The created drawing is not visible

[pnagy]

I created a part with part design and a drawing with TechDraw. I saved the file but when I open them I see only the 3D geometry. In other cases, both the Page and 3D geometry open in two separate windows. If I create another new drawing, a new window will open. If I click the original Page (this contains the created draw) the program shows the 3D geometry. How can I reach or modify my old drawing on "Page"?
I used Freeecad 0.17 on Windows 7.


Any idea? I attached the part.

camera_tarto.FCStd

(58.02 KiB) Downloaded 33 times

[jmaustpc]

In other cases, both the Page and 3D geometry open in two separate windows.

that is how it is supposed to work.

If I create another new drawing, a new window will open.

taht is also what is supposed to happen.

I used Freeecad 0.17 on Windows 7.
[/quote
Please post your version data in the manner explained in the Forum Rules link above this forum. It provides us much more information.

By the way both your FreeCAD and your O/S are obsolete or are about to be. install FreeCAD 0.18.1 and see if you problems go away. There are something like 3000 feature updates and bug fixes.

I'll look at your file and come back.

[jmaustpc]

I get the following error messages on opening your file.

If you go to FreeCAD preferences and select send error messages to report view and turn on Report view, then you will see the following

Code: Select all

Rebuilding Views for: Page/Page
Lines are parallel
Lines are parallel
Lines are parallel
Lines are parallel
Lines are parallel
Lines are parallel
Dimension Dimension004 missing Reference to 3D model. Must be Projected.
Dimension Dimension004 missing Reference to 3D model. Must be Projected.
Dimension Dimension004 missing Reference to 3D model. Must be Projected.
Dimension Dimension004 missing Reference to 3D model. Must be Projected.
Dimension Dimension004 missing Reference to 3D model. Must be Projected.
Dimension Dimension004 missing Reference to 3D model. Must be Projected.
Dimension Dimension004 missing Reference to 3D model. Must be Projected.
Rebuilding Views for: Page/Page
Exception (Tue Apr 23 20:53:56 2019): getIndexFromName - empty geometry name  
Traceback (most recent call last):
  File "<string>", line 1, in <module>
<class 'OSError'>: getIndexFromName - empty geometry name

If I right click on "Page" and select "Show Drawing" I get the following error message

Code: Select all

Unhandled Base::Exception caught in GUIApplication::notify.
The error message is: getIndexFromName - empty geometry name
Unhandled Base::Exception caught in GUIApplication::notify.
The error message is: getIndexFromName - empty geometry name

OS: Ubuntu 18.04.2 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-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/Australia (en_AU)

[jmaustpc]

If I try to delete the drawing it crashes FreeCAD.

Any crash bug is a bug, so....if its not a quick fix, I'll create a bug tracker ticket. Thank you for reporting this.

ping

do you want a ticket?

Jim

[jmaustpc]

here is your file, partially recovered, it has no techdraw drawing, you have to do that again, but I extracted you solid, so at least you won't have to start all over again. Finish the solid first then create the drawing, I have read that the "topological naming" limitation can corrupt a techdraw drawing.

camera_tarto_recovered.FCStd

(51.77 KiB) Downloaded 23 times

[kisolre]

On another note you should avoid mapping sketches to faces because of that "topological naming" issues. It already broke here:
.

Pocket_Face17.JPG (113.26 KiB) Viewed 2603 times

Pad001_MappingToFace17.JPG (100.63 KiB) Viewed 2603 times

.
See how Face17 changed to the cylindrical side of the hole and the mapping of the next sketch failed.

[pnagy]

Thank both of you for the help and quick answers!

[wandererfan]

do you want a ticket?

Yes please. Dimension003 has no references to the drawing geometry. This causes all sorts of trouble since recomputing Dimension003 fails.

I would have thought it was impossible to create such a dimension without using Python (badly).

So there are really 2 problems to solve here:
- prevent a crash when there is garbage in the model
- prevent garbage from being created.

[jmaustpc]

Bug tracker ticket created.
issue #3944

[wandererfan]

Bug tracker ticket created.
issue #3944

git commit ede3bd2210 should fix the crash.

Was there anything unusual about Dimension003? Was the underlying geometry changed after Dimension003 was created? Dimensions without references aren't supposed to happen.

I made up references for Dimension003 to repair the file. You'll want to delete and re-add it with the right end points.