Im trying to extrude sketch1 along a line i called sketch 2 to form some sort of a curved surface.
It says i cant do that, so im wondering what im doing wrong:
Is this what you are trying to create?
try to do a regular extrude with the sketch and it will highlight the part of the sketch with errors.
also, "extruding along a path" is called a sweep.
You can actually direct an extrude along a sketch path. It needs to be a straight line (or edge). This allows you to extrude in directions other than 90 degrees to the profile sketch. A sweep would be necessary only if you wanted to follow a curve or a multiple direction path.
there is a problem with sketch 2, run check sketch for feature and it will show you, then you can get it to work.
sweep only half and then mirror to ge the other half.
You can not extrude along a non-linear path. You will need to use Sweep. You need to also establish your path first, then your profile second - constrained to it.
As this would be a symmetrical part, I would start by editing the following:
Sketch 2 (profile) change the internal lines to construction geometry leaving just the outside line solid.
Sketch 3 (path) - convert one half of the line to construction geometry.
Do a surface sweep using sketch 2 as the profile and sketch 3 for the path.
Thicken the surface to 2mm
Mirror the body (merge bodies should be seletected)
This is what I ended up with.
Hope this helps...Good luck.
thanks you guys youre just great helpers!
troy nailed what i was going for so thanks you very much
One more question though, how can i make it look "sleek" without lines in the middle of the surface since it was done in two sweeps (besides changing view options)? im talking about what you usually do with splines using sketch fillet
To acheive the "smooth" effect, you have to edit sketch 2 again and apply the "fit spline" option" (Tools>Spline Tools>Fit Spline)
See attached to see what I am refering to.
All the best...Brian
Hi all, thank you for your great help
I have another question though, 1. how do i add thickness to the part troy posted? 2. How did troy using sweep chose only an edge as a path and not the entire sketch? imt trying to do it myself and it keeps choosing the entire sketch as a path -> error
the simplest way to thicken a surface is insert -> boss/base -> thicken.
for selection control, right-click and chose selection manager.
If you look at Surface-Sweep2 you will see that I converted the two edges into one Composite Curve and used that as the path or you can use the selection manager as Jeremy has suggested.
Though Troy has shown you a way of creating the part you're after, if you want a more elegant solution I'd recommend following the instructions Brian left.
Sadly i cannot open Brian's file because it says its a future version.
What I have is a student version solidworks 2011, theres a 2012 already? :-) anyway to convert it to 2011 so i can open it?
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