Hello
Is it possible to retrieve the contents of a custom property of a part from a custom property of an assembly?
Kind regards
propriete_piece_vers_assemblage.png
propriete_piece_vers_assemblage.png
Hello
It is possible to display it in the drawing, but not directly in the properties. It will be possible with a macro, but you need knowledge of VBA and to run the macro every time.
Edit: for more precision, in an annotation in a drawing of an assembly, you can choose that it displays the properties of the part to which it is attached.
A topic in English:
https://forum.solidworks.com/thread/68312
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Good morning,
yes, just click on the 1st line and press Shift and the last one, then do CTRL-C and go into the room and press CTRL-V. And if you want it for all the time, you do it in an empty room and save it in PRTDOT and there every time you create a room you will have these custom properties
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an answer was given by @ Mickael
On this communication thread it is true that it is a workaround but it can be useful ;-)
http://www.lynkoa.org/forum/solidworks/remonter-proprietes-d-piece-assemblage
Hello
I think we can make it simpler, if I understand the final goal correctly (simply retrieve a value of the part in a property of the assembly)
You can already create a "Bore diameter" property in the part and select the dimension to retrieve the value.
From the assembly, you have to make a sketch at the assembly level on one of the standard planes, a circle for example, and add a dimension to it.
We then need to add an equation at the level of the assembly, we will say that the dimension we have just created is equal to the dimension of the diameter of the bore of the part.
We will then enter a property at the assembly level which says that the value of a "Bore diameter" property is the dimension of the sketch created in the assembly.
The sketch of the assembly can then be hidden.
A Ctrl + Q is required at the assembly level to update the value of the property.
I enclose an example.
Have a nice day
Mickael
to try ;-)
Yes, it is possible even if the syntax is laborious:
In the assembly property you enter:
For example, if you want to recover the material "SW-Material@@Nom configuration@Nom piece. SLDPRT"
We use this on our mechanically welded assemblies.
In practice, you can recover any property (or dimension) of a room.
The only problem is that this property doesn't update itself (if you change the part in the assembly for example you continue to refer to the value of the ownership of the first part)
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Thank you froussel its corresponds to what I wish I have left to do more than to implement it with this technique is it possible to recover the tolerance also of a dimension in a sketch?
Retrieving a dimension in properties is super simple:
You go to your properties on the test you want to edit, just double click on the 3d to bring up the desired dimension, and you select it. SW fills the property with the right syntax (makes it easy to put the throughput in the properties for example).
Retrieving the tolerance must be possible since I did it under excel part family: a column named $TOLERANCE@h@Plan1 drives the tolerance of the h dimension (which defines plan 1)
On the other hand, if we enter this beginning of syntax in the properties (in front of the name of the dimension) it doesn't work. So the syntax must be slightly different in the properties.