Cutting walled cylinders intersection

[markp]

I am trying to cut the intersection of two 2mm wall tubes. But the result have these extra "faces" (idk how they are called), it doesn't look like a clean cut:



I attached the file I am working with, before the cut. To do the cut I expand the parts "Heat Riser" and "Feeder" on the tree view from Model, holding CTRL, I select "heat riser tube" first, then "feeder tube" and click "Part > Join > Cutout from object". Then I do the same but selecting "feeder tube" first and "heat riser tube" last. And the result is the above image.

Is this normal or am I doing something wrong?

OS: Windows 7
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.16117 (Git)
Build type: Release
Branch: releases/FreeCAD-0-18
Hash: dbb4cc6415bac848a294f03b80f65e888d531742
Python version: 3.6.6
Qt version: 5.6.2
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/UnitedStates (en_US)

[meme2704]

Hi
The sketches of the tubes are not constrained, they only need a few microns of difference to see this defect

[chrisb]

Things like this happen rather frequently if you perform boolean operations on coplanar faces or - as seen here - with tubes of the same diameter.

Furthermore it helps us helping if you minimize the model to a state where nothing irrelevant to show the problem is contained.

[markp]

Adding the same contrains to both tubes (48mm inner wall, 50 outter wall) gave me the same result. What seems to work is making outter wall of the 45 degrees tube 49.8mm instead of 50mm:



Is there any other trick to make this without modifying the tube size? It doesn't feel like the right way to do it.

[chrisb]

There's no other way, and it cannot be fixed in FreeCAD as it comes from the 3rd party geometry kernel. Usually you can make the difference even smaller, but I can very well understand that you feel uncomfortable, any difference, albeit extremely small is not equal.

[bejant]

I am trying to cut the intersection of two 2mm wall tubes. But the result have these extra "faces"
...snip...
Is this normal or am I doing something wrong?

I think that the unwanted residual faces in your image are because the two Sketches used to make the tubes aren't Fully Constrained, and not Fully Constraining them is bad practice.

Even so, after they are Fully Constrained, there are still tiny arc-like residuals that remain. This time I think they are only a display issue which happens because FreeCAD tessellates model objects displayed in the 3D view, and so the model is actually correct but is not precisely displayed on the screen. To test this, after making the Cutout, you can make another solid half-tube with an inside diameter of 100 mm and an outer diameter of something like 110 mm, enclosing the half of the vertical tube away from the angled "feeder tube":

20190612b.png (30.01 KiB) Viewed 1221 times

Do a Part WB > Boolean Intersection between this new tube and the Cutout. For me there is nothing in the resulting Common, and if this issue was actually some residual edge in the model instead of something more than a display problem I would expect that there be at least two remnants of those residual edges contained in Common.

OS: Ubuntu 18.04.2 LTS
Word size of OS: 32-bit
Word size of FreeCAD: 32-bit
Version: 0.18.1.
Build type: Release
Python version: 3.6.7
Qt version: 5.9.5
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/UnitedStates (en_US)

[chrisb]

I can confirm bejants observation and to add to it: Geometry check including BOPCheck doesn't show any errors,

There is more to say about your model: You have many repititions in your sketches where you well could use Expressions or Sketcher CarbonCopy