I'm trying to use the last sketch and wrap it on the curved helmet surface, so i could extrude these rectangles from the surface of the helmet.
Solidworks wont let me use the Wrap tool, does anyone has a solution for this
Are you sure you want something like this, radiating from the surface (like an offset)?
By the way, I tried searching for other examples in the forum but couldnt find one that explains why I cant wrap it on the helmet surface.
Also tried projected curve..
I realy need your help guys,
It doesn't like the thicken surface.
It will only take what is shown below.
What is the endresult you are looking for? Lets start there.
Thank you for the reply
I also tried doing that wrap before thickening the surface and it didnt work.
Im trying to extrude some rectangles across the surface of the helmet, so they are curved like the surface and all in the same height.
An example would be shredder's helmet :-)
The wrap works only on cylindrical, conical, planar, revolved or extruded faces.
Just make sure you have only one contour per sketch and use the Project Curve feature. So create 3 sketches and it will work.
Even better, use the Split Line Feature and split the face as per the original sketch.
Also, read this article (click on the image below):
wow that looks great!
would you mind attaching the file as well? i learn best by supressing feature by feature to see the process
Also, this might be a silly question but how can i extrude the sketch now that it is curved on the surface?
In what direction do you want to "extrude"? Normal to the surface?
Then is exactly like in the article I mentioned.
1. Use the SPLIT LINE feature to create new faces on the top.
2. Copy those faces in new surface bodies (OFFSET SURFACE ZERO)
3. THICKEN the newly created surface bodies.
some of these features i never used before, ill give it a try.
I just wonder why I cant do a normal extrude like your student did (not that i want to, i just tried and it didnt allow me to).
When extruded, your sketch has to be completely inside the surface projection on the sketch plane. Imagine the top of the helmet as a boundary or a stop face. You should not "spill" your extrusion past it.
from here it looks about right, im wondering about the sides since i cant realy see them
unless you wanted to extrude from the original sketch plane on a direction perpendicular to the sketch plane:
Which trimmed with an offset surface of the helmet looks like that (quite ugly):
yea thats not what i was going for
im trying doing it one rectangle at a time, making a curve feature but now when i try selecting a face to offset it seems like i have none to choose, how did you do it?
Just so you know, I am creating a video showing all the possible solutions I could came up with inside 5 minutes. Will send you the link shortly.
That would be great!
I'd love a link when its ready
uploading now. another 20 minutes or so...
Click here or on the image below to watch the video:
One more thing. In the end, do not forget to combine the solid bodies into one.
Thank you so much, you've done an amazing job with the video !
The radiation was exactly what i was aiming for, but the second option for the vertical was so impressing that i created one as well to save aside so I could look back and remeber how to do that in the future
your students are lucky, my solidworks tutor hasnt answerd my emails since the begining of the semester
Hello again, Alin. Can I bother you with another question?
I want to create a hole going through the feature you helped me create. I want it to go somwhat in the middle of the feature, though i want it to be a constant radius hole because im later on inserting a rod that is supose to go through that hole with the ability to move along it, therfore the hole cant be "curved" and needs to be of constant radius.
I hope im explaining myself right.. the file is attached.
You can probably use a Sweep Cut to make your holes. You will need a Path and a Profile. The Cut sweeps the Profile along the Path. You can probably come up with a reasonable way to center the path between the curves that you used to make your ridges.
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