Solidworks Student - Flattening curved sheet metal?

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narfi

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I am teaching myself some of solidworks.
Wife wants a model boat shelf behind the toilet, and work has a new cnc machine we don't know how to use yet. So Ill play with it on my own time so they don't waste money on my learning and maybe momma gets a nice shelf out of it.

I can draw out a flat panel no problem and go through all the cam steps as far as simulation and it all looks to work just fine. So for example I could cut out a plywood instrument panel easily.(well i shouldn't say easily till ive done it i guess, lots to learn still)

I can model what I want for her boat shelf 'okish' but struggling to take curved panels and flatten them for cutting. Is that a payed only feature, or am I just doing something wrong?
It seems like something you would want for most projects.....?

Using the student 2018 version license acquired through my eaa membership.
 

ScaleBirdsScott

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As far as I know, if you have curves that are more than just a simple bend in a flat sheet metal profile, most programs don't have a proper way to unwrap them.

I have seen that the new 2021 version of Inventor is offering a way to unwrap complex stamped and curved geometry into a flat pattern, but I think this is more for, well, stamped parts and not say a large curved sheet or similar.
 

tdfsks

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I cannot comment on the student version of Solidworks. However, I have commercial licences for Solidworks Standard and Professional and these both flatten sheet metal. The software can in general flatten parts folded from a flat sheet using flanges etc or lofted bends between cross sections (such as wing and fuselage skins).

However ......

It works fine in simple cases such as parts with simple flanges and parts such as classic sheet metal ducts for air conditioning etc that might be a simple circle to circle or circle to square loft. The sort of developments that can be readily produced on a drawing board by triangulation.

However, for more complex shapes that are of interest to aero engineers, say a lofted skin between frames in a fuselage it does not work properly. The people who wrote this clearly don't understand how to loft a development like this on a drawing board and don't understand the more general principles of lofting developments, consequently they got it wrong when they wrote the software. The reason for this is a bit difficult to explain but I will try. If you wrap a skin around two frames the sheet can only curve one way and essentially the surface is defined by a series of straight lines that lie on the surface that join points on the frames at each end. These lines should join points on each frame that have the same tangent slope (see Raymers book on aircraft design for an explanation). However, in Solidworks, for these types of developments, they don't do this. Instead they simply divide each curve into say 10 segments of equal length and connect the corresponding points. The resulting lines do not lie on the surface of a sheet metal wrap and you can get some strange shapes. The skin shape is exact if the lofted skin is between two frames of the same cross section but becomes stranger as the shapes of the frames differ more from each other. The software will still flatten these skins but the development is wrong, as are any intermediate sections that you generate through the skin using the intersection tools.

Anyway here is an example of a simple flat development of a fuselage skin in Solidworks.

Sheet Skin.png

Sheet Flat.png
 
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Jay Kempf

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SW flatten command is available in the higher level packages. We ran into this in a mixed office where the lower standard packages didn't have the command. Lower packages can edit the command if generated in another package. Weird.

It triangulates the sheet and then uses a finite element sort of approach to flattening the panel. There are some resolution and approach controls.

You can undo some simple lofted shapes with the sheet metal commands as well. Look at the help section or Youtube for examples of lofted sheet metal unfolding. If you have specific questions I can help you post an example or PM me.
 

Mavigogun

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Speaking to developing fabric skin patterns- but also to other sheet material -the add-on ExactFlat is a common recourse. Find it here:

 

Jay Kempf

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At $7k you would have to have a big need for flattening outside of what is already built in to SW.

Flattening to DXF in stock SW works pretty well for laser cutting or any other CNC. Have also used it for flattening composite lams and for making mockups. Works really well. One project I flattened an overhead structure for a gullwing application and CNC cut and scored the profiles in plywood, scored them perp to the curve direction and then just pieced them together to get the 3D shape full scale. Worked great.
 

Hephaestus

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Fusion360 it actually does sheet metal skin unwraps fairly nicely. Free hobby/student license. But it's a very different workflow than SW so switch may make you crazy...
 

narfi

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Here is the simple panel I want, I dont know best practices, but I sketched out the shape of the top of the panels, and then scaled down that same shape on a plane below it, and then used insert surface loft to create the side panels and transom.

1588956164084.png

I know the side panels should look something like this,

1588956487640.png

But I don't know how to find that flat shape for cutting out.
Does that make sense? Or is my approach wrong?
 

narfi

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Thanks, Ill take a look. But I think I figured it out....... or atleast in the right direction.
It wont let me convert closed sketches to sheet metal, I deleted all of the boat except the one side from my upper and lower sketches, so it was just a single curved line on each sketch, then did an insert sheet metal lofted bend, and that worked to make it a sheet metal part, and it allowed me to flatten it.

1588960261996.png

So now I just need to figure out how to convert my closed sketches into open sketches at the 3 points, so that I can make each separate panel a sheet metal part.
 

narfi

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Ya, you can’t bend a sketch- gotta bend the part.
I realize that :)
What I am saying is that it wont allow me to make the part from a closed sketch (meaning the closed loop of the bottom panel. The surface tool lets me do that, but the sheet metal tool does not.

How do you convert a closed loop of 3 lines into 3 seperate lines in the same location but 'not connected' ??
 

Hot Wings

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How do you convert a closed loop of 3 lines into 3 seperate lines in the same location but 'not connected' ??
If I understand the question:
Just open a new sketch, even on the same plane, and use the "convert entity" option and just select the line segment you want.
 

narfi

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If I understand the question:
Just open a new sketch, even on the same plane, and use the "convert entity" option and just select the line segment you want.
So if I understand you correctly, I want 3 sketches each with one line instead of one sketch with the same 3 connecting lines?
 

Hot Wings

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So if I understand you correctly, I want 3 sketches each with one line instead of one sketch with the same 3 connecting lines?
Depends on what you are doing. SW is kind of picky about combining closed and open sketches in the same operation.
Gets kind of hard to explain in words. This is going to be one of the upcoming problems with online school. Sometimes there is just no substitute for one on one real time help.

For converting a closed shape into a sheet you might try the same trick we use with pipe to unwrap a fish-mouth. Just slice it up as needed with a very thin cut - like .001" thick.
 

ScaleBirdsScott

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However, for more complex shapes that are of interest to aero engineers, say a lofted skin between frames in a fuselage it does not work properly. The people who wrote this clearly don't understand how to loft a development like this on a drawing board and don't understand the more general principles of lofting developments, consequently they got it wrong when they wrote the software. The reason for this is a bit difficult to explain but I will try. If you wrap a skin around two frames the sheet can only curve one way and essentially the surface is defined by a series of straight lines that lie on the surface that join points on the frames at each end. These lines should join points on each frame that have the same tangent slope (see Raymers book on aircraft design for an explanation). However, in Solidworks, for these types of developments, they don't do this. Instead they simply divide each curve into say 10 segments of equal length and connect the corresponding points. The resulting lines do not lie on the surface of a sheet metal wrap and you can get some strange shapes. The skin shape is exact if the lofted skin is between two frames of the same cross section but becomes stranger as the shapes of the frames differ more from each other. The software will still flatten these skins but the development is wrong, as are any intermediate sections that you generate through the skin using the intersection tools.
In my experience with this (at least in Inventor, it's been some time since lofting in SW) it's very important to use 3D sketches to force control lines for the lofts to follow. Otherwise yes, it will do some strange things indeed. When making my loft sections I will often use some reference geometry to create control points along the curve to be lofted. Then create a 3D sketch and use lines to make my own definitions of control. This tends to create much much closer approximations to what sheet metal will do when lofted, and is vital to create more accurate airfoils than what the program would like to make.

In other situations those custom control curves might be used to create bulged lofts or other such things. It's very very rare these days that I will make a loft without at least 3-4 control lines/curves/etc.
 

Jay Kempf

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Are you trying to get the outline to send CAM software, like a DXF or something? If so right click on the face you want and scroll down to save as DWG/DXF
 
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