Hi all;
I want to Create a 2 mm thick elbow and unfold it in solidworks 2014
So to do this, you have to use the swept folded sheet metal function.
But your tube will need to be opened so that it can unfold.
I'll attach a picture in 2 minutes
So oddly, I can't reproduce a round tube anymore in unfolded.
So I cheated a little bit and instead of a round tube, I took a polygon with a lot of facet, which is the closest thing to a tube.
So I drew this polygon on the plane on the right, then draw the trajectory on the plane of the front.
Don't forget to open the polygon, then launch the swept folded sheet function.
Check the "Cylindrical/conical body" box and select the polygon line that curves along the path.
tue.png
Bart, instead of taking a circular trajectory, have you tested with a segement constitutive tajector?
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No, but in this case, you have to choose the open round profile as the trajectory, and select the tube trajectory as the profile.
I leave you the honor and privilege of trying =)
Hello, working in HVAC (HVAC), our elbows have exactly the configuration of the one pictured by @NID. CAD.
They are made up of segments with folded edges and not in one piece.
Cdt
Joss
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Nn Mr Brat...
that's not what I want, unfortunately I want to get the format developed for the manufacture and then roll each hoop and finally weld them...
NB: the diameter is 240
In this case you have to make a tube in the way described by bart.
But just on a segement and do the angle cut at the ends, and you'll get the development of each section.
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Personally, what I would do is two perpendicular planes on which you draw the profiles of your tube, you connect them by a quarter circle and then, 4 other planes oriented at 11.25°, 33.75°, 56.25° and 78.75° on which you also draw the profile of your tube with your quarter circle as center.
Once this is done, you create sweeps that you unfold individually, you will get your five pieces of sheet metal unfolded and you adapt their width according to the millimeters that will be eaten up by your weld.
EDIT: of course, the profiles of your elbow must be open
Cdt
Joss
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+1 Joss !!
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For my part, if I understood correctly, I would do it in 4 pieces (2 identical for the end and 3 identical for the inside) I send you this.
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For my part, if I understood correctly, I would do it in 4 pieces (2 identical for the end and 3 identical for the inside) I send you this.
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Oh yes, and for the record, in general, the radius of the axis of your elbow corresponds to the diameter of your elbow.
(Basically, for a Ø240 elbow, you create a quarter circle with a radius of 240mm!)
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Hello
If you are an Axemble customer with the MyCadService offer, this type of elbow exists in the libraries provided by AXEMBLE.
@+
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Would that match?
For your information, it's in SW2014 format. I have just represented an example. To do again if that's right.
test_tube.rar
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See this tutorial
https://m.youtube.com/watch?v=VU8EjtD6Tgk
https://m.youtube.com/watch?v=4lThDl9txzo
@+;-))
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Well, I get it right.
Well, normally it should suit you.
=)
Edit: On the other hand, if you want your sheet metal edges to be at an angle, Solidworks 2014 doesn't handle it.
depliage_tube_cintree.sldprt
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Hi NID. CAD
I'm a little late but hey.
If you just want the lengths of your parts to cut, nothing could be simpler:
If you want like your drawing, it means in 3 parts + 2 small parts, or 4 parts (2small part together is worth a big one, it's mathematical)
for a 90° angle it's 90/4= 22.5° so 3 parts at 22.5° and 2 small ones at 11.25°
After for your easy length:
As a colleague said, you need at least a radius of 240mm.
If we place ourselves at the neutral fiber of your tube, we are at a radius of 360mm (240mm + 240/2mm (radius of your tube))
After that, it's mathematical, tangent 11.25=X/360 so X=tan11.25*360
====> Short Length=71.608mm
====> Long Length=143.216mm (Short Length*2)
That's the theory, but in practice it looks like this:
On your tube, you take your chalk (or your marker) you trace your two lines on the top and bottom of your tube.
You take your false square and you draw your first angle at 78.75° (90-11.25) and you cut.
At the point where the upper edge and your angle cross, you count 143.2mm (found by the calculation) minus 2mm because you have to anticipate your weld point (that's where the theory stops...) so 141.2 mm, you turn your squares over you draw (so you will have your angle of 22.5 (2*11.25) and you cut.
You start again until you have your three pieces
Your last song, whatever happens, is at 11.25° so it's perfect.
From there I think you know the procedure to follow...
This is where you have to make the difference in reality and virtuality. It's nice to do computer-assisted design, but if you want to be a good engineer or technician, it takes practice...
Good luck
PM
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