Failed to validate broken face

[cfuttrup]

I'm very new to FreeCAD and struggling a bit with the basics.
I have seen the first three tutorial videos, which were very helpful.
I hope it's OK to reuse this thread again.
My sketch is fully constrained, but I get the "Failed to validate broken face" and honestly, I can't see it.
I can't follow the 777 rule because I'm using elliptical arcs (need 5 constraints), but yes, the design is symmetric around the y-axis.

OS: Windows 10 (1909)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.4 (GitTag)
Build type: Release
Branch: releases/FreeCAD-0-18
Hash: 980bf9060e28555fecd9e3462f68ca74007b70f8
Python version: 3.6.6
Qt version: 5.6.2
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: Danish/Denmark (da_DK)

Any tips?

Thank you,
Claus

[kisolre]

Hello and welcome to the forum

Sketcher WB/Sketch/Validate Sketch show some missing coincidences. In order to use sketch for pad.pocket operations it has to contain closed wires - collections of edges. Having all edges fully constrained does not imply that they are connected. Since the solver approximates a solution instead of solving it if no coincidence between edge ends is specified they could become quite close together but not actually overlap and cause an error in pad/pocket.

[drmacro]

I'm very new to FreeCAD and struggling a bit with the basics.
I have seen the first three tutorial videos, which were very helpful.

Any tips?

Thank you,
Claus

Since you ask for tips...

When things are symmetrical you can avoid a lot of messy looking and confusing dimensional constraints by sketching half of the object. Then use mirror.

(Oh, and mentioned, there were vertexes that weren't closed.)

Cabinet1.png (64.75 KiB) Viewed 792 times

[SarahEckholdt]

Hey,

I have some kind of similar problem when trying to revolute my figure. I've already used the SketchValidation, but somehow the Body keeps having the error of tip shape is empyt (must be executed) after using the Revolution with the constant error of failed to validate broken face. I tried changing the way I create my figure but nothing helps. I've used the program a few times and searched through the forum to find something similar with a solution but without luck :-/

[chrisb]

Hi and welcome to the forum!

Remove the block constraints. Having a sketch fully constrained is of no avail in itself. We recommend to do it, because it makes you keeping control.

0mm constraints should always be replaced by geometric constraints.

[drmacro]

Hey,

I have some kind of similar problem when trying to revolute my figure. I've already used the SketchValidation, but somehow the Body keeps having the error of tip shape is empyt (must be executed) after using the Revolution with the constant error of failed to validate broken face. I tried changing the way I create my figure but nothing helps. I've used the program a few times and searched through the forum to find something similar with a solution but without luck :-/

In addition to what others have noted.

One trick I use to avoid missing coincident vertices (the cause of non-closed shape errors), before applying any dimensional constraints, I attempt to move all connected lines. If any of the ends come apart, I fix that, then forge ahead with dimensional constraints. If you've already applied some, you can also right click on the constraint in the Constraints list window and deactivate them while trying to find the culprit vertices.

Also, unless you have a particular need for a Block constraint, it's probably best not used. If you just want to fully constrain but don't care about the value of the coordinate, Lock constrain is probably a better option. (Beware, this could cause a problem if the sketch looses it support (See Topological naming for details. The sketch may remain fully constrained or not, but, can also can have strange results when the solver now sees the constraint in the wrong direction because the reference has been lost. In fact, this is possible with any dimensional constraint.)

A tip: if you use Polyline to draw a shape, you only need to close the final vertex to the first. I typically just end the line and then apply a coincidence to them, thus no question whether it is closed. Then add dimensional constraints.

Another tip. If you use the geometric shape tools and over lap, say a square and a hexagon, to approximate your desired shape, then use the trim tool to shape the final shape and delete the excess lines, the vertexes created by the trim tool will be created coincident. Again, less likely to miss a coincidence.

Can you tell I like "belt and suspender" engineering?

[SarahEckholdt]

This have been a big help, thank you very much both of you I'll probably never use Block Constraint again

[TheMarkster]

This have been a big help, thank you very much both of you I'll probably never use Block Constraint again

They're mostly useful as temporary constraints to hold bits in place as you manipulate other bits. I think some people like to use them with bsplines, too.