Hi all
I'm designing a Potez 60, I made the fuselage with the sketches I could find (including a plan from 50 years ago, scanned in 300x300 resolution... so I'm not telling you about the hassle:)
So for the moment, no worries, I sketched on the side view, added front and bottom view planes to give it its shape, I then made a smoothing which gave me the surfaces of my fuselage I made a symmetry and I then put a thickness of 6 (inwards), which gives me the surfaces that will be in depron:
But, now, I would like to take the inner surface to make a full volume, which I could then cut out in order to design the reinforcements (by doing this, I would be sure that any part will follow the shape of my fuselage
The problem is that I don't know how to do it at all, I've been testing things for 3 days but nothing works
A little lead please? :-)
Hello
to get there; you just have to create a plane in the middle of your fuselage (if you don't have one yet) then create an assembly with your fuselage and in the assembly tab you make new parts and you select the middle plane of your fuselage; there you select the inner edges of the fuselage and you make an extrusion to the next face on both sides and that's it...
exemple.zip
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Thank you for your answer but I can't do it (or I didn't understand what you meant)
At the same time, I'll let you take a look at my fuselage, I think I did it a bit haphazardly (at the top fitting (symmetries), some parts don't even coincide:(
Otherwise I could do the opposite? create my inner part to cut out for reinforcements ect, and extract the volume of 6mm outwards to create the "depron" part
fuselage.sldprt
DSL I can't open because I did it with a version after 2016, could you do a step of the file?
Yes I'm sending you this, thank you anyway!
fuselage.step
Here is a part of the interior of the fuselage
fuselage.zip
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Awesome!! I'll analyze it tonight to see how you did it:)
Thanks again!
No worries, have a good evening :-)
Hello
Sorry I can't mail you the modified part because I'm in SW2019.
Here is a clue:
- Merge the volume bodies into your "Symmetry11" function
- Offset your inner faces by 0mm ("Offset Surface" function)
- Sew these offset surfaces
- Hide the volume body "Thicken7"
- Use the "Surface Fill" function to close the fuselage portion
- Use the "Thicken" function to form a volume.
- Show the volume body "Thicken7"
You then have 2 separate bodies
Kind regards
fuselage.png
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A huge thank you to you! It taught me a lot of things! (sorry for the response time but I'm in vac and not much network... and then I also enjoy the sun :)), now it's good, I'm on the spot!! :D
I decided to start from 0 because I found that the logic of my modalization did not correspond with that of my future assembly
So, I'm going to make a piece by cutting a balsa board or other and put them neatly in an assembly (which seems logical in the end!)
I just have one last little question, I looked a lot on the net and looked in the functions but I can't find it: I made the board that will be the side of the fuselage with a plan and therefore a sketch each time there was a change of shape in X or Y and I smoothed it out, that's OK, BUT I would like, in my assembly, to use the shape of the low edge (in blue) of this board to make the shape of the board that will go under my plane
By doing it like this I'd be sure that when I put it all together, it will be like dad in mom :-)
Thank you in advance for your enlightenment, I'm attaching the file just in case
EDIT: I take this opportunity to ask you which technique is the best... work only on one side and make a symmetry of the whole assembly at the end? or work directly on the whole? By the way, is there a "dynamic" symmetry? so that we can see the result in real time?
fuselage_cote_gauche.sldprt
Hello
If you want to have answers to your additional questions, I advise you to create another question. Since you closed the question by validating your answer as the best (!)
Kind regards
Phew, hell of a job.
The method I would use:
1 - In a room, create the 1/2 inner skin on the surface;
2 - insert this part into an assembly;
3 - create a part in the assembly, constrain it by coincidence of the origin (+check box alignment of axes).
4 - Creation of the flanks
4a - create a part in the assembly, constrain it by coincidence of the origin (+check box alignment of axes);
4b - Edit this piece in context;
4c - create volume by leaning on the surface (surface/thicken);
4d - Getting out of the editing in context;
4th - open the part, select the median plane and make insert/symmetrical part (this will create the symmetrical part);
4f - Insert the symmetrical part into the assembly, constrain it by the origin.
5 - Creation of couples
5a - create a part in the assembly, constrain it by coincidence of the origin (+check box alignment of axes);
5b - Edit this piece in context;
5c - create a ref plane at a distance from an existing basic plane along the axis of the aircraft;
5d - On this plan, create the sketch of the half-piece by leaning on the surface (via intersection curve). Trace only the outer outline;
5th - Get out of the editing in context, open the room alone.
5f - Extrude this sketch from the thickness of the plate;
5g - symmetrize the function;
5 hours - make the inner cuts.
6 - Repeat step 5 as much as necessary.
There, you have a complete and dynamic assembly with parts that you can open independently (be careful the link exists: -> symbol at the end of the name of the function in the feature manager) to make the drawings, export for NC cutting.
Yes sorry, I'm going to make a post again
Have a nice day
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