Failed to validate broken face

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shomar
Posts: 2
Joined: Fri Dec 12, 2014 3:38 am

Failed to validate broken face

Postby shomar » Fri Dec 12, 2014 3:49 am

Hi guys,

I am trying to design my first part on free cad, I get my sketch locked and fully constrained, when I try to pad the part I get a message "failed to verify broken face" and that doesn't work, so I went and verified the sketch and received a message that no missing coincidences found.

I am not sure how to fix this from this point, tried to search a lot but couldn't find a solution that works.

I am using the following freeCAD, and also attached the file with the sketch that is failing, I would appreciate if you can look at this and maybe point me on where to go from here?

OS: Mac OS X
Word size: 64-bit
Version: 0.14.3703 (Git)
Branch: releases/FreeCAD-0-14
Hash: c6edd47334a3e6f209e493773093db2b9b4f0e40
Python version: 2.7.5
Qt version: 4.8.6
Coin version: 3.1.3
SoQt version: 1.5.0
OCC version: 6.7.0

Thank you,
Shomar`
Attachments
subtractive clamp - part 1.FCStd
(41.54 KiB) Downloaded 208 times
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NormandC
Posts: 12072
Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: Failed to validate broken face

Postby NormandC » Fri Dec 12, 2014 4:24 am

Hello Shomar,

Welcome here. It is not often that newcomers make such detailed posts and supply their FreeCAD info as well as a FreeCAD file... Thank you!

I'm guessing you are talking about the sketch labeled "Clamp handle"? It is to be expected that padding it would produce such an error. Internally, when creating a Pad or Extrude, the software must first create a face out of the provided sketch, then extrude it in the 3rd dimension.

To produce a valid face, a sketch must contain a single outer closed profile, which must not be crossed by other geometry. It can contain "islands", or smaller closed profiles, but they must not cross or be tangent to the outer profile.

Your sketch does not meet this condition: the handle is attached to a full circle. You must trim the circle using the Sketcher trim tool.

I would also like to provide more pointers: your clamp handle sketch contains way, way too many dimensional constraints - this is bad practice. You should always prioritize use of geometric constraints where you can instead of dimensional constraints.

One problem is that your sketch contains only a single tangent constraint between a line segment and an arc. You should have a tangent constraint wherever an arc meets a line or another arc. I copied your "Clamp handle" sketch to a new file and edited it to show what I mean.
Attachments
Shomar_Clamp_Handle_normandc1.fcstd
(17.54 KiB) Downloaded 165 times
shomar
Posts: 2
Joined: Fri Dec 12, 2014 3:38 am

Re: Failed to validate broken face

Postby shomar » Fri Dec 12, 2014 7:18 am

Hi Normandc,

I did try to read the "before your post here" thread and tried to follow it as much as I could :)

Thank you very much for the help and the explanation, I really appreciate the opportunity to explain where I am going wrong and best practices. as I mentioned I am new to 3D design in general and your pointers are really valuable to me in my learning phase.

I have looked at the sketch you sent (really appreciate it - again- :) ) and I see your points on the dimensional constrains, I knew from the looks of it being so missy that there should be a better way, and I can see it now from your sketch. for the tangent constrains, I deleted most of these when I got conflict messages during the trial and error process I was going through, and I totally see your point.

I am really glad I got my way to using freeCAD based on the response I got here, I like being in community where help is offered this quickly and thoroughly like your answer.

Much appreciated,
Shomar`
WLudman
Posts: 2
Joined: Sun Jan 18, 2015 2:57 am

Re: Failed to validate broken face

Postby WLudman » Sun Jan 18, 2015 3:09 am

Hello:

Attached is the first part that I’ve designed in FreeCad (v0.14). The sketch is fully constrained. However, when padding the sketch, the message "failed to verify broken face" is returned. There are no missing coincidences. The trim edge tool has been used on the arcs.

Please advise as to how to resolve this problem.

Attached is my FreeCad information.

OS: Windows
Word size: 32-bit
Version: 0.14.3700 (Git)
Branch: releases/FreeCAD-0-14
Hash: 32f5aae0a64333ec8d5d160dbc46e690510c8fe1
Python version: 2.6.2
Qt version: 4.5.2
Coin version: 3.1.0
SoQt version: 1.4.1
OCC version: 6.5.1

Regards,

Wayne
Attachments
Window Jam - Jan 17 2015 - v9 - fully contstrained.FCStd
(3.22 KiB) Downloaded 91 times
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NormandC
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Joined: Sat Feb 06, 2010 9:52 pm
Location: Québec, Canada

Re: Failed to validate broken face

Postby NormandC » Sun Jan 18, 2015 6:17 am

Hello Wayne,

Welcome here, and thanks for posting such a detailed request.

Your problem is quite obvious just opening your file: your sketch may be properly constrained, but it includes an open profile. To create a face, you absolutely need a closed profile. Add a horizontal line joining both arcs at the top, and the Pad will succeed (see attached corrected file).
Attachments
Window Jam - Jan 17 2015 - v9 - fully contstrained_fixed.FCStd
(11.85 KiB) Downloaded 137 times
WLudman
Posts: 2
Joined: Sun Jan 18, 2015 2:57 am

Re: Failed to validate broken face

Postby WLudman » Sun Jan 18, 2015 9:32 pm

Normandc:

Thank you for your help.

Regards,

Wayne L.
deltaecho
Posts: 2
Joined: Sat Mar 18, 2017 6:19 pm

Re: Failed to validate broken face

Postby deltaecho » Sat Mar 18, 2017 6:24 pm

Hi everybody,
I've the same error! "Failed to validate broken face".
Can you help me please?
Thank you !!
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SupportTEL sous contraintes.FCStd
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NormandC
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Location: Québec, Canada

Re: Failed to validate broken face

Postby NormandC » Sat Mar 18, 2017 7:33 pm

Hello deltaecho,

Welcome here. To be honest it would have been better to create a new topic rather than reanimate a 2-year old one.

Your error is obvious, to create a pad, the system needs to create a face first from the sketch. But it requires a closed profile that is uninterrupted by other elements. The problem is that the circle in your sketch is whole, and two lines are connected to it. Thus this is not an uninterrupted profile. You need to trim the segment of the circle between the two lines.

The tool to do that is Image Sketcher Trimming, unfortunately it generates unexpected results when used on circles.

Here's the method I suggest.

FC_Sketcher_Trimming_Circle_01.gif
FC_Sketcher_Trimming_Circle_01.gif (413.31 KiB) Viewed 111 times


But there's another newbie mistake you're doing: you added way too many dimensional constraints. You need to learn to rely on geometric constraints more. It's bad practice to lock the X/Y position of arcs end points. You should rather ensure their tangency to the elements they are connected to with a point-on-point tangent constraint, then lock the arc centre point.
deltaecho
Posts: 2
Joined: Sat Mar 18, 2017 6:19 pm

Re: Failed to validate broken face

Postby deltaecho » Sun Mar 19, 2017 5:39 pm

Thank you so much ! very easy to correct with you video.
I've deleted some contraints too and it's always ok... i'm beginner :)
See you and thank you again.