material there is cleared away, then run some other cutterpath everywhere else. In this case, a contour cut. The two cutterpaths together allow for a smoothing of the rough model.
The roughed out part, from the 1/2" and 1/4 inch is shown below.
Semi-Finish and Finish
Although there are many different finishing strategies which can be used, we chose to use a combination of a parallel cutterpath (planar finishing), along with the contour cutterpath (Z-Level finishing) utilizing a slope option. For more information on the differences in strategies, and what the benefits of this are, see Part One of the blog.
This strategy was used for both the finish and semi-finish. Only the stock allowance and stepovers would differ. With Semi-finishing we left 0.005" of material for a finish cut with a .020 stepover. With finishing, we cut to net zero, with a 0.005" stepover. The two cutterpaths work together to cove the part completely, without large cusps or scallops remaining.
After the semi-finish operation the part looked like below:
And during the actual finish process with the 3/8" ball
We used a 3/8" ball mill for most of the finishing, as it would deflect less than a 1/4 inch, and all of the radii of the part would still be milled. We used a 3/8" bull nose with a 0.015" corner radius for the bottom of the part to get a relatively sharp corner, yet still achieve a smooth finish.
Want to watch the semi-finish operation, check it out below. Sped up to save time.
During roughing operations, we had to pause four times to remove chips. Even so, many of the images during roughing show a lot of chips in the mill.
During finishing, we would check the runout in the tool and holder prior to milling. Using R20 collets, it is easy to have excessive runout if tightened too tight or put together incorrectly. We would check the runout and adjust the tool and holder until we could minimize runout, though we were never able to get it to zero.
We can say the part is not hand-polished, but it is polished, so we can share another tip on surface finish. I have a friend that made small molds for the badges placed on cars. He would set several up on his mill at one time, program all of the parts, hit cycle start and practice some golf. Afterwards, he would place a small polishing bit in, with some compound, program that, let the machine run while practicing more golf.
In this case, you can use Dremel polishing bits with a 1/8" shaft. Simply place some polishing compound on your part, and use the polishing bit in your mill with a 3D cutterpath like Scallop. Let it go while you practice a round of golf, or do other work around the shop. For this part, we used the large cylindrical bit, approximately 0.42" in diameter and a spindle speed of 9000 RPM.
Milling 3D contoured parts is quite different from milling prismatic parts. Excellent surface finishes are possible, with almost all mills, with careful programming and strategies.