One of the most useful tools to have around is the ability to broach your own gears and pulley. We lost the ability to do broaching at our local shop so we decided to invest into a rotary tool for our CNC Bridgeport.
Most people hasn’t seen one before so I threw together a video of us testing ours out. We got ours from Polygon Solutions, who were quite friendly helping us out and answering questions as well as giving us a small edu discount.
Let me know if you have any questions!
We have one from Slater tools. Pretty pricey, but it works well.
I made my own on a Bridgeport in 2015. Fairly easy to make if you have a lathe and mill, and tricky but possible to make on just a lathe or mill. Broaches 3/8" hex fine in aluminum but I haven’t bought a 1/2" broach yet. You can find holders on Ebay for $200-500 depending on the source (not China). They work great for FRC and are a lot faster than regular broaches, not to mention cheaper (apart from the holder cost).
I’m considering making a much larger holder and broach for a cycloid gear project. Make sure that you use ball or roller bearing if you make your own; I did not have much luck using a plain bearing for mine and had to remake part of it.
Do you have a source of drawings for a make your own? We have a hex broach, but I keep it at work rather than the shop because that is where the press is.
Fascinating. I can easily imagine fabricating what looks like a rotary hex broach from steel, but wonder if it needs to be hardened?
CAD and drawings available here: https://drive.google.com/file/d/17DqaOrdD7BHjIMFXGhzZHs2h5HZPBdtN/view?usp=sharing
Accepts all standard 1.75" long 1/2" shank broaches. Put a 1.75" ground rod into the sleeve and use the set screws to adjust it on-center.
I made a 3/8" hex rotary broach out of A2 tool steel but needed to go to the community college nearby to harden it. They never got back to me on that, actually… presumably it’s still sitting in some corner.
We’re considering a rotary broach for our shop. We’re not sure what’s the best tool to use though. We could program our Tormach, as you have done with your Bridgeport, but the broach manufacturer suggests it will need ~650 lbf of axial force to push through which I gather is pushing the limits of the Tormach’s Z axis. http://www.slatertools.com/customer-support-service/technical-assistance-/thrust-lbs-for-broaching-information
We could also use our manual 12" lathe, but I really don’t know what kind of axial force the tail stock or the feed screw can apply. Does anyone have any experience with rotary broaching on a manual lathe?
I believe tormach sells a rotary broach as part of there TTS system, so you could give them a call and see about that. NYCNC did a review of it on there youtube channel.
12inch seems a bit small but it might be okay for alumium, I use a 16x40 lathe that’s a monster that can easily handle it.
What is this black magic?
I read they also call it a ‘wobble’ broach, but watching it looks just like a normal broaching operation where you shove it through a hole. Can anyone explain the dynamics a little better? The videos and tutorials on line just kind of breeze over how the cut is made.
The broach bore is not coaxial with the spindle (It’s 1.75* off, IIRC) and it is also on a bearing such that when the spinning tool (in the case of a mill) makes contact with the part the tool itself appears to stop spinning.
Essentially that creates a wobbling action when it comes into contact with the workpiece which is proportional to the speed of your spindle. One corner at a time is cutting and it oscillates from corner to corner, as opposed to a normal broaching operation where all 6 corners are cutting simultaneously.
The downsides of rotary broaching arethat you’re very limited on broach length (about 1.5xD typically) and because of the oscillation the form tends to “spiral” as it goes through the part. You can sort of counteract this by stopping halfway through and reversing spindle direction, but it’s just inherent to rotary broaching. You also really can’t broach a full form hex as the tool needs an ID larger than the nominal hex size, but that’s fine for FRC purposes.
Perhaps the biggest downside is that you cannot clock your hexes without a separate attachment that clamps onto the body of the toolholder that has a dingus which pushes up against a stop on your spindle/table to keep the same orientation of the flats from part to part.
While it’s very cool I’m a little unsure of the utility of rotary broaching for FRC. If I need to CNC a whole bunch of hexes I just mill them with drilled dogboned corners. A pretty quick and easy process especially if you use a a 1/2" drill to remove the bulk of the material before milling. If your planning on using thunderhex then there’s no need to dogbone if using a 1/8" or smaller endmill.
Besides perfectly sharp corners what advantage does this have?
It takes 5 seconds to rotary broach a hex. Way faster than drilling corners or using a 1/8" end mill.
So the problem with using a birdgeport as “a huge press” is that you will ruin the bearings on the spindle, these rotary broach holders lets you spin up the spindle while the borach is “freefloating” so when the touch the material they don’t spin.
This lets you apply force with the broach without damaging the machine.
If it works on the lathe, it looks like something that could be easily used with only a little training. That makes it attractive against the alternative of an expensive fragile linear broach (and a new 3T press with enough stroke to fit it), or programming a CNC path with tiny end mills. It’s also extensible to other broaching features, like versaplanetary splines perhaps.
I haven’t used one of these, but it looks like a rotary broach doesn’t need a through-bore? E.G. you can rotary broach a blind hole to partial depth, whereas a standard press broach requires a complete pass-through.
That would be a big advantage in situations that require it.
Not exactly.
It pushes the chips ahead of the tool. So you can do a blind bore but you cannot do it up to a shoulder, you need some relief behind it for the chips to flow into (which you alluded to, just want to be very clear for those who aren’t totally sure how the process works).
I tired it on our bigger lathe and it worked fine. That’s why we ended up going down this road, it was buy a huge press or this. This took up a lot less space and costed about the same if not less.
This video certainly didn’t make it look all that fast. They used three ops before they could start broaching. While I’m sure that in a production enviroment rotary broaching would be faster. For FRC purposes the costs involved seem rather high. Cutting time shouldn’t really be a big factor for an FRC team anyway as setup and CAM will make up the majority of the work 90% of the time.
On the other hand milling a Thunderhex compatible hex would just be:
That could be done pretty fast in aluminium especially if your machine has a reasonably high spindle RPM. It’s also trivial to adjust the fit of your hex, something which comes in handy when Vex’s inventory is oversized.
For us it’s way faster (and higher quality) to rotary broach than it would be to mill. Especially for anything thicker than 1/2" which is typically the LOC for a 1/8" end mill. The only point in milling’s favor is adjusting the hex size, which we do via a nominal and oversize rotary hex.
Well if your item isn’t already to size, you still have to drill (or mill it out, I could have drilled it but I like milling bores) and a chamfer. So it’s not really any slower… i could have probably push the broach through faster but wanted to start slow.