Our team just started back with our regular fall meetings and one of our current tasks we want to accomplish is running some drivetrain rails on our OMIO CNC. We purchased a tube-magic clamp setup to help us with this, but I wanted to know if anyone had tips on setting up the machine. I’m very familiar with setup for running flat parts out of sheet, but it has been several years since I did any mill work. I’m using Autodesk Fusion 360 for the CAM setup.
My previous milling experience had me zero off on parts using an edge-finder on one end of the stock material for X, Y and then zeroing off on the top of the part for Z. Would this not place my origin point -2mm X, -2mm Y off of the part corner if say I was using a 4mm cutter? How do I set the origin in the CAM properly?
Am I completely off-track about this? I’ve looked around for videos to see if I can learn from someone else’s process, but I’ve had no luck finding anything.
You have to change your offsets after you edge-find by the radius of the edge finder (unless you have a haimer or something similar).
Typically there are two ways to do this:
Move your x and y axis the radius of your edge-finder until you are centered over the corner of the part and then re-zero or
Manually enter in the offset (edge-finder radius) into your machine to change the zero position ensuring the right sign.
To check you have it in the right place clear the tool in the Z axis (G0 Z4) and then command the machine to travel to your origin (G0 X0 Y0). You can then jog the tool down to see if it’s central axis is above the corner of the part.
If you touch off on z using a piece of paper or a shim, its the same process to account for the thickness of the shim as it is for the radius of the edge-finder. This is an excellent video that explains the process, and if you have the time the rest of Haas’s videos are fantastic as well.
Edgefinding works ok, but I’ve actually had better results putting a 4mm endmill in, eyeballing the xy zero, drilling a hole, measuring the hole location, and adjusting appropriately. Takes less time than edgefinding and is a lot harder to kill tools. Scrap 2x1 is easy to come by as well.
Another question… when running bearing holes in the side of 1x2 tube… Is it better to run one side then flip the tube? If you can square of the end properly… or do folks run 1 operation to cut the holes through both sides most of the time?
1 cut through is ideal but can be unrealistic. 3/8" endmill reportedly can work, albeit with chatter. Flipping the tube can work if you’re very careful to edgefind accurately, but I screwed up several drive rails this year doing that. 3/8" endmills are in the mail.
The ideal situation would be to go through both sides in one setup, both to save time and to retain concentricity, but sometimes the tooling required isn’t available, or the rather small and/or not very rigid routers most teams have are the limiting factor. I would guess the minimum to make this happen without too much chatter and flexing of the tool would be a 3/8" endmill. A larger diameter would be better, but most relevant routers can’t reasonably hold a tool of that diameter safely anyway.
This is an application where end-stops can be absolutely fantastic:
The intention of these is to create a repeatable X (or Y) axis stop to prevent the need for indicating during each setup. We used almost identical setups with ±0.0005 repeatability for reference standards and aeronautical components at a few of my previous jobs. They save countless hours of setup time over the years because once you do the setup once you know when you run the next part against the stops it will be in (almost) the exact same place.
Here is the process I have used in the past with various parts, both for work and robotics, that works very well:
Mill flat the ends of the tubing you intend to use to size
Place the stock in the fixture (vice/tubemagic/whatever) up against the end stop
Indicate your part on the edges that are against the end-stops (typically back left corner)
Run your first setup operations on the first side. We usually run this as one program, separate from the other, but you can simply put an op-stop in the program and tell the operator to flip the part
Flip the part and run your second setup operations on the second side.
IMPORTANT: The axis you flip the part about is CRITICAL and completely dependent on how it was CAMmed. If you are rotating the part about the X axis, in CAM you need to set the origin of each setup in the correct location. I made a quick example below.
We were flipping our tube the way Cyberphil mentions… the issue we discovered afterwards was that the end of the tube that we had lined up with the end stop was not perfectly square. Thus the holes ended up non-concentric. We don’t have any manual mills to do a flat milling process on the end of the tube… if we did this problem wouldn’t have happened.
I’m not sure if any of our router end-mills are long enough to do a through cut all the way through both sides of the tube in one operation. The cutter and the shank are the same diameter on all of the end-mills we use so maybe we can make something work. I’m not sure yet.
If you’re struggling to get square cuts I do suggest getting a metal blade for a chop or miter saw. While we generally mill our stock square and to size, I have worked with teams who use a standard chop saw and get really reasonable square and parallel cuts that minimize this effect.
Okay, what you need to do then is drill a hole or more into your tube jig sized for a 0.191 hole. You then drill an extra hole in your part or make sure the one in your jig will line up with the ones in your part. Do your top face operation, then remove the part, place a dowel pin into the jig hole, flip your part onto the dowel pin, and now you have a precisely indexed part without the need for a square end. Pro-tip this is how 1678 machines anything longer than about 30 inches, we can then move the part down and perfectly index to within a few thou.
before you start, flip the tube 90 degrees, mill the corner end off about .250" deep or so. now you have a squared off corner going the whole depth you can zero off of. and make sure the work center offset is changed to the same corner after you flip it.
also double check your tram at the far end if youre going to flip the material.
but if its only a 1x2 tube, i’d find some end mills that can cut 1" down in one setup. a 1/4" dia end mill or even 5mm end mills long enough should be easy enough to find and not chatter.
We currently use Tubemagic, and while we do love it, our setup commonly results in misalignment for the different tube faces (entirely our fault, but it seems to happen really easily).
I’m considering switching our tubing fixture to a couple of these low profile vises so that we can put the tube on some parallels and machine through the 2" face in a single run, and hopefully figure out a combination of end-stop + better tube squaring pre-machining to prevent the misalignment issue.
Not sure if I’m expressing this question clearly, but how does this interact with the jig setup when the stock is not quite the right size? Or do you reference off the same physical side of the stock regardless of its orientation in the jig?