multiple views from same prospective

[efferre]

I have the following design:

with.png (11.57 KiB) Viewed 1827 times

without.png (12.42 KiB) Viewed 1827 times

and I am preparing the drawing using TechDraw. The two pictures differs from a cover part which is hidden in the second picture.

I would like to show two top views with and without the cover at the same time to put in evidence the inner channel but as soon as I create the second view also the first one is updated. Is there a way to avoid keeping a view linked with the original 3D?

I am using latest FreeCAD version from repository

[wandererfan]

I would like to show two top views with and without the cover at the same time to put in evidence the inner channel but as soon as I create the second view also the first one is updated. Is there a way to avoid keeping a view linked with the original 3D?

You'll get better answers if you post the FCStd file.

I'm guessing this is an assembly of some sort? if it is, you can select just the pieces you want in the drawing as the Source objects.

[efferre]

Here is attached the file. It's a step file provided by a supplier and imported into FreeCAD.

What I do is the following:

• I select the tab with the 3D design and define the left view so that the assembly is shown from the top
• I press the "Insert default Page" button from TechDraw toolbar
• I select the master object Fiber-A-Protection_assembly and then press the "Insert a view" button from the TechDraw toolbar
• I toggle the visibility of Fiber-tubing_A_cover object and select again Fiber-A-Protection_assembly
• I press the "Insert a view" button from the TechDraw toolbar

In the drawing page I can see now two views as expected, like this:

drawing.png (18.28 KiB) Viewed 1797 times

If I press the "redraw page" button, the first view is updated and becomes identical to the second one. I hope it's clear.

[wandererfan]

[*] I toggle the visibility of Fiber-tubing_A_cover object and select again Fiber-A-Protection_assembly

Visibility in the 3D window isn't considered in determining what gets printed. It's an interesting approach though.

To print the whole assembly, select the whole assembly as the source. To print only parts of the assembly, just select those parts.

portA_visibility_partials.png (49.34 KiB) Viewed 1769 times

[efferre]

Visibility in the 3D window isn't considered in determining what gets printed. It's an interesting approach though.

actually the visibility has some effect as described above but it's not what the user expects was able to destroy a drawing when playing with my experiments, most of the quotes and dimensions were lost, I'll post again if I find a procedure to reproduce the problem

To print the whole assembly, select the whole assembly as the source.

yes I confirm that works, thanks

[wandererfan]

actually the visibility has some effect as described above but it's not what the user expects

Not what the programmer expects either. Something somewhere is "doing us a favour".

[vocx]

... most of the quotes and dimensions were lost, I'll post again if I find a procedure to reproduce the problem

This sounds like the topological naming problem. Essentially, TechDraw dimensions (TechDraw_Dimension_Length) depend on the names of the edges in the 3D model. If you change the 3D model, the dimensions in TechDraw may break because the edges are renamed. Therefore, you should only add your dimensions as the last step, when the model is not subject to change any more.

[efferre]

This sounds like the topological naming problem. Essentially, TechDraw dimensions (TechDraw_Dimension_Length) depend on the names of the edges in the 3D model. If you change the 3D model, the dimensions in TechDraw may break because the edges are renamed. Therefore, you should only add your dimensions as the last step, when the model is not subject to change any more.

No, I didn't change anything in the 3D model. I'll post back if I am able to reproduce the problem.

[efferre]

Today I have found a minor issue, when exporting the front view I get an extra point in the drawing which is not available in the 3D model, see the picture here (I am starting from the freecad file attached above):

front_view.png (20.49 KiB) Viewed 1679 times

[wandererfan]

Today I have found a minor issue, when exporting the front view I get an extra point in the drawing which is not available in the 3D model, see the picture here (I am starting from the freecad file attached above):

There are a bunch of geometry errors in the file, notably "Fiber-Protection-flange_EDFA". See the short lines near the left end.

portA_GeometryErrors.png (221.32 KiB) Viewed 1650 times

Geometry errors confuse the Hidden Line Removal algorithms in OCC. We don't have a general solution for detecting and correcting this situation automatically. It usually happens with assemblies and/or STEP imports.

You can often trick HLR by changing the Direction property of the View by a tiny bit.

HLRTrickery.png (100.86 KiB) Viewed 1650 times