Part of pad disappears when adding additional features.

[PunyTune]

I have a file with a body that is padded symmetrically from the center.
Afterwards, I have added holes both perpendicular and parallel to the pad.
But when I display the holes now, half of the pad disappears.
So, I can’t export a correct STL file.

Perhaps I have done something wrong? Is this a problem caused by applying sketches to the base shape instead of a datum plane?

The problem pad is “Top plate”

OS: macOS Sierra (10.12)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.15525 (Git)
Build type: Release
Branch: master
Hash: 1a7d3d9a37fe43468c8ac84590c1db53e2b2000a
Python version: 3.6.7
Qt version: 5.6.2
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/UnitedStates (en_US)

[openBrain]

Your file is quite complex to look at. And so to understand exactly where is the problem.
But basically you're right. If you have mapped sketches to faces of an intermediate solid that you have modified afterwards (adding extra pad/pockets), you may have broke (actually you'll almost always break) due to Topological Naming Issue.
Mapping to datum planes will make your model more robust, obviously as long as your datum planes are linked to base planes with offset & angles, and not to faces...

[HarryGeier]

I must be blind.. i don´t see that pad at all ?

2019-03-01 22_27_24-FreeCAD 0.18.png (106.46 KiB) Viewed 1220 times

i suspect you talk about something that comes in place after the base feature..not in that fcstd file
I am not sure, why you create the fusion at all, and why then go back into PD World with the base feature.
Foot and Arm i suggest are either indivdual bodies ( fuse them at mesh level later ) or combine into a single body, which for 3D print would be correct design and make all easier

Mixing PD and PART is feasible, but sometime creates awkward structures.

[PunyTune]

I must be blind.. i don´t see that pad at all ?

Oh crap. I posted the wrong file. I am so sorry.

[openBrain]

I think that your problem is otherwhere.
That's very strange that in Top plate, you successively do a Pad then a Pocket with the exact same sketch (Sketch008). Thus the Pocket just erase one half of the Pad.

[PunyTune]

That's very strange that in Top plate, you successively do a Pad then a Pocket with the exact same sketch (Sketch008).

How in that heck can that even happen? Anyway, you are right. I deleted everything but the main pad and created two datum planes for the holes, and that works. Thanks for having a look. I didn't notice that Sketch008 was used twice.

[HarryGeier]

Yes, that is the problem, sketch008 for unkinown reason is used twice, and as the pocket that it is in second feature, it cuts away itself .

If you delete the pocket, top hole works.. disregard the warning..

One thing, you should try to avoid unconstrained sketches..sketch008 is underconstrained

harry

[openBrain]

Mainly thanks to this forum, I learned that Tools -> Dependency Graph is of precious help when looking for problem causes.
And in your case, it makes it clear that Sketch008 is used twice.

dep_graph.png (36.57 KiB) Viewed 1194 times

[PunyTune]

I was interested in the Dependency Graph but was put off by the need to install both it and Homebrew and being uncomfortable with Terminal install scripts. I'm unqualified to judge if these tools put my system at risk of problems I would never understand.

[PunyTune]

HarryGeier said:

I am not sure, why you create the fusion at all, and why then go back into PD World with the base feature.
Foot and Arm i suggest are either indivdual bodies ( fuse them at mesh level later ) or combine into a single body, which for 3D print would be correct design and make all easier

The "L" shaped part was a problem for me. I first drew it as two overlapping bodies, and when summed, the STL looked okay in FreeCAD but printed incorrectly on the 3D printer. So I redrew it as two bodies that touched but did not overlap and that printed okay. I am open to advice on how to handle these sorts of situations. I needed a hole in each leg of the "L", and I wanted the ends of each leg to be semicircular. I felt that I needed to sum the bodies in FreeCAD (Fusion) to generate one STL.

You said:

Foot and Arm i suggest are either individual bodies ( fuse them at mesh level later ) or combine into a single body, which for 3D print would be correct design and make all easier

I thought that what I did was to combine them into a single body with Part Boolean Union.