CNC WIP - small flipper.

BossDog & Owner
I have been using a shop vac during the cutting. I stick my head in the side window and vac up the dust as it is cutting. If I end up making a production run of composite scales I'll have to figure out how to get a vac hose in place and leave it on during the run. After doing this a few times, I think a decent CNC router with tool changer and dust control would be a better way to go for scales in any kind of volume.

BossDog you’ve probably thought of this already but when I worked in a machine that cut lots of carbon fiber, they had it set up with a really powerful shopvac that sucked most of everything out and they just ran it dry with no coolant.

BossDog & Owner

So getting this bevel modeled into the blade profile should be easy.
It took three days and dialing a friend to get it figured out.

It went like this:
model up the profile (easy)
make a swept cut for the bevel (harder)
notice that the bevel edge is not even. (huh?)
watch videos ( there are ZERO videos about this using solidworks)
try this, try that, wave a chicken foot over your head,
go home and try again tomorrow.
(tomorrow) find anything else to do in the shop other than sit at the computer again
(next day) beat yourself bloody trying multiple sweeps, get some to work but the dang edge thickness is still all over.
(next next day) call your buddy Travis who eats this stuff for a living, he tells me a different approach and a couple hours later it's done.

For the record if this makes sense to you.

I had been creating a plane on the tip and sweeping back using a profile line and fully defined V shaped cutter. This gives a bevel on both sides but has uneven edge thickness. Try to keep tweaking and walking it in. It's madness.

Travis's suggestion:
Create a perpendicular plane at the plunge, create a center of blade plane, than create an offset plane from the center (this will determine edge thickness - offset .01" gives you a .020" thick edge) sweep cut one side using the offset plane profile, mirror the feature.
Seems like it would work but I couldn't get the mirror feature to properly duplicate it.
I finally noticed some vestigal zero thickness geometry left over the sweep cut. I thought it would be ignored, it wasn't.
I redid the sweep cut by using an offset profile line that eliminated the dangling geometry.
Boom, mirror function now works perfectly.

It's insane how one stupid little thing can really eat up time.
I should be able to take a picture with my phone, text it to the CNC controller, throw the material into the CNC, hit green and walk away.
sweep cut.jpg

BossDog & Owner
managed to make a fixture for the blades.
It's 1" aluminum. Something I have lot's of end cuts of. Once I get this project all proofed out and developed, I'll switch the fixtures out to 1" steel.
Anyway, this fixture will hold two blades and allow me to mill the bevels, arc slot and pivot hole in hopefully a fairly rigid set up. I have my doubts. I think the hold down screws will need some help with bumper pins to keep things aligned.

The large hole is used for touching off with the wireless probe to set G54 X and Y. I'll touch off on the stock for Z.

I have two sample blades laying on the fixture to kind of show where these will be positioned. Next I have to mill some more sample blades out of 1/8" aluminum stock with the tabs in place. After I get a few of those I can start working on tool paths to mill the bevels in along with the rest of the features.

The Solidworks pic on the right shows the blade with the tabs in place and the cut sweep for the bevels.

The work flow right now requires me to mill out the blades blanks in a separate op and then move to this fixture. At some point I'll work on combining those two ops into one. I'll need to work on nesting several copies on one fixture first and that can wait. For now if I work on two parts that gives me access to both sides, I can easily scale up from there.

as always, any feedback or advice is appreciated. This thread is not a tutorial. I would have to know what I am doing for that.

IMG_3385.jpg sweep cut.jpg

BossDog & Owner
good progress today.

I milled out some extra blade blanks from aluminum and they fit perfectly in the indexed fixture.
Tomorrow I'll work on making some bevels in the blades. I think the aluminum is going to chatter and move around quite a bit, even with the 3 point hold downs. I'll run some in aluminum and then try some mild steel to proof the speeds and feeds.
IMG_3391.jpg IMG_3386.jpg


Well-Known Member
I know zilch about this kind of stuff, but with your ambition to learn how to do this and the stage your at it certainly looks like your going to be putting out some fine blades soon Boss, good luck.
I had somewhat of a hard time just comprehending what you wrote, but reading thru the lines, it seems you'll get this. :D

BossDog & Owner
I made a test pass yesterday on one bevel on one blade to see how the roughing tool path was working. It wasn't.
The depth of cut at the edge is too shallow. In other words, the edge thickness would end up around .050" thick. I want .020" on the edge. This had me stumped for a bit and I had to think it through.

I went back and made some changes to the roughing pass by extending the containment boundary. This added another .010" to the depth but it is still not deep enough. but the finishing pass cleans that up and gets it where I want....I think.

I'll cut another part today and see how that comes out.

This is an aluminum test blade using a 3/16" ball cutter.


Below is the verify feature of Mastercam. It is animated and shows how your finished part should look. Looking at the tips of the blades you can see where the ball cutter drops off the edge. I had to set Z limits to avoid the cutter from plunging past the blade thickness into the fixture. The pink material represents the metal. Really, there is only metal for the blades and it is not a flat sheet as you see it here. I'm sure I could model it so that didn't look like a flat sheet but there is a benefit to showing it this way. Now I can see the plunge at the blade tips and make sure I'm not taking too much or slamming down into the fixture.

In Mastercam you preview the tool paths (blue lines) and make decisions on how the tool is going to move. I am using a different roughing tool path for the top blade so I can see the difference on how they cut. My worry is the finish pass will end up taking too big of cuts in some places so I will have to see if and where that happens.

BossDog & Owner
Today was a good day.

I ran a few test passes (one side) tweaking the tool path on the bevel for a decent finish. I changed the toolpath for the V(ersion)3 test to waterline for the finish passes. I also ran both blades, flipped them in the fixture and did it on the other side. This gives me at least some idea on how to run parts on both sides so they index properly which was the most important part of the day for me.

I wish I was faster at this. If I had to depend on this to make money and feed my family, I'd be divorced and starving.

Looking good sir! What’s the stepover or scallop height your using for your roughing and finishing passes? It’s been so long since I’ve done any programming or setup on a CNC that I’m not even sure if I’m using the correct terms.... Anyway, not critiquing, just curious.

I wish we used MasterCam at work. That’s what I learned on in college but they use a super old version of Surfcam on an ancient computer that still posts the code on floppy discs lol. Thankfully I haven’t had to do much CNC at work cause I’m the “manual” guy now but I’m not sure I’d wanna do anything on our dinosaur software after using MasterCam and seeing how powerful it is.

BossDog & Owner
Step over is .0015” using a 3/16" ball mill.

Floppy discs. That is old.

I've heard of several old copies of surfcam still being used. Mostly from guys attending Mastercam training classes. You could hear them gasp at what MC could do compared to their old software. They couldn't wait to switch.

BossDog & Owner
Not a lot of machine time today.

I did spend a little time on the blade fixture.
I drilled and reamed the pivot hole, milled in stop pin arc slot and then profiled all around the blade profile.
Tomorrow I'll mill .005" to .010" off the top to remove the burrs sticking up from this process.

The reason for these relief areas is to give chips a place to go and also to minimize burrs from bumps, handling, etc in the fixture that can really create some tolerance issues.

I used a dremel vibe tool to mark the fixture plate originally. I'll have to start putting some milled engraving fixture ID names/numbers in the future.
Making the fixtures is almost more work than making the parts.