TechDraw Dimension Link - No dimensions appearing in dialog?

[benjaminwharton]

Apologies if this has been posted about before, but I've done some searching and haven't found the exact thing I'm looking for.

I'm trying to show correct dimensions in TechDraw using the dimension link tool as explained here, except when I try to create the link no dimensions appear in the dialog.

I'm doing the following steps:

• Open Freecad 0.18
• Click "create new empty document"
• Open the Part workbench
• Click "create a cube solid"
• Set the view to isometric.
• Open the TechDraw workbench.
• Click "insert new default page"
• Select the cube in the tree view
• Click "insert view in page"
• Select the top and top left vertices (top left edge)
• Click "insert new length dimension" (and drag the resulting dimension text away a bit so it's more visible). At this point the dimension lines/text appear although not with the correct length (I realise this is normal)
• Go back to the 3D view and select the top left edge
• Click "link a dimension to 3D geometry"

And this is what I get:

nodimensions.jpg (186.65 KiB) Viewed 1360 times

OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.15938 (Git)
Build type: Release
Branch: master
Hash: acdd4b097bbaf6d94bc09cf38f25924bd5d3e778
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: French/France (fr_FR)

[openBrain]

Hi,

I remember I also had troubles with that.
If I'm correct from what you explain, I think that you should go back to drawing display ("Page" tab) before clicking "link a dimension to 3D geometry".

EDIT : I just checked and I guess this is the actual problem you have.

EDIT2 : after completing the link, you have to recompute to update the displayed dimensions.

[Syres]

I'm doing the following steps:

• Open Freecad 0.18
• Click "create new empty document"
• Open the Part workbench
• Click "create a cube solid"
• Set the view to isometric.
• Open the TechDraw workbench.
• Click "insert new default page"
• Select the cube in the tree view
• Click "insert view in page"
• Select the top and top left vertices (top left edge)
• Click "insert new length dimension" (and drag the resulting dimension text away a bit so it's more visible). At this point the dimension lines/text appear although not with the correct length (I realise this is normal)
• Go back to the 3D view and select the top left edge
• Click "link a dimension to 3D geometry"

I followed your steps exactly and confirm that method produces the same for me but, replacing tbese steps:

• Select the top and top left vertices (top left edge)
• Click "insert new length dimension" (and drag the resulting dimension text away a bit so it's more visible). At this point the dimension lines/text appear although not with the correct length (I realise this is normal)
• Go back to the 3D view and select the top left edge
• Click "link a dimension to 3D geometry"

with

• Select the top and top left vertices (top left edge)
• Click "insert new length dimension" (and drag the resulting dimension text away a bit so it's more visible). At this point the dimension lines/text appear although not with the correct length (I realise this is normal)
• Go back to the 3D view and select the top and top left vertices
• Click "link a dimension to 3D geometry"

shows Dimension in the Available box.

So in summary, if you select an edge in the Techdraw view for the dimension, you must select an edge in the 3D view but if you select two vertices in the Techdraw view for the dimension you must select two vertices in the 3D view.

OS: Windows 7
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.15959 (Git)
Build type: Release
Branch: master
Hash: 397418078a6f61e8c39cedfe1160adc2abd73510
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)

[Willem]

This works correct in my version, under the tab "Available" I get a list of dimensions I can change.
OS: Ubuntu 18.04.2 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.15860 (Git)
Build type: Release
Branch: master
Hash: 3b708c7f84b0425076b520e1d95627b20fd75fe0
Python version: 2.7.15rc1
Qt version: 5.9.5
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: Dutch/Netherlands (nl_NL)

[benjaminwharton]

Thanks for the helpful responses.

So in summary, if you select an edge in the Techdraw view for the dimension, you must select an edge in the 3D view but if you select two vertices in the Techdraw view for the dimension you must select two vertices in the 3D view.

Ah, I can't believe I didn't realise I was making the mistake of mixing up elements even after typing out my steps here. Thanks, that was the issue.

If anyone with edit permissions wants to note this on the TechDraw Dimension Link wiki page I'm sure it'd help a few people like me.

[openBrain]

I would notwithstanding advise a (IMO more robust) workflow.
By modifying your final steps as is :

• Click "insert new length dimension" (and drag the resulting dimension text away a bit so it's more visible). At this point the dimension lines/text appear although not with the correct length (I realise this is normal)
• Deselect all
• Go back to the 3D view and select the top left edge
• Go back to the TechDraw page then Click "link a dimension to 3D geometry"

With that way, you'll be proposed with all the dimensions of the drawing and you can choose the right one (or even several of them). A pity is that selected dimension is not highlighted, thus with a complex drawing, you'll have to rename the dimensions with clear names and/or to temporarily switch to the "Model" tab of Combo view to check the right item.

[wandererfan]

If anyone with edit permissions wants to note this on the TechDraw Dimension Link wiki page I'm sure it'd help a few people like me.

Done.

"Note that if the Dimension to be linked is based on two vertices, you should select two vertices in the 3D view. Similarly if the Dimension is based on an edge, you should select an edge in the 3D view. "