We have a pretty high number of Help Forum entries concerning sketches that cannot be padded. The message says “Failed to Validate Broken Face”, which is not immediately understandable for everyone.
Since the reasons are manyfold it is not always the same answer to be given, but a dedicated wiki page might help. That could be linked in the common questions.
This topic is about the contents of such a page. Perhaps it will result in some kind of a best practices page.
Make sure the sketch is closed. Use the Validation tool.
Use Sketcher Polyline
Don’t put too much in a sketch.
NormandC hase made some general recommendations on how complex a sketch might be. And there is the 7-7-7 rule which comes from the Creo world and sure has to be adapted to FreeCAD but the idea is still valid. It says a sketch should contain either no more then 7 elements or 7 measures or take no more than 7 minutes. The last one is for newbies of course hardt to meet.
Control the degrees of freedom (DOF) and don’t overconstrain a sketch, e.g. with a horizontal or vertical symmetry constraint on a rectangle. It would be preferred if the sketcher could check it, but currently he doesn’t.
The previous point could be extended to how many DOFs are consumed by which constraint, e.g. horizontal/vertical: 1, coincidence: 2, tangent line/line: 1, tangent point/line: 2, tangent point/point: 3, …
I haven’t seen this view on sketches before but it helps constraining.
Basically it should be good to created “standard answers” to common questions in something like the WIKI Pages.. this help us and the users a lot :
1: Newbies can read the answers before even asking
2: We can point askers to the pages
3: Efforts to describe Problem solutions only need to be done once
4: These solutions can be translated
Well , if they do not.. they will ask..and will be pointed there ( if applicable).. we do this at work with the ticket systems FAQ pages since years..
and ONCE pointed to.. they will probably bookmark and re-use next time ..
Surely, if they search..they would find a lot of other pages with solutions.. but that is not the point , it´s for those who do not find a proper solutions around the search engines and ask here.. to have a valid , clear and repeately usable answer..
i once was active on a forum in thingiverse.. there , daily we had the same 4 newbie questions.. no one would have looked and/or searched before and we had to write the same blablabla over and over..
We had the same situation here, remember the questions about exports missing their pockets or not being able to move a sketch? Their occurrence has dropped significantly since it is mentioned in forum rules.
There’s already the FAQ, linked in the forum rules. But it’s so huge and has so many different topics, it may be best to make geometry problems separate.
I was originally thinking about adding it to the PartDesign wb page but it’s quite long already. A dedicated page may be best.
Don’t forget the validation tool is not fully reliable, there are many conflicting constraints it cannot find.
More stuff: there should be no intersecting geometry, unless they are construction. Explain that multiple “islands” in a larger closed profile is OK, a circle inside a circle inside a circle (3 levels) is not. Show this with pictures.
I’m travelling all day and half the night and hope my laptop has enough power to work on this. Actually the laptop has not my preferred OS, but I bought it due to its long lasting battery.
It was luxury combined with nightmare: both seats beside me were free, but a baby was crying all night. Now I’m afraid that deep inside me there exists a baby killer.
Back to FreeCAD: I reached nothing here, had to repair a postprocessor instead.
When adding dimensional constraints, take care with selection of points so that the extension lines don’t overlap the geometry. Move away the dimensional constraints from the geometry so that it remains clearly visible. Avoid extension lines crossing dimension lines from other constraints. This might seem superfluous but it’s worth spending the time. It will be easier to have a general view of the complete sketch.
And that piece of advice can then be put to good use in TechDraw.
It baffles me that people seemingly create dimensional constraints and leave them as they are. After 15 or 20 such constraints all overlapping the geometry, the sketch becomes a big white and red blob.
I understand that with abdullah’s new virtual space, you can hide all constraints with a button click. But it remains that if you need to troubleshoot constraints, you need them to be visible. And you’re back to the white and red blob.
Check that you don’t have two elements overlapping each other. Use the Elements list in the Tasks panel and cycling through the elements one by one; this highlights them in the 3D view. When you find the overlapping element, select it and delete it.
I always invest considerable time in arranging the dimensions, the drawback being different scales. Depending on the zoom level it is sensible to have the dimensions in different places.
Where we come back to the recommendation not to “draw” the whole complex outline in ONE sketch and extrude at once, which is an obvious reaon for lots of dim constraints.