Using shell on an extruded spline fails

[Wink Saville]

I'm unable to shell a wing created with a spline based airfoil file. I get

the error "Null TopoDS_Shape object", here is the file, nwing.py:

(cqgui-master) wink:~/prgs/CadQuery/projects/wing4 (master)

$ python nwing.py 

Traceback (most recent call last):

  File "nwing.py", line 30, in <module>

    halfWingShell = halfWing.shell(-0.1)

  File "/opt/anaconda/envs/cqgui-master/lib/python3.7/site-packages/cadquery/cq.py", line 1123, in shell

    s = solidRef.shell(faces, thickness)

  File "/opt/anaconda/envs/cqgui-master/lib/python3.7/site-packages/cadquery/occ_impl/shapes.py", line 1630, in shell

    s1 = self.__class__(shell_builder.Shape()).Shells()[0].wrapped

  File "/opt/anaconda/envs/cqgui-master/lib/python3.7/site-packages/cadquery/occ_impl/shapes.py", line 312, in __init__

    self.wrapped = downcast(obj)

  File "/opt/anaconda/envs/cqgui-master/lib/python3.7/site-packages/cadquery/occ_impl/shapes.py", line 286, in downcast

    f_downcast: Any = downcast_LUT[shapetype(obj)]

  File "/opt/anaconda/envs/cqgui-master/lib/python3.7/site-packages/cadquery/occ_impl/shapes.py", line 276, in shapetype

    raise ValueError("Null TopoDS_Shape object")

ValueError: Null TopoDS_Shape object

If I use an ellipse, ewing.py, it works:

 (cqgui-master) wink:~/prgs/CadQuery/projects/wing4 (master)

 $ python ewing.py 

[Jeremy Wright]

I can get it to work if I select one of the X faces and use a positive shell value.

halfWingShell = halfWing.faces("<X").shell(0.1)

[Wink Saville]

Yep, I just tried it and it did work when using `halfWingShell = halfWing.faces("<X").shell(0.1)`.

But get the error below with -0.1,  `halfWingShell = halfWing.faces("<X").shell(-0.1)`:

(cqgui-master) wink@3900x:~/prgs/CadQuery/projects/wing4 (master)

$ python nwing.py
Traceback (most recent call last):

  File "nwing.py", line 31, in <module>
    halfWingShell = halfWing.faces("<X").shell(-0.1)

  File "/opt/anaconda/envs/cqgui-master/lib/python3.7/site-packages/cadquery/cq.py", line 1123, in shell
    s = solidRef.shell(faces, thickness)

  File "/opt/anaconda/envs/cqgui-master/lib/python3.7/site-packages/cadquery/occ_impl/shapes.py", line 1622, in shell
    rv = shell_builder.Shape()
OCP.StdFail.StdFail_NotDone: BRep_API: command not done

I now notice the trailing edge looks funny even without the shell but looks fine if "fattenTe" is NOT used.

Although even without "fattenTe" it still fails as above with not only -0.1 but also -0.01 and -0.001. So the problem

doesn't seem directly related to using "fattenTe".

I'll investigate the trailing edge problem and report back tomorrow.

Good night/Good morning :)

--
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[Jeremy Wright]

> BRep_API: command not done

Yeah, I dread that error. It usually means it's a kernel problem and doesn't give you any information for tracking it down. Adam might have an idea on what the problem is, but I'm not sure. As a work-around, offset2D was recently merged. You could try to offset the spline inward and then extrude the inner and outer profiles as a shell. No guarantee, but it might work for you. https://github.com/CadQuery/cadquery/pull/397

I notice the weird rendering artifacts in CQ-editor. I'm not sure if the exported mesh would have those same artifacts or not.

[Wink Saville]

I've looked at the trailing edge problem using nwing.py, below, from my cq-wing4 repo.

(cqgui-master) wink:~/prgs/CadQuery/projects/wing4 (master)

$ cat nwing.py

from naca5305 import naca5305

from scale import scaleListOfTuple

from fattenTe import fattenTe

import cadquery as cq # type: ignore

chord: float = 50 

h = 100

# Normalize, Scale, fattenTe

scaleFactor = 1/naca5305[0][0]

nNaca5305 = scaleListOfTuple(naca5305, scaleFactor)

sNaca5305 = scaleListOfTuple(nNaca5305, chord)

#fNaca5305 = fattenTe(sNaca5305, 0.25, 10)

fNaca5305 = sNaca5305

# Create the 2D airfoil then extrude

airfoil = cq.Workplane("YZ").spline(fNaca5305).close()

halfWing = airfoil.extrude(h)

# Shell the halfWing

halfWingShell = halfWing.shell(0.1)

show_object(halfWingShell)

#show_object(halfWing)

I've taken some screen shots, the first one, halfWingShell-nrmlTe-shell_+0.1-yAxis-3.png

shows the "normal trailing edge" with a "full" positive shell and it looks "clean":

But if you look at the "fattened trailing edge" you can see a big "notch" and and other "divits":

So fundementally the fattenTe logic seems to generating a contigious trailing edge

although the simple interpolation isn't the smoothest it's weird it would causes the

discontinuities we see along the trailing edge. Here are pics of the 2D airfoil for both

normal and fattened:

Normal:

Fattened:

Actually with a fattening of 1 you can see a small ridge on the top because I assume the

points are equally distributed. Maybe that's part of the problem?

I'll keep looking, but wanted to post what I've learned so far.

[Adam Urbanczyk]

It seems that you reached some kind of limit of the CAD kernel. Here are some  ideas:

(1) If you have the exact function that describes your profile you can try if parametricCurve and higher number of points would help.

(2) If you know the tangents at every point you could also use those, possible making the spline more well-behaved

(3) The other option, as Jeremy mentioned, is to try offset2D.

[Wink Saville]

So I've done some experiments with ellipses which are "kinda-like-airfoils". Since they can't be done well, it's no wonder my airfoils don't do well. So I think I'll try the `offset2D` suggestion from Jeremy.

The reason for choosing that is in general the airfoil can be many different shapes and in most cases not computable. Although, in actual fact, the one I'm trying now, naca5305, could probably be turned into a "parametricCurve", but since shell can't handle ellipses well, I don't have much hope it could handle something that is round on one end and very very thin on the other.

Actually, I may have to handle the entire wing my self. Along those lines, I'm wondering, if I use "wires" or "edges" can I create manifolds of "arbitrary" shapes?

[Jeremy Wright]

This WIP PR might be of interest to you: https://github.com/CadQuery/cadquery/pull/406

With that you might be able to define your airfoil profile as a DXF, import that, then extrude it. It probably won't fix the shelling issue, but would give you some extra flexibility on how you create the outer and inner profiles of the airfoil.

[Wink Saville]

That is very interesting, I've subscribed to them so I can follow along, txs.

[Wink Saville]

In repo cq-offset2DvsShell I explore the two commands, and indeed

offset2D does work in cases where shell doesn't.

My explanation for this is that if the number of vertices for the "inner"

object is not equal to the number of vertices in the outer object you

get a `ValueError`.

I could be totally wrong, but that is my guess.

This intformation, with the "actual" reason it fails, might be useful

addition to the documentation. Be glad to add it if there is an appropriate

place for this type of information in the documentation.

[Adam Urbanczyk]

The offset algo does not work (yet) with self-intersections (see https://www.opencascade.com/doc/occt-7.4.0/refman/html/class_b_rep_offset_a_p_i___make_thick_solid.html#a96e66fd6d047d844eb6f261b86e0a9a5 ) and that is why you saw weird result for offsets >minor radius on an ellipse. I don't think though that is is the same issue for the simple object you linked above.

[Wink Saville]

Could defintely be two different problems.

One other note, my son-in-law has SolidWorks and its shell command

was able to produce reasonable results for both the simple "airfoil" with

the thick trailing edge and the ellipse.

[Adam Urbanczyk]

If I set the Intersection arg to true (see link above) your example works. SolidWorks has no relation to CQ (i.e. different CAD kernel), so I'm not sure how it is supposed to help.

[Wink Saville]

On Wednesday, July 22, 2020 at 12:57:48 PM UTC-7 Adam Urbanczyk wrote:

If I set the Intersection arg to true (see link above) your example works. SolidWorks has no relation to CQ (i.e. different CAD kernel), so I'm not sure how it is supposed to help.

I've probably done something wrong, I changed "def shell" in shapes.py

to set Intersection to True and it didn't make any difference for me. As for

SolidWorks, it was just a check to see if it was valid on other platorms, for

all I knew it was totally invalid.

I also needed to change increase the "Deviation" by 10x, to be at least "0.0001",

in 3DViewer preferences, otherwise cq-editor didn't finish within a few minutes.

As you can see in the screenshot I was using "Deviation=0.01" the these tests.

Here is the shapes.py diff:

(cq-dev4) wink@3900x:~/prgs/CadQuery/forks/cadquery (master)

$ git diff

diff --git a/cadquery/occ_impl/shapes.py b/cadquery/occ_impl/shapes.py

index c26889d..7f33f41 100644

--- a/cadquery/occ_impl/shapes.py

+++ b/cadquery/occ_impl/shapes.py

@@ -1677,20 +1677,23 @@ class Mixin3D(object):

 

         occ_faces_list = TopTools_ListOfShape()

 

+        intersection=True

         if faceList:

+            print(f'shapes.shell with faceList, Intersection={intersection}')

             for f in faceList:

                 occ_faces_list.Append(f.wrapped)

 

             shell_builder = BRepOffsetAPI_MakeThickSolid(

-                self.wrapped, occ_faces_list, thickness, tolerance

+                self.wrapped, occ_faces_list, thickness, tolerance, Intersection=intersection

             )

 

             shell_builder.Build()

             rv = shell_builder.Shape()

 

         else:  # if no faces provided a watertight solid will be constructed

+            print(f'shapes.shell NO faceList, Intersection={intersection}')

             shell_builder = BRepOffsetAPI_MakeThickSolid(

-                self.wrapped, occ_faces_list, thickness, tolerance

+                self.wrapped, occ_faces_list, thickness, tolerance, Intersection=intersection

             )

 

             shell_builder.Build()

Here is the output at the terminal:

(cq-dev4) wink@3900x:~/prgs/CadQuery/projects/shellellipse (master)

$ cq-editor shellellipse.py 

Namespace(filename='shellellipse.py')

TKOpenGl | Type: Other | ID: 0 | Severity: Medium | Message:

  OpenGl_Window::CreateWindow: window Visual is incomplete: no stencil buffer

Font_FontMgr, warning: unable to find font 'Courier' [regular]; 'Cantarell' [aspects: regular,bold] [paths: /usr/share/fonts/cantarell/Cantarell-Regular.otf;/usr/share/fonts/cantarell/Cantarell-Bold.otf] is used instead

shapes.shell with faceList, Intersection=True

(cq-dev4) wink@3900x:~/prgs/CadQuery/projects/shellellipse (master)

$ cq-editor shellellipse.py 

Namespace(filename='shellellipse.py')

TKOpenGl | Type: Other | ID: 0 | Severity: Medium | Message:

  OpenGl_Window::CreateWindow: window Visual is incomplete: no stencil buffer

Font_FontMgr, warning: unable to find font 'Courier' [regular]; 'Cantarell' [aspects: regular,bold] [paths: /usr/share/fonts/cantarell/Cantarell-Regular.otf;/usr/share/fonts/cantarell/Cantarell-Bold.otf] is used instead

shapes.shell with faceList, Intersection=False

And here a screen shot, it is the same whether I left the code unchanged or

set intersection to True or False:

[Jeremy Wright]

@Wink I wondered if there's maybe some things you could gather from this article for your work with airfoils. https://hackaday.com/2020/08/14/quick-3d-printed-airfoils-with-these-openscad-helpers/

[Wink Saville]

Txs for the info!

[Adam Urbanczyk]

This looks relevant too: https://github.com/chiefenne/PyAero . Especially the "airfoil splining and refining" part.

Op zaterdag 22 augustus 2020 om 23:11:20 UTC+2 schreef Wink Saville:

[Wink Saville]

Very nice, txs.