Looking for insight milling tubing

[Dalego]

Hey all,

I have a 3 x 5 tube that we will be milling. I want to use our 3/4 5 flute end mill in one pass. Depth of cut would be 3.125" for the one pass ( or less but for now this would be suffice). I want to make sure the feed is correct when it hits the full 3". Perhaps I would want to do this in passes? Typically this would be done on a robotic laser/plas but we do not have that just yet. I am not even sure if the way I want to do this would be good for the tooling. I have attached a snap shot of the model so there is a better understanding here (hope it worked). What would you guys recommend doing on this part? I am not sure if 200 SFM would be to much.

 

[memphisjed]

A tube? Torch and grinder. 10 tubes, torch and grinder or porta-band if you do not have a profile saw. 20 tubes, sub to tube laser shop maybe. 2000 tubes, get a tube plasma, 20000 tubes a laser down payment.
You have a mill, not every job is a nail.

 

[Dalego]

I agree with all that. We have a very very picky client so the cut and grind method does not work for them. Customer drives quality. Subbing out adds cost so again the customer we have would not like that either. I am in a position that leads me here asking for advice. Either way this will end up being milled. Trial and error until success. Just seeing if others out there may have some insight on what works and what won't work.

 

[dandrummerman21]

The areas where you transition from 3" deep cut to ~1/4" deep cut are going to be hell on your carbide endmill.

I've milled 2x3 tubing to length before, and that stuff will sing and not be happy, and probably chip your rather expensive carbide endmills.


Now, they aren't a ton cheaper if you need to buy them new, but my suggestion is to use cobalt/hss corncob roughers, think 1" or 1-1/4".

I might also be inclined to finish it with HSS/CO as well. But we have a whole big lista cabinet with 3/4" - 2" hss endmills for crappy jobs like that.


Pro tip: you can find rather large and nice roughing endmills on ebay for much much cheaper than buying new.


If you're running on a machine with not enough torque for a 1.25" endmill, I might still suggest you can get away with it if you only cut halfway down per pass, or take 2 radial cuts.



Another suggestions regarding the laser, even though you shot it down. I would at least try to get a quote for it. A decent laser shop would make quick work and it shouldn't be ugly. the amount of time to laser that off would be way less than milling, in my opinion.

 

[csteen]

Many years ago we cut some tubing similar size around a .08 wall thickness 45's on the ends that got welded together. We ended up using HSS Fine Pitch roughing endmills to keep it from grabbing the edge of the tube and just folding it in. The job ran really well and some members of this group may have even had machines with the final product on them as they were door frames for the large machine tool builder in southern California. We machined them for a large sheet metal shop in Lancaster. Just cut it but keep in mind a normal endmill may want to grab the edges.

 

[Dalego]

I was wondering about the cutter grabbing edges so I am glad that was spoken on. Thanks. We are in the middle of no where so going to another shop to have them laser cut is at least a 50 mile (100 round trip) venture. We do have a robot laser but it is not set up for this long of a part....yet. I like the idea of using a rougher cheap end mill and have been digging in my box of junk to see what else I can conjure up. Thanks all!

 

[dandrummerman21]

On reflection, another option you would consider would be using a small tool, like a 3/8 or 1/2" and do some flipping.


cut the ramp shape and end, flip 180 to cut the other ramp shape and end. Flip 90 and hit it with a 45 degree endmill (or whatever angle that is), and flip 180 once more to finish the end to length.

I don't think you mentioned quantity. For just a few, to a few dozen, this would be the way to go, assuming you have the means of having a decent stop on the other end of the part so your profiles match within a few thou. And small tools are cheaper.

 

[Jashley73]

QUANTITY?

The most important detail, and it's the one that everyone always fails to mention.

If I were doing it? Low-ish quantites? Saw first. Mill 2nd. Use a small diameter endmill - 3/8" max.

Tubing sucks, and it will flat beat up a large diameter cutter. You don't want to go near a piece of tubing with a large diameter cutter, at full length of cut. Screw that. Think of any other way but that.

 

[trochoidalpath]

Can you flip it against a stop or put it on a fourth? That would save you the unpleasant depth of cut problem.

 

[Booze Daily]

Kinda hard to visualize from that pic. Is it even to scale?

 

[Jashley73]

Now I'm thinking about it, hold it upright just as pictured, and turn it all into chips. Take a 1/4" endmill in a slim end-mill holder, start in the outside middle of the top, slot in, then mill outward until the "top" is gone. Then mill down the legs & angle, and finish.

Trying to cut any part of that away as a solid drop/waste is going to mean that there's even greater risk of breaking an endmill now, on top of the threat that steel tubing generally foists upon carbide endmills.

I still stand by my statement though, that a long, large-diameter endmill belongs nowhere near this part.

 

[BugRobotics]

Do it like Jashley73 is saying.

Saw most of it within an 1/8" or less and then grab a bull nose 3/4 or 1/2 or 3/8 endmill and surface with it upright to get that smaller radii in one shot. Low load on the cutter. No need for a long stick out.

 

[13engines]

I'm with Jashley and Bugs... Make a tin or stiff paper pattern that you could cup over the tube and draw out the shape quickly. Freehand vertical bandsaw it close as you dare, then do the bullnose interpolation thingy starting on the inside edge and continue nonstop all the way up and around. Could even pull off an edge break/chamfer with the same tool.

I'd do this up to about hmmm... 50 -100 parts maybe. That is if they were paying me enough. Any more then that I'd want to think harder about it.

On the other hand. If it were sawed close, a single pass with the aforementioned fine tooth 3/4-1" CO-HSS rougher might do the trick too. I suppose the inside corner radius might have something to say about that tool choice.

 

[Jashley73]

I'm with Jashley and Bugs... Make a tin or stiff paper pattern that you could cup over the tube and draw out the shape quickly. Freehand vertical bandsaw it close as you dare, then do the bullnose interpolation thingy starting on the inside edge and continue nonstop all the way up and around. Could even pull off an edge break/chamfer with the same tool.

I'd do this up to about hmmm... 50 -100 parts maybe. That is if they were paying me enough. Any more then that I'd want to think harder about it.

On the other hand. If it were sawed close, a single pass with the aforementioned fine tooth 3/4-1" CO-HSS rougher might do the trick too. I suppose the inside corner radius might have something to say about that tool choice.

Now that I've had more time to think about it, I wouldn't even bother with a saw...

Hand-feed on a vertical bandsaw? Maybe for (2) pieces. 3+ --- Screw that... Throw it in a vise, and let the VMC turn it all into chips while I flip through a car magazine.

Less risk, less handling.

Oh, and machine it dry, because few things suck worse than cleaning wet chips from the inside of a long tube...

 

[Dalego]

I love this group. We do these parts per order so it could be anywhere from 2 - 50 tubes depending on the week. Currently its just 2 for this week and they do not come through each week. I have discussed some other options with the rest of the guys as well. Even turning the entire corner into chips, or cutting out the majority with a hand plasma and milling the remains to clean it up. Until we do get our robot up to par milling is needed for "fitment" with other parts in the unit for welding. I am not used to ever having to mill out tubing so I truly appreciate all the insight on this. Thanks again to all.

 

[DDoug]

Can you make up some templates for a hand plasma to get rid of most of the material ? (much like the bandsaw method posted up above only faster)

 

[drewboyer]

I used to mill a lot of tubing parts. I set up a stop to catch the bottom corner and used 2 offsets. 1st offset cut the angle and finish one end facing Y+, M0 flip it 180 push against the stop with the finished end and use the second offset and cut the angle but now on the Y- side. Done. If it's just mild steel you could run at 350 sfm with .0025 chip load on a 1/2 end mill for the roughing pass, then 450 and .005 load for the finish pass, each op should be about 2 or 3 minutes, 6 minutes a part.

 

[ManualEd]

Dumb question, but why not a 3/4 or 1" HSS corncob mill to take it all in one shot?

They eliminate nearly all vibration from the tubing, and you can walk those suckers through nearly anything at a full depth of cut.

I've done a similar cut in an old BP with a 1" corncob with no problems.

It would probably be faster than farting around with low carbide speeds trying to not blow up a $300 cutter.

 

[Dalego]

Can you make up some templates for a hand plasma to get rid of most of the material ? (much like the bandsaw method posted up above only faster)

After going over the process with the rest of the shop this is the way we feel will work best until we get the robot ready (unknown ETA on that) Good talk and some great advice.

 

[Jashley73]

Dumb question, but why not a 3/4 or 1" HSS corncob mill to take it all in one shot?

They eliminate nearly all vibration from the tubing, and you can walk those suckers through nearly anything at a full depth of cut.

I've done a similar cut in an old BP with a 1" corncob with no problems.

It would probably be faster than farting around with low carbide speeds trying to not blow up a $300 cutter.

Have you actually tried this, with a 1" corn-cob rougher, on tubing? I have, and it sucks.