TechDraw not updating with parametric length

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Giuliano1969
Posts: 31
Joined: Wed Jan 16, 2019 10:15 pm

TechDraw not updating with parametric length

Post by Giuliano1969 »

I created a furniture with parametric values (length, height, depth...) . See attached file.


BUT if I change the parameters, the 3D solid changes are NOT reflected into the 2D TechDraw drawings.
The 2D techdraw keeps the old initial values, as the it was created.

Is this behavior supposed to be right ?
Any workaround ?
Attachments
TD error.FCStd
(119.91 KiB) Downloaded 54 times
chrisb
Veteran
Posts: 53919
Joined: Tue Mar 17, 2015 9:14 am

Re: TechDraw not updating with parametric length

Post by chrisb »

Please be more specific. The TechDraw page updates correctly if I change "Larghezza" from 0.5m to 0.6m.
And please note that this is an English forum, so not everyone knows what things like "Larghezza" or "lunghezza tacco" mean.
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mendy
Posts: 262
Joined: Mon May 21, 2018 2:16 pm

Re: TechDraw not updating with parametric length

Post by mendy »

Thanks @chrisb. I didn't know what it meant. Tried file and works here.

OS: Ubuntu 20.04.2 LTS (MATE/mate)
Word size of FreeCAD: 64-bit
Version: 0.20.24910 (Git) AppImage
Build type: Release
Branch: master
Hash: 089b2ae47824232f649eb74ce1f97673cf77b78c
Python version: 3.9.4
Qt version: 5.12.9
Coin version: 4.0.0
OCC version: 7.5.2
Locale: English/United States (en_US)

Screenshot of possible places to look. Had slightly different issue that was solved with help from @Roy_043
In my case wrong setting was corrupting page till refresh. All well now. Pardon inches in spreadsheet, my units are set to imperial decimal.
Attachments
td.jpg
td.jpg (558.87 KiB) Viewed 2172 times
Giuliano1969
Posts: 31
Joined: Wed Jan 16, 2019 10:15 pm

Re: TechDraw not updating with parametric length

Post by Giuliano1969 »

@mendy , @chrisb,
thanks for your kind replies.

I’m astonished…. Now It works… I’m without words…. Sorry for the inconvenient, and thanks for your help.

TWO more questions:
1-You can see I’ve added two sweeps, that are correctly displayed into the 3D.
BUT they are NOT present in the TD 2D.
What I’m missing to let them appear into the TD page ?

2-If I try to save the TD in dxf, the dimensions appears with the unit of measure (m), but NOT with the values....
Has it something to do with parametric config ?

BR
Giuliano
mendy
Posts: 262
Joined: Mon May 21, 2018 2:16 pm

Re: TechDraw not updating with parametric length

Post by mendy »

1:
You set the view in 3D window. Then select Body and with ctrl key select Sweep and Sweep001 and then Insert a View. Think you are looking at 3D but not selecting the Sweeps to send to page. Works here just arbitrary views.

2:
No clue know next to nothing about DXF.
Attachments
sweeponpage.jpg
sweeponpage.jpg (61.18 KiB) Viewed 2094 times
Giuliano1969
Posts: 31
Joined: Wed Jan 16, 2019 10:15 pm

Re: TechDraw not updating with parametric length

Post by Giuliano1969 »

Thanks Mandy.
If I set some dimensions in Freecad, and then export the drawing in dxf, this is what I found in the dxf.
Seems that dimensions values are lost.
Even more strange, when trying to set dimensions in QCAD, the size of the object seems completely different !!
Is there something to set as a scale, when exporting to dxf in Techdraw ?
The 0.18m become 3.56 ?!?


Image
Attachments
tderror.dxf
(28.96 KiB) Downloaded 55 times
Schermata del 2021-05-25 23-33-43.png
Schermata del 2021-05-25 23-33-43.png (22.22 KiB) Viewed 2039 times
Schermata del 2021-05-25 23-31-39.png
Schermata del 2021-05-25 23-31-39.png (56.12 KiB) Viewed 2039 times
domad
Veteran
Posts: 2051
Joined: Mon Jun 22, 2020 12:16 pm

Re: TechDraw not updating with parametric length

Post by domad »

Giuliano1969 wrote: Mon May 24, 2021 9:32 pm .............
Is this behavior supposed to be right ?
Any workaround ?
Greetings to the Community, hello Giuliano1969!

You could have previewed the topic in the Italian forum, then eventually in the general or specific ones in English. (take it as advice for the future)
In addition to what chrisb and mendy suggested.
After having checked the workflow of your file and having found a non-compliant modeling method, I proceeded to recreate it by following, let's say, a more “suitable or adequate” one.
The reconstructed file is almost completely parameterized by interfacing with the "Spreadsheet" tool or workbench (I tried to keep your parameters).
The components of the object (I think shop furniture) are all separate bodies, in fact the "bodies" created with "Part Design" must be understood as unique, monolithic not assemblies of bodies.
An assembly of bodies, which in reality are detached, "forced" into a single unit or body, due to a common or adjacent face, is an inappropriate way of designing / modeling, as it will be subject to problems of topological redefinition/renaming.
In addition, a very long structure of functions will inevitably be generated that will significantly slow down the updating of changes, also and especially in "TechDraw", as well as subject the processors to strong "stress".
On the other hand, a design / modeling of separate bodies will considerably limit (possibly completely eliminating them) the problems mentioned above, making the recalculation and visualization much more fluid, also being able to intervene very easily to make even radical changes (elimination of the body or part ).
This is the applied workflow (not the only one [!], FC also allows you to model correctly by applying other flows through the use of other workbenches also in synergy):
- creation of separate bodies with "PartDesign"
- creation of links and / or groups of links for identical bodies - creation of references in "Spreadsheet" for editing parameters (assembly and modeling)
- creation of an assembly assembly in "Assembly", in this case 3 (this is the default one), which in this case had the sole task of acting as a "container for the various bodies" (however it can be used to set assembly constraints)
- creation of the technical drawing quoted in "TechDraw" of the assembly.

Now it is possible to intervene through the controls in "Spreadsheet" to modify the geometry or the position of the various bodies, this will be reflected immediately and correctly on the rendering of the 3D view, on the technical drawing and on the dimensions in "TechDraw".

Obviously these changes must be "relevant" that is not "oversized" otherwise errors will be produced in particular in "TechDraw".

I hope I was useful, attached the revised file, a greeting.
Attachments
no_TD error.FCStd
(101.41 KiB) Downloaded 50 times
1.png
1.png (167.63 KiB) Viewed 1943 times
2.png
2.png (162.67 KiB) Viewed 1943 times
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