We use similar vises from LittleMachineShop.
Do yours have holes on the bottom? I’m unsure if the ones I linked have holes on the bottom. If not, how are you mounting yours?
Looks like they’re relying on the edges of button head screws to clamp the vices.
LittleMachineShop sells these mounts: https://littlemachineshop.com/products/product_view.php?ProductID=2675
EDIT: Tagging @Andrew_L since the reply didn’t go through.
Lets say you are about to machine a 1x2 tube. Measure its true extruded dimensions, lets say we get 1.002x2.010" for the outer dimensions. Now when you go to CAM for the 2 inch faces you need to set your work offset 0.005" from the 1" side face, which now perfectly matches what it will be like while you are machining the part in your fixture. This solution solves the axial concentricity shift issues. The reference pin solves the linear shift issues.
We use these. Can confirm they are simple and get the job done.
This makes perfect sense. Thanks for the clear explanation.
It’s an annoying step to have to take every time you run tube, but the results that you will get every time from this method speak for themselves. We actually added 2 rows of holes 0.25" apart that are at 0.50, 0.75, 1.00, 1.25, 1.50, and 1.75 on our jigs so that we have all the options covered.
In your post here you have a great picture of 1678’s tubing jig (with the machinist’s vises). Did you switch to a flat plate jig with a different kind of clamping system and then add the holes for dowel pins to that?
On a Velox platform, we’ve been able to put a 1/2" 2-flute endmil in our Porter Cable router head, spin it up to 21k, and cut both sides in a single setup (with lubricant) at about 60ipm to get concentric bores.
It definitely violates both SFM & feed per tooth rules but the bit rigidity gets us round holes at both depths and we haven’t seen problematic levels of cutter wear yet, with the same one bit for >2 seasons cutting twin [significantly underweight] WCD bots each year.
(In contrast, when trying to use 4mm bits, we’ve run into what appear to be bit rigidity problems trying to get a round hole? Plus definitely failing to maintain alignment when flipping tubes.)
The last time we tried (and failed) to flip tubes in process, I wasn’t measuring the as-extruded dimension and using work offsets, so that’s an important tip…
@RoboChair Have you found the dowel pin to cause any workholding issues with clamping force acting on the dowel instead of the fixture face (if the tube is undersized) or not fitting against the fixture face (if the tube is oversized)?
EDIT: Or is extrusion error just actually closer to 0.003" than 0.010" and then the 0.0015" gets absorbed by slip fits?
We still have the vise set up for running larger tubes like 2x2 on the Velox, but we are running 3 Tube Magics on one of our Omio routers and that is what has the hole pattern I described.
@sNeff 0.010" is a very big error in tube size and it is generally much smaller than that. When dealing with over or undersize tube you are only dealing with half of the error at any one time, so 0.010" would be a 0.005" error from centerline of the tube and much less of a problem from an indexing point of view.
Your suggestion of using a larger endmill is not a bad way to go about it either.
No, we use 4 bolt heads to hold it down on the the 2 lips on the sides.
I’ve been using a technique suggested on CD (can’t recall who) which involves using a 4x2. Was skeptical but it works well in my experience. Gist is: true the wide face of a 4x2 (flyover bit), screw the 4x2 to the OMIO deck reasonably aligned to Y axis. Use a flyover bit to cut a tube width slot into 4x2, 3/4" deep. Slot is now true to Y/Z. I make sure the fit is such that the tube slides in with just a bit of hand pressure. Hold tube down with “bridges” or screws. If you have an accurate 90 deg cut on the end of the 4x2 a stop can be mounted to get reasonable X positioning as you rotate between milling operations. Edge find to validate where needed.
For anyone that’s using an Omio and wants to use the auto probing capabilities in Mach3 to zero the machine, there’s a great video tutorial on YouTube here: https://www.youtube.com/watch?v=MQ9XT30s-PU
After playing around with his script, we discovered that it’s calling a command
GetVar(200x) that isn’t supported by the Omio controller. Replacing every
GetVar() call with
GetOemDRO(80x) seems to fix the issue. The scripts attached to this post have been modified to work with the Omio. Hope this helps!
We do this on our machine too, using a 1/2" mill, with the addition of a piece of 1/8" scrap Al sheet screwed in at the end to cut the X reference stop into, so that there’s a harder stop and we can get more uses out of the wood before it warps beyond usability.
Normally we have a tight enough fit that we can run drilling operations (bunch of 5/32 holes at 1/2" spacing) with just 2-4 wood screws with washers at the edges of the tube, and then run about 8x ~1.5-2" long wood screws through those to fixture for more aggressive milling operations afterwards.
Wood (red), scrap aluminum (grey) with screws (green), slot (blue) with “dumbell” shape to get a flat face for the tube stop
Can we get pictures of some of the jigs/fixtures that people are referencing?
So, in the end no matter what saw we cut the tube on we can’t seem to get the end of the tube perfectly square. So 180 flipping won’t work for us at this point. I do like the dowel pin idea, but I’m not sure how we would go about it yet.
Today we will have a 1/4" diameter end-mill with about an 1.5" cut length that we are going to try and run. https://www.amazon.com/gp/product/B007BTQ502/ref=ppx_yo_dt_b_asin_title_o00_s00?ie=UTF8&psc=1
We’ve been getting very good results cutting tube with an old miter saw and a “non-ferrous” metal blade. I very carefully adjusted the saw to give the cleanest cut possible, then locked every adjustment to keep people from messing with it. The saw gets us 95% of the way there, but a very quick brush with a carefully squared sander finishes the job. The blade wasn’t cheap, but the cuts are well worth it. The saw we’re using isn’t anything special either. It was in rough shape when we got it, but does extremely well after some rewiring, adjusting, and clean-up. Can’t argue with free!
So we were able to run some tube on our machine tonight with the longer end mill (1.5" cutter length) and were able to make some nice and easy through cuts that are right on size and are concentric as they should be. Yay progress.
John, any hints on feeds and speeds and toolpath type you’re having success with?