Hello
The following image will certainly explain better what I want to achieve, The goal being to symmetrize the surface with respect to the vertical and merge it with the existing volume, but I don't understand how to do it in solidworks 2018.
So in fact, make a volume delimited by these profiles:
Thank you for your help
Hello
Why not make a circular revolution and apply a shell function if necessary then symmetrize what you need??
Good evening
Although I could only look at this tomorrow morning under SW, and not being a specialist in surface at all, I would still say that you need 2 profiles and 2 guide curves.
For the profiles you use the small one that is vertical that you already have and I think you need another one that is vertical too but at the other end of your shape.
For the Guides uses the existing and the horizontal ones.
To be tested from Monday ;) (what do you mean we like challenges)
I also have a dedicated book on the surface under SW, see if there isn't something close to it.
Register your parasolid part for me
and posts the
I'll do this to you in SW 2017
Has SW accepted your surface straightening? ........... 1st image
if yes (but I have a doubt)
It's simple, just create a sketch on the base of the half dome below the surface
Convert entities
and extrude to the surface
then you make a symmetry
and it's closed
@+ ;-)
Good evening
Ac Cobra and Gt22 have already given you a solution, I'll add one:
Create your first surface by smoothing as you intended to do, make it symmetrical.
Hide all the volume around your surface (just to see underneath and to one side).
Create two flat surfaces to close your surfaces.
Sew them together and select the "Create Solid" radio button.
All that remains is to redisplay the volumes and merge everything.
@Ac Cobra, I don't think that in his case the revolution works because the horizontal and vertical shapes are different.
By you should also try the opposite of what I said, that is to say use your arc as a guide and use 3 shape sketches, the horizontal one on the left then the vertical then the horizontal one on the right, pay attention to the position of your click on the sketches, aim for the end on the arc side of the circle. otherwise the faces will cross.
Well, my last solution turns out to be the one that works.
After that, you have to set on departure/arrival at a tangent.
I also attach the image as a file to download to see better.
If necessary you can add a guide curve either halfway or a few cm or mm opposite the 1st guide curve. (to the right of the image)
It all depends on the precision you are looking for.
All that remains is to close the surfaces and convert into volume (I'm looking for the right solution)
Since you're in SW2018, I'll provide you with the file so you can go back up the tree to look at each step.
So before (or after) the straightening you have to create 2 surfaces that you will have to sew with the dome.
In the file I added a 2nd guide curve, of course its height must be identical to the central curve.
Super FUZ3D, I'm going to look into that.
But first problem a priori, I don't see the surface functions in 2018, I consulted tutorials 2016 where there was a Surfaces menu....
To answer gt22, my method failed with the message "Unable to create this feature because it would result in zero-thickness geometry."
Except that I only had half a shell because I couldn't achieve something similar with the small arc of the full background.
Well I tested the shell in my model and it's frankly strange.
Already, I couldn't realize this semblance of a shell when the side profiles were splines. I had to convert this to 3 arcs of circles like you did.
Then, I can't select the sketches but the open loops. I then arrive at this:
Another problem, maybe due to the "open loops", I don't have the constraint "Tangent to the face" but "Normal to the profile". I don't know if it changes much but in the end, when I try to constrain to the background arc with "Guide curves", the function fails with the message "Guide curve n°1 is invalid, it does not intersect section N°2"; Which I find rather unexplanatory.
Finally, I have the impression that I don't need the complementary surfaces and the sewing function because by omitting the fact that I don't stick to the arc of the circle, I get a volume it seems to me?
I'm attaching my model, it may be easier to identify what's wrong.
OK I'll look at it tomorrow morning. (annoying not to have the double home/work license anymore)
As for knowing if you have a volume or a surface, just look at the top of your creation tree, or simply make a cut that goes through your shape and you see if it's hollow or not.
See you tomorrow
Good night
So, I looked at your piece and it's normal that you don't have the same thing because you did it directly in volume and not in surface and therefore more appropriate if the goal is to make a volume. So obviously it's normal that you don't have the same words as the surface function.
As for the guide curve, you have to keep only the arc part and change the horizontal line to construction geometry or simply delete it.
Attached is the corrected part with the guide curve.
NB: It's a bit my fault to have made you the demo in surface, and I think it comes from the fact that you used the term Surface and merge in your 1st post, obviously I wasn't the only one, while yes (and can be seen on your photo) that we can do it directly in volume which will automatically merge (unless we unchecked) with the master volume.
So sorry to have misled by going through the surface. (even if the final result is the same but longer)
No FUZ3D problem, I probably didn't express myself clearly enough.
I understand that you are in SW2017, if someone can tell me how to access the surface functions in SW2018, it could be useful to me.
In any case, thank you very much.
Alan
If you right-click on FILE there will be a surface and you will have to click on it for your bar to activate and if not, do insert==>then surface...
Oh yes found.
Thank you