I always have to redo my designs. What am I doing wrong?

[chrisb]

Some issues reoccur and you are right, we should document them. However, it's a lot of work and so it isn't done (yet). It might be sensible if newcomers document these things.

On the other hand, I have learned myself, that 3D modeling is inherently difficult. Much more difficult than 2D, really! We have a guy in the german forum who used to work as a teacher for one of the professional systems, and he says, that they started with a 1-2 weeks course and afterwards the people had to exercise 8 hours a day for some more weeks. And those pupils where probably already well educated in the matter.
I have learned very much by listening to the forum. Whenever someone asked how to model this or that, I tried it myself, and often was surprised about the final solution the experts came up with.
It often is what I call "think perpendicular": assume you have a cube and want to chamfer one edge at an angle of 30°; instead of trying to do something to the edge or the faces building the edge you have to apply an appropriate pocket to one of the sides of the cube.

Thinking like that is not always easy, but it can be learned. And you have here the best support you can get.

[bejant]

Indeed the issue seemed to be coplanar surfaces. The surprising thing (for me at least) is that the shift needed cannot be arbitrarily small. It must be large enough, so that the planes are not "too coplanar" (sounds weird in a mathematical sense).

Hi ulfwin, and welcome! My understanding is that there is a tolerance in FreeCAD, where two points within this tolerance are considered to be at the same coordinates. I think the same is true for edges and surfaces.

Actually, besides getting help with this specific issue, I was hoping to get some general advice.

General advice:
Be nice to people, never stop learning, don't forget to wash behind your ears, always wear clean underwear, don't eat yellow snow, always --- oh, what? --- you want FreeCAD advice? Well then, here you are:

1. If you have a piece you need to create, upload a doodle of it to the forum and you will probably receive more than one way to create it.
2. In FreeCAD there are usually multiple ways to create a model.
3. Don't wait to ask for help and know that replies in this forum usually happen quickly.
4. Read other topics in the help forum, even if you don't understand them yet.
5. As with co-planar surfaces, concurrent seams can cause problems.
6. For Part Design using Sketcher:
   • Create an enclosed area.
   • Other enclosed areas can be inside an overall enclosed area; these become voids when the Sketch is used to create a Solid.
   • Only two white edges per vertex.
   • No crossing white edges.
   • Know which Constraints to favor and which to avoid:
     
     Good constraints to use are:
     • Horizontal/vertical length.
     • Horizontal/vertical constraint.
     • Point/Point tangency.
     Bad constraints:
     • Length.
     • Edge/Edge Tangency
     • Point on line
     • Symmetry
7. Understand the concept of a Feature.
8. Be aware of a resilient modelling strategy.
9. Learn how to create robust models and how to avoid creating fragile models:
   • A model will usually break if Links To External Geometry are used to link to a vertex or edge of a Feature and afterwards something earlier in the model changes.
   • Consider using one or a few master Sketches because even if a master Sketch is not used directly to create a solid (by Pad, Revolution, etc.), the included geometry can be linked to in other Sketches.
   • Learn how to use Expressions, particularly with Constraints.
   • Learn how to use the Spreadsheet WB with your models.
10. If you have to rebuild a model, or have to start again from scratch:
    • Don't delete your Sketches - re-use them instead.
    • Know how to use the Map Sketch To Face tool.
11. Loft never creates planar faces between Sketches, but Sweep does.
12. Don''t overlook the Thickness tool and understand that it is really a hollowing tool.

The issue here is one of many of very different types I've had with Freecad, and to be honest at times I've considered switching to something else.

Ask for help here first instead of deciding to switch (and then you're back to square one again - you have to learn some other software and the time you spent trying to learn FreeCAD becomes wasted).

Mostly I'm curious whether this trail-and-error approach is inevitable with Freecad, or it's enough to learn a few tricks (like the coplanar issue).

There is always some degree of trial and error when learning, and (to be clear) the co-planar issue exists in commercial software too.

[ppemawm]

Actually, besides getting help with this specific issue, I was hoping to get some general advice. Perhaps you can shortly share your views?

FreeCAD is a sophisticated engineering design/analysis tool. It is quite capable of creating complex models and assemblies. I use it as an experienced consulting engineer to routinely create mechanical models for design and FEA/CFD analyses. I also use it to create engine assemblies as a hobby such as you might find on the Users Showcase in this Forum.

As such, like any other complicated software, it has a steep learning curve. One must invest not 10's or 100's of hours but 1000's to become reasonably proficient. I started with Unigraphics I/II/NX many years ago and can attest to the having same difficulties and limitations as you are experiencing with FreeCAD, but with incredibly expensive hardware/software and extensive documentation. FreeCAD is free, open, runs on a laptop, but documentation is not the best and not always up-to-date, especially now with the migration to V0.17. In my experience, however, one does not learn from documentation but only by doing. Everyone learns differently I suppose but a few of my suggestions for newcomers:

1. Learn the CAD language and graphics user interface first by experimenting with each feature and transformation tool. Discover their limitations and quirks in as simple a way as possible, one tool at a time.

2. Pick a workbench and stick with it until you are comfortable. You must decide early on if you are going to use CSG (Constructive Solid Geometry) with the Part workbench or the parametric solids approach using the PartDesign workbench. I do not recommend mixing the two. In all the engineering work I do day in and day out I prefer the PartDesign workbench and rarely use or need the Part or Draft workbenches.

3. Developing a good modelling strategy early on is important, i.e. how do you start a model and what process should you use. It can save you much grief when you have to correct errors and make changes especially with more complex models. Google "Resilient Modelling Strategy" for some excellent guidelines on how to build robust models.

I highly recommend starting models using simple master sketches to which you can attach feature sketches. It forces you to think through the process before beginning to create the model features. The sequence of steps are important: additive/subtractive features, transformations, holes, then fillets and chamfers last. You will quickly find that there are many different ways to build a model, some better than others when you have to make changes.

4. Practice, practice, practice. Start with many many simple models (100's) before attempting more complex ones, i.e. do your homework, put in the time. After all, a complicated model is no more than a collection of simple features. I find a good way to learn is to try to recreate someone's file following the same steps in the model's tree history.

5. Get in the habit of fully constraining sketches in a simple manner as possible (fewest constraints). Many apparent software problems are solved or avoided by correctly applying constraints.

6. Do not attach sketches to model vertexes, edges, or faces. Period. It is a bad habit and a poor crutch. I had to unlearn that when I migrated to V0.17.

7. If you are new to FreeCAD, I wholeheartedly suggest you start with V0.17 rather than the older versions. It is quite different in modelling approach but much more capable especially when it comes to creating assemblies. The sketch/datum Attachment tool along with Shapebinders of master sketches are incredibly powerful. If you start with V0.16 you may have to unlearn some bad practices when you advance to V0.17.

7. Follow the Forum daily especially the Help section to learn from others as well as Open Discussion and Developers Corner to keep up with the concepts being developed.

Finally, try not to forget the old adage "it is a poor workman that blames his tools." I have to remind myself of that often.

[ppemawm]

I made one quickly.

Please note that this model is not valid when checked with Part>CheckGeometry tool. It is likely due to the coplanar surfaces. If not valid, it is likely that the model will fail at a later stage of the process when adding other features.

[chrisb]

Thanks bejant and ppemawm for these general hints. I have bookmarked them so I can reuse the link in the future.

I hope it's needed for FreeCAD questions only, although the general remarks might be valuable too, especially the one concerning colored snow.

[Tilli]

. . . FreeCAD advice . . . issue exists in commercial software too.

. . . is quite capable . . . I use it as an experienced consulting engineer . . . can attest to the having same difficulties and limitations as you are experiencing with FreeCAD, but with incredibly expensive hardware/software and extensive documentation . . . a few of my suggestions for newcomers . . . Follow the Forum daily especially the Help section to learn from others as well as Open Discussion and Developers Corner to keep up with the concepts being developed . . .

Merely to say, explicitly, thanks @bejant and thanks @ppemawm for taking the time to compose these "overview" posts.

Reading the plentiful, detail-heavy, posts which condense to "Help! foobar-abc failed ... Try barfoo-jkl ... Nope, you need to do foobar-pqr" reminds me of apprentices accompanying craftsmen to disparate, random tasks. You're watching and listening but lots of it goes right over your head at the time. And the lottery of "job-callouts" sometimes skews the perception of what's important or usual.

That's why I find it both helpful and extremely encouraging when experienced users like yourselves --- with real-world knowledge of both Engineering and the mythically-capable industry-tool Objects Of Desire --- offer us a little of the bigger picture.

It helps to have Context. It's good to read your reflective pieces and distilled wisdom. And comparative insights remind us that the megabuck emperors, though maybe not naked, still have their flaws and indignities. That surely strengthens wavering resolve when the hair-pulling episodes inevitably appear.

It was actually here I first encountered the phrase "Expert-Blindness." In the same way that not all cartographic-maps or natural-history field-guides present all the available information at the highest magnification, so too, it's good to have these introductory overview forum posts. Maybe a locally British thing, but how many of us, I wonder, began our route to later passions and expertise with a humble "I Spy" or "Observer's Book Of..." eh?

As a newbie, and speaking personally (but, I suspect, not just for myself), these sorts of posts are like accessible, cheerleader-lined, colour-coded, floodlit nursery-slopes before the eventual steep dark learning-curves. Ideally this style and level should, I believe, be much more prominently and widely peppered throughout the FreeCAD Documentation. It really does offer toe-holds which are otherwise missing. Helps us feel much more included, and often prompts the joining-of-the-dots and the laying-down of memory-pathways much more quickly than they otherwise would have.

Pre-existing CAD-insiders are a perhaps a special case, merely looking to learn a the local FreeCAD dialect. But for novice outsiders like myself, before you'll spend even those "10's or 100's of hours" you have to be convinced that the project's ultimately accessible and worth it. And I believe posts like yours are vital to that.

So yeah, just to say, unequivocally, Thanks!

[bejant]

Thanks bejant and ppemawm for these general hints. I have bookmarked them so I can reuse the link in the future.

You're welcome (I bookmarked them too).

Merely to say, explicitly, thanks @bejant

You're welcome, and as I mentioned: post a doodle of what you want to create and we'll help get you started.