BRep_API: command not done - When doing a thickness

[Tinkefu]

I've seen some info on this error but mostly related to fillets. In the attached file I'm just trying to do a thickness inward of 2.5 mm on faceds 33 and 17. This has worked in the past, though in the past I had built the additive loft portion first and worked from there.

How can I accomplish/fix this to end up with a hollow additive loft section with an inward thickness of 2.5mm.

Thank you.


OS: Debian GNU/Linux 9.7 (stretch)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.13541 (Git) AppImage
Build type: None
Branch: releases/FreeCAD-0-17
Hash: 9948ee4f1570df9216862a79705afb367b2c6ffb
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/UnitedStates (en_US)


Quick edit: Was reading some of the posts about this and fillets and it mentioned OCC version. I grabbed the newest appimage and tried that, same issue.

Also. I should have mentioned the thickness settings I was using are:
Face17
Face33

2.5 mm
Pipe
Arc
Make thickness inwards.

[bejant]

How can I accomplish/fix this to end up with a hollow additive loft section with an inward thickness of 2.5mm.

You can add a smaller rectangle inside the Sketches named "bottomBodyEdge" and "Sketch003" to create the void. I wasn't able to get the Part WB > Thickness tool to work either.

20190207a-MAP_Camera_V7.fcstd

(54.76 KiB) Downloaded 18 times

OS: Ubuntu 18.04.1 LTS
Word size of OS: 32-bit
Word size of FreeCAD: 32-bit
Version: 0.18.15780 (Git)
Build type: Release
Branch: master
Hash: f94e76c1116ec3b818961ff65131b3d86fa5b95e
Python version: 2.7.15rc1
Qt version: 5.9.5
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/UnitedStates (en_US)

[Tinkefu]

You can add a smaller rectangle inside the Sketches named "bottomBodyEdge" and "Sketch003" to create the void. I wasn't able to get the Part WB > Thickness tool to work either.

Thank you bejant. I had just started to do that figuring why not just pad the correct shape to begin with and skip the thickness.

I'd still be curious to know why the part design thickness tool didn't work. As in should I have just done it this way to begin with?

[openBrain]

Hi,

Below is what I get when I just recompute all your project (with a 0.18 release) :

cam.png (24.65 KiB) Viewed 645 times

All your sketches are either redundantly or over constrained. This should be corrected first.
Also I would advise to apply fillets as latest operations as it is quite sensitive.
To achieve your hallow shape, maybe it could be easier to use an additive wedge then a substractive one.

EDIT : also notice that after recomputing, face numbering is changed thus it could explain why the Thickness fails.

[Tinkefu]

Hi,

Below is what I get when I just recompute all your project (with a 0.18 release) :
cam.png

All your sketches are either redundantly or over constrained. This should be corrected first.
Also I would advise to apply fillets as latest operations as it is quite sensitive.
To achieve your hallow shape, maybe it could be easier to use an additive wedge then a substractive one.

EDIT : also notice that after recomputing, face numbering is changed thus it could explain why the Thickness fails.

Not sure I'm clear. I've opened that in .18 and have none of the issues you see. Also I'm not sure how things are over constrained?

[openBrain]

Not sure I'm clear. I've opened that in .18 and have none of the issues you see. Also I'm not sure how things are over constrained?

When I open your file, I have an error set on the Body. Thus I mark all the tree for recompute, and then after recomputing I have what I attach.
When opening the sketches, FC will tell you what are the redundant/over constraints.

EDIT : after a quick check, I confirm that your sketches have constraint issues.

[bejant]

Thank you bejant.
(snip)
I'd still be curious to know why the part design thickness tool didn't work.

You're welcome. I could do a Thickness selecting the top face but not when selecting both the top and bottom faces; the bottom face always remained. I did get some "Links go out of allowed scope" (I think that was the warning) in the Report view. Maybe setting the Property > Refine (from the Data tab) to True on the previous Features would help the Thickness tool work but I haven't tried that.

EDIT : also notice that after recomputing, face numbering is changed thus it could explain why the Thickness fails.

I didn't have what is shown in your image happen to me using 0.18; did you change your Edit > Preferences > Part Design > Automatically Refine settings?

Not sure I'm clear. I've opened that in .18 and have none of the issues you see. Also I'm not sure how things are over constrained?

In the history tree, look for a white exclamation point in a red circle to the left of your sketch names, or open the sketches and look at the Solve Messages and you'll see. Are you sure you used 0.18?

When I open your file, I have an error set on the Body. Thus I mark all the tree for recompute, and then after recomputing I have what I attach.
When opening the sketches, FC will tell you what are the redundant/over constraints.

EDIT : after a quick check, I confirm that your sketches have constraint issues.

Same results here.

[openBrain]

EDIT : also notice that after recomputing, face numbering is changed thus it could explain why the Thickness fails.

I didn't have what is shown in your image happen to me using 0.18; did you change your Edit > Preferences > Part Design > Automatically Refine settings?

I never changed this kind of settings. But I indeed get a different behavior on my other PC (which has a slightly different build).

To come back to OP, I guess that Thickness is broken due to the first Pads in the tree. As inside a body each step creates a new complete solid, I guess the Thickness isn't easy to proceed on the final solid (maybe even not possible).
I can achieve a result (that I think is the expected one) by changing the order in which functions are used.
The file is attached. I used "Copy sketch geometry" feature as well as "Reference to external geometry". Sketches are properly fully constrained. The fillets have been done inside the sketch, which I guess is more suitable for a robust design. Robustness isn't fully ideal as I mapped a sketch directly to a face but that was mainly for quickness purpose.

[Tinkefu]

I think I understand most of what has been said here.

The only part I'm not clear on is the over constraint portion. I only constrain until I have 0 degrees left. I'm not sure what I'm doing wrong? I try to follow the guidelines I've read. Less is better, use symmetry etc.

[openBrain]

A simple example is with Sketch003 of your original file.
On the toppest line, you add a symmetry constraint between the 2 endpoints relatively to the Y (vertical) axis.
Geometrically it imposes that this line is horizontal (because it's an axial symmetry vs. a vertical line). Thus the horizontal constraint of this same line (which probably comes from the rectangle primitive) is redundant and shall be removed.
I'll try another example with another of your sketch but they are quite complex to explain.