Hi all
I want to show some properties of a part in an assembly. I don't know if it's possible. Does anyone have an idea?
Thank you in advance for your answers.
Hello
Yes, it is possible if you use an annotation (note) and it is "hung" on the piece in question.
A video tutorial (1€) explains all the possibilities here: http://www.lynkoa.com/tutos/th%C3%A9matiques-avanc%C3%A9es-propri%C3%A9t%C3%A9s
Thank you for your answer.
The problem is that I would like to make it appear as a property of my assembly.
That is to say, to create a Ø Bore property in my assembly and tell it that it is equal to the Ø Exterior property of my part.
I don't know if it's very clear..................;
You are very clear in your second message.
Indeed, directly in the custom properties of a SolidWorks assembly, it is not possible to take dimensions of a part or subassembly.
So you have to go through a macro, or better, a utility like SmartProperties
I use smartproperties but I haven't found a way to display the properties of a part in the properties of an assembly!
ha, you're right...
Indeed, it is in the drawing of an assembly that it can be done, or in a mechanically welded file.
I could have sworn I saw it in a van...
I'm going to see if we can't do it through APIs...
Ok, thank you very much for your answers.
I'm also going to continue to look on my side...
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
assemblage1.zip
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it works with Mickael's workaround (what a cunning one) ;-)
Hello
Thank you for your research. It's an interesting solution but we have more than 5000 references as head assemblies and which contain about 15 parts. Redoing a sketch with each new head assembly would be too tedious...
Thank you again for your help. I continue my research...
Hello
Also think about the document template (asmdot) in which you can already have a sketch, an equation and a property pointing to the dimension of this sketch (method described by the cunning mickael!). The same goes for the part template (.prtdot). That way you always use the same information and every time you need to make a part or assembly you don't have to create that information anymore.
Kind regards
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There is no solution!!!