Drilling holes through 1x2 tubing - advice needed

Team 4152 is working on improving their manufacturing capabilities. We are building a new drive train (you can follow our progress at https://mrmctavish.wordpress.com/category/robotics/st-drive-train-build-blog/ ). Our drivetrain will use 1x2 aluminum tubing that is 0.095" thick. We have a CNC router - our goal is to drill the holes on one side then turn the piece and do the other. Any tips or tricks to ensure we get a good result?
Here is one of the pieces.

Use a the shortest length drill you can, make sure your location is accurate when you flip it. You can probably don’t need to use a chip breaking cycle, make sure your feed per rev isn’t too low or high

Do you have a tube setup on your router? If not, you should probably get one. We made ours with three vises; I want to say each cost about $100 (though I could be wrong about that). It took about 6" off our work area, which was definitely a worthwhile tradeoff.

I highly recommend drilling and tapping two holes in the side of the static jaw and attaching a machining parallel spanning the gap between the jaws. That way to align the edge of the tube all you need to do is press it against the corner of the static jaw and parallel and close the vises. Then you can set offsets in your CNC router program to make it easy to make CAM for tubes.

You can also get a Tube Magic from OzzyBoards. I haven’t used it myself, but I’ve heard good things.

I’ll also add that it’s important your tube ends are square when using this setup, otherwise your top and bottom holes can end up misaligned. If you use the horizontal bandsaw setup you described in your blog post it should be fine. But you probably want to periodically re-square the bandsaw vise to keep everything properly aligned.

Edit: Also, if you find that your holes are coming out mis-aligned or mis-located you may want to use a pilot hole pass first before opening the holes up to final size. This will help make sure the larger drill bit doesn’t walk and the holes are properly located.

1 Like

For the drilling I would make sure to do the following things.
-Stubby drills: buy stubby drills that are set aside only for use on the router. As said above the stubby drills will help prevent the drill walking and thus make the holes more accurate.
-Use as much coolant as you can: This will both extend the life of the tooling and will make the holes come out better.
-Centerdrill: Center drill all the holes before hand, this like using stubby drills will help with accuracy.
-lower rpm: Figure put what the lowest rpm you can run the router at is while still maintaining a decent amount of torque. Drill bits, unless they are designed for it, really don’t like the very low feed per rev you get with a z-axis on a router.
-hearing protection: Wear hearing protection, I almost guarantee you the drill bits will scream when drilling until you find tune your feeds and speeds to minimize it.

2 Likes

Great information from everyone. Any suggestions on optimal feed rates and speeds?

I don’t remember any of the actual numbers exactly. That being said I believe we ran the spindle at 12k rpm and drilled by doing ~20thou pecs. I don’t remember the feedrates we used but I would start off slower like 10ipm and go up from there until you find a sweet spot. I’m guessing someone here will be able to give you better numbers than I.

The router we use is an omio x8-2200 btw.

  1. Use a drill, don’t do a bore

  2. Set up your tubes in a vice / a few vices

  3. Use an end stop to bump your tubes up against to locate it

With that setup, you can get tubes with holes within +/- .003", depending on how accurate your router is. On the CNC I use at work, we use this method and it’s +/- .0005"

Note: I don’t think you would need a spot drill. Just get a stubby drill bit and you’ll be good:
https://www.pts-tools.com/catalogue/product/287413
https://www.pts-tools.com/catalogue/product/287423

This.

And don’t reference off of an end with a questionable cut. Square reference ends up on a mill/router, or cut them with a well-dialed-in cold-cut saw.

1 Like

Investing in some quality drill bits is another thing to not overlook. Cheap HSS bits will dull out on you pretty fast with the High RPM the router spindle’s operate at. If you can swing it i’d recommended using carbide drill bits.

for example: https://www.mcmaster.com/2956a65

Having used this product I cannot support it and say that it is accurate… Conveinent sure… but the toggle clamps you are using rely on rubber end tips… which degrade and also allow for movement. If you are just buying the setup for drilling… sure. If you expect to drill and do pocketing or routing with it, I cant recommend it. The toggle clamps are cheap. Responses from the company are lackluster… I have been contacted multiple times to get replacements for the quality control on the toggle clamps only for the company to go silent after getting my info and never responding after. They seem keen to squash any bad reviews on CD but once its taken to a private channel no word after… I would suggest getting some small vises and clamps and setting it up on your router. It will be a much more robust and last you longer.

1 Like

I’ve actually heard that cheap uncoated HSS is the way to go. 4mm and 5mm split point drills are sub-$0.50 from China, and I’ll soon be trying some that were sent to me by another Omio user.
Shorter is definitely better, however. For drilling the 1" side you can sometimes go all the way through with certain short drills.

@bcampbell That’s concerning. We just got one. Haven’t tried it yet. I wonder if the clamps can be replaced with something more rigid.

Just saw that post sorry, the clamp wear is a known issue and there might be a solution on the horizon. I actually remove the rubber tips on the clamps on purpose to make it more rigid for milling, but they work fine for drilling and light milling.
@bcampbell I have some extra clamps I can send you. Emails about clamp replacements usually get redirected to me, seems like he forgot this time.

548 runs uncoated, cheap HSS “screw machine” drills from our local tooling store with mist coolant. We have never had to center drill before hand, but we are on a decently rigid Velox router and don’t drill any holes larger than F. For most drill bits, we just run them at 20kRPM (the max speed of the router spindle) and maybe 15-20ipm and only peck for stock thicker than 1/8". For F bits, we run them somewhere between 10 and 15kRPM. These speeds are definitely too high but we don’t have issues. We get good enough life from the drills and they don’t complain too much.

We are basically using the inertia of the spindle to do the drilling. Since we are drilling such shallow holes, the hole is drilled by the time the spindle bogs down too much from the load. Again, it isn’t great but it is rather fast. We are planning to upgrade to a VFD-driven spindle soon and will probably run it differently.

We hold the tube in a pair of toolmakers vises which back to a precisely-aligned rail so that we can move the vises around for longer or shorter tubes. Then we have a random bit of aluminum for an end stop that we also milled straight. Don’t buy the cheap Shars toolmakers vises. If you have the space, I would use real screw vises.

1 Like