We just bought a tube laser, I'll have to model tubes to be cut and bend by hand. I saw a few methods to do that but I need the fastest way to do that.
"Best" & "Fastest"? You don't ask for much.
The attached file is what I've come up with. You have to understand that SolidWorks doesn't do tube bending so I had to get creative. I used Surface Offset, Thicken, and Combine features to get the copes to look like they would on an actual lasered part. Not the most commonly used features. Your situation may or may not need you to do this portion of it. I also have it set up so it give the appearance of unfolding (see the configurations). It uses the Move Face feature as a way to add bend allowance in - that has to be calculated manually. In some cases the Move Bodies feature may twist(rotate) the bodies (rare). In those cases I add little orientation notches before moving the bodies so I have something to align after the move again. I wouldn't worry too much about that though - as I said, it's rare. Anyway, I think this is the best/most accurate way. I don't know if I'd call it fast.
Good luck. I hope this helps you.
That's really nice Lee Wondra - I like it!
- My "quick & dirty" method is usually to model it as a sweep, delete most of the faces, and finish with a surface thicken - a lot of times our tube laser parts get dumped out as a parasolid or iges, and it works fairly well.
(I could do it start to finish as a surface, but there is usually something that pushes me the solid route.)
My method is definitely not what I would call the "best" way to do it, but it is pretty fast.
Todd Blacksher- could you upload the sample on how you model a laser tube at an angle like the demo you did at the user group meeting last night 11/15/17. Thanks
You got it Wayne Schafer!
I believe that the sheet metal one that I uploaded in May was the same one I used last night, but here is the solid tube that I bent with the Flex tool.
Hi, I was talking about square tubes like this video: square steel tubes bending | CMM laser - YouTube. We already made some tubes like that but it's too long and unproductive.
This should work the pretty much the same for square tubing. You just have to select all the inner or outer faces to offset zero distance. I do it all the time.
If this is too "unproductive" for you, then "no". I can't tell you the best way.
I'll keep watching this thread to see what other people come up with though. Every little trick helps.
Sorry and good luck.
I originally guessed that was what you had in mind, and the video link confirmed it - very popular new technique for fully utilizing tube lasers . . .
This is an even uglier method, which I had planned to save for my SLUGME presentation this year, but if you "act surprised" during the presentation, I'll let it go.
Sounds like you are looking for something like this:
I have attached a parasolid as a "teaser" - I will upload the .sldprt shortly.
o.k. Here is a somewhat ugly, "outside the box" solution . . .
I start out with sheet metal, and leave a small sliver between the ends,
Simple cut & mirror for the cutouts (nice thing about sheet metal is that it will make all the cuts "normal to"),
Unfold the part and finish the cutouts (these "wrap" around the bends and the last side, so this is an easier method),
Fold it up to get back to your straight piece of "tubing",
Since it is sheet metal, you can use Sketched Bends to get the desired "finished" shape,
To fix the little "gap" along the open faces of the part, you can just extrude from surface to surface,
(This will make it so that you can no longer use the "Flatten" tool within sheet metal.)
BUT you can suppress your sketched bends to see the unbent tube!
This is what I save out and send to our tube laser department.
Make two configurations so that you can easily toggle between straight and formed.
hope this helps,
Remember, you have to act surprised if I show this for slugme
Here are a couple examples using surfaces.
Simon try something like this you can fold and unfold
there's many ways to design these pieces. I tougth someone brig me something magic but everyone was similar to my way. here's an example. To main feature is to be able to modify quickly the dimensions an angles.
Use one or two driving sketches with any one of these methods, and you should get the flexibility you want.
If this was something that I did a lot, I would create a start part with some rough information in the sketches that could be easily tweaked.
The good thing is that you were already headed down the right path!
You could use the same "sheet metal" approach in a different way -
Use your main profile as one side, then make the rest of the "tube" with a miter flange.
This makes it pretty easy to make tweaks on the fly -
btw, on your part I would recommend continuing your cut through the radius - it will make it easier to bend, and it won't "pucker" the corners. A bit of a bend relief will also help make a cleaner bend.
Definitely cool stuff!
Bending in one direction (normal to the thickness) is simple. What about bending in multiple directions?
Try this challenge!
The 3rd Weekly Power-User Challenge (May 5th, 2017): Bend a square profile in multiple directions and determine its flat pattern
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