Extrude shape to 3D produces strange geometry

[Cekuhnen]

Ygoe

FreeCAD cannot deal with shapes inside a sketch line two squares next to each other

It is not able to simple select both fill areas and make it one big rectangle

If you out a smaller rectangle inside a bigger it understand that you extrude a volume like a square pipe


Expressions are just another means to drive your design they can automate a lot of tasks - so nothing wrong with the sketcher but it can auto adjust sketches for yuh when you change dimensions

The other video shows a special freecad build from realthunder
Some prefer his build as it has more tools

Here is the download link

https://github.com/realthunder/FreeCAD_ ... 3/releases

Note files made in his build don’t work so good in main freecad !

[ygoe]

There are several Tees, very similar to your sketch. Three line "segments" meet at a single point.

Ah, that you mean. Yes, that becomes a problem if FreeCAD forgets about the rectangles I created with the rectangle draw tool and only remembers its edges with no further information. That probably means that I could only use a sketch for one part after another. 4 parts, 4 sketches. Or in this case at least 2 for the non-touching (opposite) parts of the frame. It's not intuitive though.

[Cekuhnen]

yeah this is a limit in how we could use sketches

here is a do and don't

sketch.png (54.86 KiB) Viewed 442 times

FreeCAD is working internally very strictly for both Part and Part Design WB - you can also see the machining philosophy in it.

For example instead of extrude join it is called pad and extrude cut it is called pocket.
In the end they do the same just broken up into a specific commands but each step then also needs its own sketch.

However here you can use expressions or project edges between sketches to make alignment of the sketches to each other easier.
Note FreeCAD struggles from features breaking when geometry was changes too much and it looses the names.

Again in the RealThunder build this is less of an issue and as long as the model is not to complex broken references can easily also be reapplied - most times.

look here: https://wiki.freecadweb.org/Topological ... h%20issues.

[Cekuhnen]

Also to put freecad into a better light

The idea of one sketch one body is technically speaking how you should work in cad too

Because when you export parts as individual files those files should only ideally have their own sketch

That’s also why assemblies or joint tools are so useful

I approach cad as a product designer and break with the flow an engineer would build the model

Different needs and use case scenarios

[ygoe]

Which leads me to the next issue. I already failed to align the frame parts with the backplane from the other sketch. How should I proceed to align the parts at each other if they're in different sketches each?

[Shalmeneser]

Sketcher_External but beware of the TNP beast
Woodcutter ! Bodies = PartDesign_SubShapeBinder

[Cekuhnen]

WARNING: Yikes Screencastify audio quality and ignoring dialog boxes - sorry I saw this only after I finished the recordings ... should have used my lecture recording hardware


NOTE: as I also state in the video this is not the ideal way you should currently work in FreeCAD but it often work but can break

How to make sketch references
https://drive.google.com/file/d/1Cyb5Kr ... TED-u/view

How to fill in the blank - here I break the video
https://drive.google.com/file/d/1rc7aWA ... kHp6c/view

Here I fix the sketch engine flip problem
https://drive.google.com/file/d/1P0D4uS ... 8q4GT/view

And here the mirror part
https://drive.google.com/file/d/1GnOjft ... B1RXf/view

Screen Shot 2021-07-23 at 4.49.03 PM.png (88.77 KiB) Viewed 405 times

[Cekuhnen]

and one design via linking dimensions

https://drive.google.com/file/d/1yb7clL ... EueCj/view

[GeneFC]

Yes, that becomes a problem if FreeCAD forgets about the rectangles I created with the rectangle draw tool and only remembers its edges with no further information.

The sketcher uses a "solver" approach to creating the final sketch. Every constraint is satisfied at the same time. There is no history of how the user drew the individual elements of the sketch. Unlike the model tree there is no order to the individual lines, circles, etc. (Yes, for the pedantic crowd there are some things for which the exact order matters, but not here.)

Again, as has already been said, the sketch is not illegal or incorrect. It just does not work as a basis for creating a solid through a pad operation because it is not clear to the pad operation what is expected.

Gene

[Cekuhnen]

not so sure about that

when you have multiple circles not overlapping and adding it to a block it works

padding multiple circles not overlapping into no contact surface would result into multiple bodies FC does not allow in Part Design WB - for philosophical/process reasons = one part one body

what either the sketcher or the modeling tools lack is the ability to select sketch profiles - currently the modeling tools are truly based on sketch edges

Part WB extrude cannot also select individual sketch elements too

I am not a coder But I assume this is more tool related than sketcher.