How to build a fuel Tank

[phil1284]

Hello Users,

I am a beginner with FreeCAD and want to model a fuel tank.
My version is 0.18
the inner part of the tank is no problem, just an extrusion of a b-spline.

With the side walls I am stuggeling.

the schape should be like this:


this was modeled by a sweep of these two sketches:


The problem is that it doesn´t create a real solid:


Is it possible to use two parallel splines to prevent overlapping or is there a complete other way to get such a shape?

I tried also with revolve and common of different solid shapes.

Thanks for your help.

[chrisb]

You may want to have a look at the Curves addon workbench.

[kisolre]

Remove the straight inner part of the profile so that the remaining curved part will have size smaller that the minimum curvature radius of the path. Fill the resulting hole.
Could you attach the file with those sketches for better explanation?

[phil1284]

thanks for your suggestions.

@chrisb: i will try that workbench

@ kisolre: changing the profile of the sweep results in the same error. the overlap at the corner is still there.

File is attached

[mrdic]

It appears that the top and bottom of the tank are flat, and the sides either have draft with the upper edge radiused, or the sides are a continuous fillet into the upper surface. You can loft between the lower edge and an upper profile, then fillet the upper perimeter edge, or extrude the profile then fillet the upper edge.

[chrisb]

I found an issue with a modification of this model, see https://forum.freecadweb.org/viewtopic.php?f=3&t=48043.

[chrisb]

You get self intersections as soon as the length of the section is longer than the smallest radius of the path.

[papyblaise]

Your aproch is too complicated , you use two b-spline that Fc isn't fluant to use it
My proposal is use a simple sketch , extrude , and large filet around it

[chrisb]

Here is a proposal. I changed the path to get smoother edges and changed the section too. BTW: The shape of the tank looks rather arbitrary.

The changes yield this:

Snip macro screenshot-bd4aed.png (13.91 KiB) Viewed 238 times

- To close the hole I created a simple copy and downgraded it 3 times in Draft to get the wires. I deleted all unnecessary stuff left over from the downgrade

- I added a dimension for the height to Sketch

- I extruded the wire in Part WB to the height previously defined in Sketch

- Finally made a union of the two parts. The union passes CheckGeometry with BOPCheck enabled.

Snip macro screenshot-84c429.png (11.58 KiB) Viewed 238 times

[chrisb]

Just saw papyblaise's proposal, and he is right: keep it simple.