"And please dont comment the body disain my first body in solidworks :)and my first car body at alll "
Looks great to me, nice job.
Very nice car body
In order to do what you would like you are going to have to have the break points for the panels drawn in 3d, so that each section you want control over independently has the entire 3d border drawn, the sketch should include the gaps and tolerances you want between the body panels.
Once you have everything drawn up - and you can use every single 3d sketch you have - start a new 3d sketch and use convert entities to convert all the edges of a single piece, from there you can use a "fill surface" to create just that section.
If you want to combine multiple sketches 3d and 2d into one sketch you use the "composite" sketch option found under insert - curve.
then each piece can be thickened using the thicken command.
Alternatively you could just draw a 3d sketch over the body you have now and using surface extrudes you can trim away everything but one panel and repeat this under different configs until you have each panel as a separate single body, then make assembly from each config and you will have an assembly built entirely out of sectional configs all based upon a single body that is based upon one -ten master sketches...
or since there is so much symetry try to cut the door s out from the rt plane, the front window from a plane inserted perpindicular to its curve, and the trunk much be more difficult but manageable using a 3d sketch
good job so far.
I build furniture but use surfacing quite a bit...
Ok thanks for anwsering. I try to do somthing but to me it is very hard to understand your explanations because specific termins and i do not understand what i have to do exactly because i have larned solidworks by myself and so those expressions ...do not completly understand them ...
so if you could use more specific words connected to real commmands mayby i understand better
But start working on it after couple of days...
found some article where somebody told that he always make first model to see overall design and if that is in place he makes new model so that the ree is in right orded and so one ..i think i'm going on that way because complex commands are quite hard to understand right now to me ...
like i told had made some school rpojects in solid works but never used surface tools so ...:D ...
Use the convert entities tool to make a new 3d sketch out of the pieces you want to keep individual,
1. start a new 3d sketch, select the edges that would contain a surface that you would like as an individual piece and hit the V key on your key board - now you have converted parts of other 3d sketches in to a single 3d sketch that defines a boundary, then insert - surface - Fill.
Then insert - surface - thicken.
You may have to add details that separate out each section, changes made to master sketch will automatically update into the converted sketches as long as you don't delete and line or add any sketch fillets.
You have no reason to apologize for your car!
I find it interesting that you prefer to work with 3D sketches. I am just the opposite, only using 3D sketches when I am forced into it, much preferring 2D sketches.
I suspect that some of the problems you are having with thickening your surfaces are inherent in SW and your design. In real sheet metal, you can form the metal so that it doesn't have a constant wall thickness. That's how they get outside creases that have a tighter radius than the sheet metal thickness. SW will not be able to do that with a straight-forward thicken command. It can often do it if the outside radius is always smaller than the thickness, so that the inside becomes a simple edge. It almost always fails if the outside radius goes from larger than the thickness to less, so that the inside transitions from a radius to a sharp. If you made sure that your outside radii were always more than your wall thickness you would not have nearly as much trouble, but it probably won't look the way you want. I can't give you any easy way to fix this type of issue. At least in some cases you will just have to thicken parts, trim the inside edges to remove the bits that poke through the mating parts, and then join them together. To make the trimming easier, you might want to build the original surfaces so that they extend a ways past the mating surfaces. Another method would be to offset surfaces to the inside and then mutual trim the inside surfaces to one another. This will require you to build the surfaces on the outside edges that close the part to make a solid. No matter how you do it, it will probably be a lot of work.
Yes last night i find out a way to "bend" 2d sketches ...and found out some ways how to do in 2d sketches lik "bending" sketches and using more trimming.
for example to do whole side of the car with on surface and then cut in front and in back it to lengtht ..
but thanks for your last anwser that was a lot of help ..now i think i maybe only thikness parts that are connected to somwhere and change my oeall approach how to design a car in solidworks ...i think i maybe delete all faces an then with a help of sktches taht i have make a new body with different build up ....keeping mind your ideas and what i have leaarned in last day in different articles and videos lets hope this time i succeed ..
i keep you posted