CAD Forum

One of our groups that uses Solidworks is asking to try out NX because they don't believe that Solidworks is capable of modeling their product, which is a very large spiral-wound steel cylinder made from curved rectangular (?) plates. Picture a paper towel tube but made from short lengths rather than a continuous strip of material:
I always say that you can do anything with every CAD package, the only true difference is the user experience (how quickly and easily I can do what I want to do).

I would be surprised if Solidworks cannot offer some relatively straightforward way to model this. Perhaps there are some limitations in the weldments module?

We are going to give this a shot @rodface .. It's kinda confusing and hard to grasp just exactly you want to do with this. Apparently you do not want (or can't do to manufacturing issues) make it in one piece. Do you want to make each revolve of the helix one piece? And if so you can't just make the sections cylinders (non helical)? My screenshots are with the helix/spiral style. Made it from sheet metal so I have 8 flat patterns. The six in the middle are identical and the two ends are the same. If you need the cuts staggered and at an angle similar to your red marks on your tube I suspect that can be done also. Maybe we can kick around some ideas. If you would like to do two or more turns per body, that can be done also.

Ok,, I managed to come up with something that looks more like your screenshot. Made a surface extrude of a circle and sliced it at an angle. then took the surface bodies and made lofted bends from that. then patterned the sheet metal loft.

We used spiral wound aluminium tubing extensively back in the day to manufacture long cylindrical pressure vessels - high voltage gas insulated busbars.

So you have a required tube diameter and strip width - what is the wrap angle ? Best explanation I've found is this:

https://www.apogeerockets.com/education ... ter304.pdf

Thank you for the responses, I'm studying in detail. @Dennis Bacon the result in the 7:20 post looks almost dead-on to the real thing. One observation I made (I did not use a real photo for confidentiality reasons) is that the seam lines for the individual sections appear to "rotate" along the length of the cylinder. In other words, if I draw a line from one end of the cylinder to the other, parallel with its axis, it will intersect each seam at a different point. I will try and mark up your screenshot to better describe what I mean.

And yes I presume that this cannot be manufactured from a single sheet due to the size, I think we are talking about a cylinder that is 20-30 feet diameter at least.

I attempted a markup of what I am referring to.

One thing I also noticed is that the product (at least in the photos I have seen) seems not to cut "flat" at the end, rather the rectangular(-ish?) sections are left whole, producing that pointed end as it wraps around.

I don’t see any reason this is not modelable in SW, using a number of different methods. Which methodology to use depends on what you intend to use the model for and how, and what your manufacturing parameters are. Do you need flat patterns for each plate piece? Does it need to be modeled as a single part, or do you want it to be an assembly? Are you going to put holes or other features on the sides of the tube that must be in the flat pattern so they can be pre-cut before forming and welding? Any particular spec for how the seams between each strip must line up or not line up?

Here's just one way to do it. The length, diameter, end piece shapes, raw material sizes etc are set up in the first sketch, then each section is individually wrapped onto the cylinder and thickened. There's a tiny gap between each piece to avoid zero thickness geometry errors, although that could be a weld allowance etc.

And here is another start. I believe the OP is trying to use like a 4'X8' sheet rolled in such a way that that several sheets end to end create a spiraled tube. But... then I've been wrong before. This is the attached part is just a start. I'm not sure what I would do if it was me trying to create the OP's design. One thing I have found out in SW is that in order to utilize the flatten part or unfold or convert to sheet metal it almost always requires a flat spot. Hence the short flat spot in my part.

DLZ_SWX_User wrote: ↑Thu Aug 29, 2024 1:50 pm And here is another start. I believe the OP is trying to use like a 4'X8' sheet rolled in such a way that that several sheets end to end create a spiraled tube. But... then I've been wrong before. This is the attached part is just a start. I'm not sure what I would do if it was me trying to create the OP's design. One thing I have found out in SW is that in order to utilize the flatten part or unfold or convert to sheet metal it almost always requires a flat spot. Hence the short flat spot in my part. image.png
image.png

To be honest there is probably a better way to design it to get it to flatten & to be able to adjust for different diameter barrels. I have only been working as a designer & with SolidWorks for a little over 3 years. Prior to that I worked in the dairy industry and had very little knowledge in engineering.