I want to continue to build this list (below) of items in my own way, that's why I titled the post with my user name in it. The wiki is free to use any and all my writings but my goals are to keep this short with few replies, mostly to tell me that I wrote something incorrectly.
First thing to do is get the newest release version. Then watch a couple tutorials and stop, try replicating what you saw. The learning has to be done in short enough sessions to remember what you saw. At least that's what I did.
Here is my top 10+ list using V17.xx and newer.
1)Use combo view(kind of a default), click Model tab and watch the tree, it shows your progress. View back and forth the tabs "Model and Tasks" alot.
2) Start your project in Part design workbench, it will automatically take you to Sketcher (to draw in 2D) and then back to Part design (once the sketch is closed) where you use the sketch to make 3D solids or add more features. Keep adding sketches and features until your finished. A Sketch really needs constraints to hold it together and in place.
3) In Part design you are working on a single solid part called a "Body", it can have many features, i.e. cuts, pads, patterns. The single solid is the "Body," it can't be taken apart or split in two or have 2 pieces. It is the smallest piece of whatever the designed device. You can also add more Bodies (Blue icon) to your current file. You might draw a cup as one Body and a lid as another Body. You only edit one (the selected) Body at a time.
4) If you need to bring some separated (different files) Bodies together, use File->Merge. You can create a kind-of assembly, more like a planned pile. Save that file and now you have a multi-body solid file. Part placement is saved with the file.
4.4) A typical design of a multi-part
unit like a box and lid can be accomplished in one Part design file
. The base of the box is one Body and the lid is another Body. Shapebinders allow referencing between the two Bodies.
4.5) The best way to structure something more complicated ( more parts, see item 12) is to use a part container (yellow icon). Freecad uses the concept of a body (Blue icon) as a single part/solid or a sub-part of the multipart Part container. A part container can hold many bodies or even more part containers. The part container holds all the objects in their place, this means you can move the part container and all object inside move with it. The Part container can't be arrayed in Part Design currently, you have to use the Draft workbench.
5) Learn to use Datum planes. You can place sketches on them and place them anywhere/any-angle. Change their offsets with the properties window. If you want to see thru one, select it (in the tree or work area) and hit the space bar, Visibility will change. To quickly create a sketch on a axis, goto Origin in the tree and select/highlight a standard axis, then create a sketch or create a datum plane and place a sketch on that.
6) If you don't see your part, click on it in the tree and tap the space bar. The space bar changes visibility i.e. visible or not.
7) Left click on anything in the tree and look at the properties in the window below it. Many of the values can be modified. There are 2 tabs in the property window. Get used to both.
8) Your mouse and viewing; work in Gesture mode, it's a good place to start. If you want to select something (whole) with a drag-window, goto Menu->edit->box selection.
9) If you can't see what you want, click the "zoom full" button.
10) If you try to apply a feature to a surface and you don't see it occur, try "Reverse " in the parameters or select Symmetric to get the best chance to see the feature because it applies in both directions from the surface. Thru-all will also help find pocket cuts.
11) As for viewing, "Draw style", do all your detailed sketching in "wireframe mode", then verify your solid in "flat line mode" or sometimes in wireframe if you think something is being created inside the solid and you can't see it.
12) A note about CAD; The wording used is kind of weird. We normally think of a part as a single item. CAD uses "part" more like a car part, it could be a windshield (single item) or it could be a transmission (hundreds of parts).
13) Save many times thru the design. Goto Menu->Edit->Preferences->General->Document->Maximum number of backup documents saved. Set it to maybe 50. Backups are saved with the file name appended with a number, they are saved every time you select "Save". If you ever need to restore an old version don't go by just the filename, check the creation date also.
14) When sketching, if you start drawing in Blue then you have clicked the construction Mode icon. Construction lines are reference only. Normal sketch lines are White. It can be troublesome if you get them over-lapping and loose track.
15) Go to Preferences->Sketcher->Marker size. I set mine to 9px. This allows you to pick line end points better and pick points for constraints.
16) When using Sketcher, lets say to draw a line; Mouse Left-click to continue with the drawing tool or Right-click to finish and close the tool.
Here is a post from Ickby some time in the past, I think it was just as version 0.17 was being released. A good list and right to the point.
Post by ickby » Wed Apr 13, 2016 11:34 am
As of now the FreeCAD 0.17 development version provides a largely updated PartDesign workbench. As workflow changed in many aspects here a overview of the most important new concepts:
Body. A body is a single solid created from multiple individual PartDesign features. It does group all features used for its creation beneath it in the tree. It does provide an Origin (Planes and axis) which can be used in the features as references. Furthermore it can be freely moved without making it necessary to move the individual features.
Part. A part is not related to PartDesign but is a new general FreeCAD element. It provides a local coordinate system and can be used to group any kind of FreeCAD stuff and move it as one unit. This will be the future basis for assemblies.
Active objects: There is now the notion of active objects. for example your file can hold multiple Bodies. If you create a new feature the feature is added to the active one. To activate a body double click it, the state will be indicated in the tree by background color.
It is now possible to create datum planes/lines/points and attach them to features. Those datums can be used as basis for sketches or as revolution axis etc. There are a multitude of attachment possibilities for datums, try them out
It is not needed anymore that a sketch is located on a face of a feature. Even if created anywhere in the 3d space the features get added / subtracted from the body.
Sketch based tools (pad, revolve, ...) now work not only with sketches but also with faces of a feature.
Cross referencing: It is now possible to reference things from a body in another body via datums. for example the datum shape binder allows to copy over faces from a body as reference in another one. This should make it easy to build a box with fitting cover in two different bodies. FreeCAD helps you to not accidentally link to other bodies and inquiries your intend.
Additional toolset: all relevant tools formerly exclusive to the Part workbench are now also available in PartDesign. The do have the usual different behavior: always creating solids, automatic adding or subtracting to the body.
Migration: Files created with older freecad versions can still be opened and edited. If pure part design feature based they can be converted to the new style via the menu ->PartDesign -> Migrate. If they are mixed Part / Part Design/ Draft the conversion will most likely fail.