You replied while I was typing but you should be able to adjust my file to your values...
dapab wrote: ↑
Sat Nov 21, 2020 9:47 pm
Can anyone please advise the best way forward.
there are many choices, it also depends on what data you are bsing you design. E.g. are you defining the angle of the sloping sides via an angle measurement or just by the lineal dimensions of the top, bottom, vertical height and wall thickness? If you are modelling an existing object then measuring those dimensions would be easiest. If so you could model it like this, this is also the easiest way from just a modelling point of view.
here is a screen shot
All I have done here is
1) simple sketch to define the outer dimensions of the base
2) the same but for the top
3) both sketches are attached to the XY axis plane of the Body when first created, so once created you then need to adjust the vertical offset of the top sketch by the amount of the intended vertical height of the pot (not the angled edge length which would be slightly longer). So in my example attached, look at sketch001, look at its attachment property, expand it, you will see Attachment...Position...z has been changed to 480mm which is the height of the pot (just change that value to what ever you want)
4) Select the first sketch, then PartDesign additive Loft then add the second sketch in the dialogue that pops up. You will now have a solid that you need to hollow out.
5) select just the top face of that solid (which the thickness tool will remove) then click on PartDesign "thickness" tool, add the value of the desired wall thickness, by default it is 1mm and makes the wall thickness go outwards, I guessed 10mm and toggled "reversed ...true" so that the wall thickness goes into the centre of the sketches rather than the default outwards
6) then I created another sketch on the xy axis plane, put three circles in it, one with centre coincident with origin, the other two with centres using "point on object" constraint to the horizontal axis. Then applied a radius to the centre hole, and an "equals" constraint between all three circles. Lastly I positioned the two outer circles with a Horizontal distance constraint, the value of which I defined via an expression that calculated one quarter of the total length of the base of your pot as read from the constraint in the very first sketch named "sketch". For convenience I anmed that constraint in that first sketch (gave it an alis) "base_length". If you use an alis in many places in FreeCAD, do not use spaces in the names as an Expression will not be able to read a name with a space.