(what the difference with part design WB? Also unclear to me)
This is probably the source of most of your confusion.
Part Design Workbench is intended to construct a
single complex solid for a series of simple features. When you start a project in Part Design, you
always begin with an additive feature such as a Pad or Revolve, never a subtractive feature like Pocket of Grove. Once that first Feature is created, you then apply to that
single solid, additional features, which can then be either additive or subtractive, but are always features of that same base solid. This is considered to be linear construction.
In the Part Workbench, you have tools to make solids from shapes and then to make new solids through boolean operations between 2 or more solids.
Lets take a simple example. A basic cube with a hole in the center. First let's construct that in Part Design.
1 - Make a Square sketch 10 mm each side and Pad that Sketch 10 mm.
- Shot1.png (6 KiB) Viewed 2416 times
2 - Now click on that Cubes top surface and create a new Sketch and make a 2 mm radius Circle in the center and Pocket it Through all. That pocket is now the
second feature of the
single solid.
- Shot2.png (6.31 KiB) Viewed 2416 times
Now start a new document and switch to the Part Workbench.
1 - Click on the default Cube and then the default Cylinder. Notice that you now have 2 separate solids in your new document.
- Shot3.png (4.49 KiB) Viewed 2416 times
2 - Using
Edit > Placement ... change both the X and Y Translation values to 5 mm. This will put the Cylinder in the center of the Cube. Now Select Cube, then holding on the [Ctrl] key Click on Cylinder in the tree view, (in that order), and then select Cut from the toolbar.
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3 - Now select Cut from the tree and go to
Edit > Placement ... and change both the X and Y Translation values to 30 and click OK. now expand Cut in the tree view and make both Cube and Cylinder visible. What you have now are 3 separate solids. Cube, Cylinder and Cut which is parametrically linked to the difference between the first two solids but is in fact separate 3rd solid.
- Shot5.png (6.08 KiB) Viewed 2416 times
This method of construction is called CSG, or Constructive Solid Geometry. While both methods produce the same looking part, they in fact accomplish this in very different ways.
Constructing something like a propeller is
NOT a task for someone new to FreeCAD, or any parametric CAD for that matter. You really need to have a grasp of the basics first and that is something that is not learned overnight. It can take weeks, if not months.
To pick up on another note. FreeCAD is a
Solid Modeler and has the capability of converting solids into meshes, usually for export or FEM analysis. Within FreeCAD, you either import a mesh or you intentionally created one. They just don't pop up out of nowhere and when you have one imported or intentionally created, they have a unique icon in the tree view and a different color (by default) in the 3D view.
Mesh icon -
which looks completly different from Solid or Shape icons, so it is very easy to tell the difference, once one learns the basics.
As it has been said before, CAD is hard. Once that fact is accepted and one makes the decision to learn, you'll quickly find out that it is not impossible and maybe not all that hard as it first appeared.
Mark