In this article, I’ll be writing a detailed transcript of how to create a parametric tapered footing in FreeCAD, similar to the one given in SP-34
So, the resulting model will look something like this:
We’ll start by creating a new file and then opening the sketcher workbench. Then we’ll select the create new sketch option and set the orientation to XY plane.
One may increase the grid size as per convenience. Now, simply create a rectangle any size from sketcher geometries toolbar. Always create the geometries around the origin for better references of constraints.
Now by simply selecting the end points of any side of the rectangle and the axis perpendicular to that side, create a symmetry constraint between them from sketcher constraints toolbar. Similar apply this operation for any of the adjacent sides of the rectangle.
Then selecting any horizontal side, fix its horizontal distance and give it a name say length. Similarly, do it for the other side too by setting its vertical distance and name it as width. Here in this example I’ve taken L=1200 mm and B=1000 mm.
After getting a fully constrained sketch, close the sketch and rename it as Base from the tree view and also save the file with the name Tapered Footing.
Now, once again create a new sketch on XY plane but with an offset of 150 mm, as this will be the top of the footing.
Similarly, as of the previous sketch, create a new rectangle with relatively smaller size and apply all the operations as done earlier. Set L=350 mm & B=250 mm.
Close the sketch and rename it as Top.
Then open the part workbench and select the utility to loft from the part toolbar.
Add both the sketches to loft and tick the create solid. Then press OK.
Now, create a new sketch on XY plane at the same offset of 150 mm. This sketch will define the extrusion of the column to be attached to the footing.
Once again, create a similar rectangle with relatively more smaller size and apply all the operations as done earlier. Set L=300 mm & B=200 mm.
Rename this sketch as Column. Then opening the part workbench, click on extrude a selected sketch option.
Select custom direction and set Z=1.0 and leave others as zero. Set length along to be around 50mm and tick create solid. Then press OK.
Rename the extrusion as Column’s Height.
Now we’ll select the base sketch of the footing and extrude it in direction Z=-1 and length along 150 mm.
Rename this extrusion as Depth(d).
Now, create the final sketch for the base of the slab for the footing, i.e, PCC. Set the orientation to XY plane and set an offset of -150mm.
Once again, create a similar rectangle with relatively Larger size than the base of footing and apply all the operations as done earlier. Set L=1300 mm & B=1100 mm.
Rename this sketch as Base of Slab.
Then opening the part workbench, click on extrude a selected sketch option. Select custom direction and set Z=–1.0 and leave others as zero. Set length along to be around 80mm and tick create solid. Then press OK.
Rename this extrusion as Slab Thickness.
Now select all the part objects created till now and select Make compund from part toolbar. This will result in a single part object.
Now opening the Arch workbench, create the structure by selecting the the compund object.
Change the role of the newly created structure to Foundation from the data properties.
The modeling of parametric structural tapered footing is completed here. There are some other BIM related parameteres that we’ll also define here.
Create a building object from the structure and change building type to Residential-House.
Then create a Site object from the building object and change its GIS parameters.
One thing more that we can add material to the structure from create material definition in arch workbench only.
Now selecting the site object, export the file as IFC.
Finally you recheck it by opening the IFC file just created.
NOTE: There can be other methods too for modeling such parametric tapered footing. However, satisfactory results can be obtained from this method too.