"failed to validate broken face" when making new pocket

[jp2112]

I'm trying to make my first 3d layout with FreeCAD using sketches and pads/pockets (I followed the Basic Part Design tutorial and it appeared easy enough) so all was going well with my simple enclosure design until I wanted to add two more pockets onto a side face, in similar manner as two previous pockets. I created a new sketch then mapped it to a face, but when using the pocket tool and entering the dimension I get the dreaded "failed to validate broken face" error. I have not found an identical forum help thread on this, please help me figure out how to make these pockets.
The attached jpg file shows the sketch that has the geometry I want to cut out of the 2mm side wall, and I've attached the design file.
I read on this forum that zero distance constraints are problematic, so I changed the two that I had (used by the rectangular pocket sketches) to be point-object coincident constraints but it didn't solve this error.
Thanks

OS: Windows 7
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.15.4671 (Git)
Branch: releases/FreeCAD-0-15
Hash: 244b3aef360841646cbfe80a1b225c8b39c8380c
Python version: 2.7.8
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17

[ektus]

there are two problems with your model:


1) It is forked. Sketch001, Pad001, Sketch005 and Pocket001 must be deleted. Then change change "Pocket" to "depth: 75mm"

2) The sketch for the key slots is invalid. See attachment for corrected version. The horizontal lines must be converted to construction geometry (displayed in blue) and the circles must be replaced with arcs.

There is no need to manually mapping a sketch to a face. In part design, simply select a face and then start your new sketch. Also, make sure only the very last feature in the combo view is toggled visible.

Regards
Ektus.

[quick61]

I have a bit different take. First, the model is not forked, but 2 separate models. This can be easily fixed with a Fusion between Pocket001 and Pocket004. (Pocket004 is the result of Pocketing Sketch008)

Second, there is a slot tool in sketcher that can be used for the slotted holes.

Using that tool and a much more reasonable constraint scheme, including the removal the 0.0 distance constraints which often lead to trouble, are never necessary, and IMO should never be used, one can come up with a sketch like this -

SlotSketch.png (13.22 KiB) Viewed 2451 times

enc_Fused.fcstd

(40.45 KiB) Downloaded 30 times

Mark

OS: Kubuntu 14.04.2 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.15.4671 (Git)
Branch: releases/FreeCAD-0-15
Hash: 244b3aef360841646cbfe80a1b225c8b39c8380c
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17

[jp2112]

Thanks Mark and Ektus for quick responses. Because I needed to keep that end cap with round pocket, I'm going to continue with Mark's updated design file. I apologize for ignoring my own comment about not having any zero dimensions--I made those slots as rectangles first then decided later that I better round them, without thinking about what I was doing! But now I know the slot tool is better (is there a general rule against overlapping sketch geometry?)

Also, I searched in the help about Fusion and saw nothing. How did you do that? and what are the repercussions for not doing that? The stl file I exported as a test gave no clue that it would be a problem.
It's not apparent to me why pocket001 needs to be fused with pocket004 (i.e. why not pads and why not the other pockets) in order for the tool to be happy with my two separate but connected pad models. Can you explain so I can recognize when this needs to be done in the future?

Final question on the new pocket004, did you simply accept the default or was there a reason for making it 5mm in dimension?

A sharing of gratitude--my little world of amateur 3d cad design is so much better owing to people such as yourselves who are so generous with their time! I'm guessing no big-time $ tool would have this level of support (i.e. instantaneous). I received the same terrific experience with gnuplot forum, too. But I speak to the choir, right?
JP

[quick61]

Thanks Mark and Ektus for quick responses. Because I needed to keep that end cap with round pocket, I'm going to continue with Mark's updated design file. I apologize for ignoring my own comment about not having any zero dimensions--I made those slots as rectangles first then decided later that I better round them, without thinking about what I was doing! But now I know the slot tool is better (is there a general rule against overlapping sketch geometry?)

Also, I searched in the help about Fusion and saw nothing. How did you do that? and what are the repercussions for not doing that? The stl file I exported as a test gave no clue that it would be a problem.
It's not apparent to me why pocket001 needs to be fused with pocket004 (i.e. why not pads and why not the other pockets) in order for the tool to be happy with my two separate but connected pad models. Can you explain so I can recognize when this needs to be done in the future?

Part Fuse The bottom and sides appeared to be intended as a single part. Fusing the 2 parts make a new single part so any further features or Boolean operations will be applied to the single new part and not one or the other. I suspect that when you exported the model to STL, you selected both parts, which made them a single mesh in the export. If you would of only selected one or the other, that is all that would of been exported. In the scheme of things, maybe to you it would not matter for this project, but best practices would be to have a single part be a single part and not 2 or more sub parts. Assemblies are made up of 2 or more single parts. Make any sense?

Final question on the new pocket004, did you simply accept the default or was there a reason for making it 5mm in dimension?

I was in a hurry and the default got it done. I could of just as easily made it Up to face, but there is a minor bug in 0.15.4671 release with the up to face and it might not of come out the way it was intended.

A sharing of gratitude--my little world of amateur 3d cad design is so much better owing to people such as yourselves who are so generous with their time! I'm guessing no big-time $ tool would have this level of support (i.e. instantaneous). I received the same terrific experience with gnuplot forum, too. But I speak to the choir, right?
JP

This forum is a pretty good place to get quick help. It's one of the things that make FreeCAD such a great program to learn and use.

Mark

[jp2112]

For the record I just found the tool for performing a fusion, it's under Parts workbench->"make a union" button.
This feature will in fact help me on the mating enclosure cap part I'm doing next.
Thanks again.
JP