Part imported into Assembly not as saved part.

[un1corn]

OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.16110 (Git)
Build type: Release
Branch: (HEAD detached at upstream/releases/FreeCAD-0-18)
Hash: f7dccfaa909e5b9da26bf50c4a22ccca9bb10c40
Python version: 3.6.6
Qt version: 5.6.2
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/UnitedKingdom (en_GB)

I hope I can get advice on where I am going wrong, I am still struggling with V0.18 in particular Datum plane and shape binders, also when importing parts into an assembly.

The attached screenshot shows (on the left) the saved part. The part imported (on the right) into a assembly as can be seen the flange trim pad and the dome inner form although removed from the saved part are not so in the part imported to an assembly.
In V0.16 I did not have this problem as can be seen in some of my user showcase posts.
I attach the part file also.
Comments appreciated people.
Thanks.

[openBrain]

At first if you look at the dependency graph, you'll see that your file as lot of errors of "go out of allowed scope" type.
This should be corrected.
Basically you can either use the Bodies instead of their internal functions to achieve the Part boolean functions. Or use the boolean function provided in the Part Design WB.
Then actually what you see in the assembly is just your file. Just all top level objects are visible. This is (I guess, didn't try on your file) a consequence of the previous issue.
Once your building tree will be clean of errors, everything should be OK.

[openBrain]

It was actually quickly fixed.
Attached your modified file (I just didn't redo the fillet, up to you).
If I guess right, it should import well in assembly now.

[un1corn]

Many thanks 'openBrain' for taking the time to read, react and rectify my post.
I had intended to attach the PDF of the part drawing of the Steam dome which I have now included in the event anyone is interested.
In truth I had many problems trying to download Graphviz but have now managed to install and use the Dependency graph however I do not know how to interpret the errors let alone correct them.
I am unable to find information on how to use the Dependency graph within FreeCAD and the info' I have found seems to show how create graphs only.
If yourself or anyone else can point me to useful info on the use etc of the Dependency graph and what the errors mean I would be very grateful.
Thanks again for your help.

[Willem]

In my opinion this dome is best to be constructed in the sketcher workbench and the part workbench and because there are a lot of boolean operations that are hard or not to do in the part design workbench I prefer not to use the part design workbench this time. One of the main rules in Freecad is to make the construction without fillets and do all fillets as the last operation. When I did this I saw that I did not get the thickness of 3 mm that is requiested. To solve this problem I constructed the outside of the Dome and later I did the same dome 3 mm smaller and did a boolean cut on it

Schermafdruk van 2019-06-22 15-21-58.png (160.91 KiB) Viewed 395 times

[un1corn]

Thanks for your advice 'Willem' I will certainly try your suggestion.
I am finding V0.18 difficult to use, probably an age thing..........(75)
Regards.

[Willem]

However I tried also to do this in Part design workbench and it also works with the Part design boolean operation

[openBrain]

Many thanks 'openBrain' for taking the time to read, react and rectify my post.
I had intended to attach the PDF of the part drawing of the Steam dome which I have now included in the event anyone is interested.
In truth I had many problems trying to download Graphviz but have now managed to install and use the Dependency graph however I do not know how to interpret the errors let alone correct them.
I am unable to find information on how to use the Dependency graph within FreeCAD and the info' I have found seems to show how create graphs only.
If yourself or anyone else can point me to useful info on the use etc of the Dependency graph and what the errors mean I would be very grateful.
Thanks again for your help.

Actually displaying the Dependency graph is one thing, understanding the errors in it is indeed another.
I guess you can't understand it without previously understanding the underlying concepts of FreeCAD.
In the present case, this is the known PartDesign vs. Part workflow.
Mixing both has to be avoided but sometimes you can't. The important here is that Part tools use "solids" for its operations. And PartDesign actually creates only one solid, which is the "Body". The items inside a Body are only "functions" that lead to the Body.
So if you want to perform a Part operation (eg. a boolean cut), it shall be done between 2 solid objects, i.e. a 2 Bodies, or a Body and a Part feature, ... But in no case the operation shall be performed with a function inside a Body.

[un1corn]

Thank you 'openBrain' for the information, I have a little better understanding of the Dependency graph now.

Thank you 'Willem' for your help, I did note however that the bottom radius is incorrect (should be 72.55mm) and would not mate with the boiler shell. probably caused by the flange fillet causing a misshape.

Following the guidance from you both I was able to rework by changing the 75.5mm Rad to 96.6mm and offsetting the Z axis to help compensate for the flange radius, I have achieved a reasonable flange shape. which appears agreeable to the Dependency graph.
Thanks again both.