I will try to describe simply. I hope that it would help for starting point and you canmake better. All dimensions are example. Ive just tried to show way of it. If you remember iam using CATIA V5 R21 , if you have recent versions like R20, 19 ,18 etc you wouldnt open my CATPart so ive added step version of my data too. ( of course It doesnt have product history :) )
This is result of our drafting phase
We are starting a base profile of tank from top view. ( I always recommend symetrical approach for surface modelling processes) We are drafting half profile for it. Important point is keeping tangency at the end points of curve. It could be fixed by fillets etc after that but that would cause decreasing of surface quality.
We will use "Fill" command in GSD for base surface of tank. So we need some surface around boundry to use as our tangency referances. Ive used "sweep" command with draft direction option. ( Details can be reviewed by option box parameters in screenshot )
Now we have a good referance ( sweeped surface ) to draft our side profile. In sketcher iam drawing a spline which is similiar with side profile of chopper tank. Important point again : Try to keep tangency at end points of spline. We can use projected lines of sweeped surface for it.
We are extruding our side profile along normal direction of sketch. That will help us to keep curvature transtition between mirrored surfaces.
We will use "fill" command to fill surface between two guide ( bottom profile and side profile ) Of course we are selecting our support surfaces to keep tangency.
Now we can hide support elements ( extruded surface, sweep surface ,guides etc...) we dont need them anymore :) And we have half side of our tank surface
So we have to mirror it
Iam closing bottom hole with "fill" surface command. But iam not using support because i dont want tangency at bottom. After filling and joining operation iam adding fillet to bottom edge to have smooth tank
After that step we dont have anything to do in GSD module . So we are switching to Part Design module.
* First we have to make solid body by "close surface" command of PD module
* After it iam drafting a cylinderical profile in sketcher to give some space for frame of chopper
I used pocket command with frame profile. We would have smoot tank with a small valued fillet around frame cavity.
Lets add a simple cylinderical profile to have feature for tank cap.
Iam adding a variable fillet at intersecting edge between main tank and tube. As a last part of tank process iam using "shell" command of PD module to make our tank empty. We need some fuel to go :)
And ive added a simple cap for it as bonus.
I always like to say CATIA drafters have many options to achive their goals. My choice is just one of them. I hope that helps for you and rest of community. Thanks everyone for their time.