Flat pattern problem

I'm designing 1.2m long RC-boat using SolidWorks 2006. I have made own plane for each frame and then lofted frames. My problem is that I don't know how to flatten sides and bottom? Could somebody help me? If you don't understand how I have made the hull here is the image http://hezzu.daug.net/hull.jpg

 

think you're lookin for this:

http://www.touchcad.com/

 

With the older versions of SW you had to have SurfaceWorks to do what you want to do. With the newer versions I think they are all one program. Search the help file for surface development or panel development. If they can be developed it is possible to use many different programs if you can export the proper file.

Gary

 

Or try Rhino

 

If you use the sheet metal tools to make the surface or thin feature you will be able to open a drawing and choose flat pattern from the dialogue. search the sheet metal tools in the help menue. Hope that helps

 

dougfrolich:

I have tried to loft using thin feature and then moved to the drawings but I can't find flat pattern from the dialogue. Do I need separate the side somehow before I move to the drawings or what I do wrong?

I think that there is not easy way to make lofting (or same kind operation) using sheet metal tools. Is there?

 

You can used "Lofted Bend" to make a feature but it will only loft two profiles,(I did not realize that) Then you can use "Unfold", to make it flat--But that won't work for you either,I see. I looked through Surface Tools too and could not find anything helpful. --Sorry
I Import Hulls from Maxsurf, it is very good for generating hull and foil shapes. Then I finish the deck and inside with Rhino or SolidWorks-

 

To make hull plates in solidworks that can be flattened you need to use the "lofted sheet metal" comand. Sheetmetal parts cannot have any other "bodies" in the same file. You will need to make a new part for the hull plate and the topside plate.

start with the hull shape you have. I assume it is a part. Use it to start a new assembly file. This hull shape is now the "frame" the sheet metal plates will be built on.

Insert a new part in context into the assembly. Edit this new part in context. Start a 3d sketch and copy the shear line from you hull shape part. Start a second 3d sketch and copy the chine line from you hull shape. Now use the lofted sheet metal command with these two sketches. (You might need to be sure the two sketches do not touch at the bow, otherwise you will get a self intersecting geometry error). You should now have a sheetmetal topside plate that can be flattened. You should understand that Solidworks does not produce true developed plates. In models that have extreme differances of curviture between the shear and the chine, or the chine and the hull, the modeled sheetmetal will show concavity. Imagine a pringle chip.

If this does not work for you, Rhino is a great tool. The demo version with its 25 saves should be enough to do the trick.

 

E Hanson's instructions were the right way to do this. Keep in mind, however, that your model is symmetrical. You only need to model half then mirror.

As for 'true' developed plates, if the surface is developable, SolidWorks will flatten true. You will need to set either the K factor for this material or enter a bend allowance or deduction in line with whatever the shop practices are. In SW 2006 you also have a sheet metal guage table that you can use. If it is non developable, SolidWorks will not flatten it and will error if you attempt to insert bends. Developable plates are those that curve in only one direction. A pringle chip will not flatten in SolidWorks.

No matter how hard you step on it.

Cheers,

Rick