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Is it possible to link Custom Property value from the Part/Assembly, to the Custom Property Table of the Drawing?
Categories: Drawings and Detailing
If you mean under File > Properties for Drawing, then there is no direct way. You'll have to use a macro to update that. And every time properties are changed in model, you need to re run the macro to updated drawing properties.
If I understand your post correctly, I was able to assign a custom drawing property to the value of a custom part property.
It auto updates with a drawing reload, a Ctrl+B or a Ctrl+Q. No macro necessary.
Part1 is an extrude with the extrude length equal to the part custom property "length".
In the Part1 drawing, custom property "dwglength" refers to $PRPSHEET:"length"
In the drawing's properties dialog, the evaluated value quotes this text, but as you can see on the drawing, the actual part "length" value displays correctly in the note.
The note is hard text left of "=" and a link to "dwglength" right of "=".
I hope this solves your issue.
Yes I can link annotations to custom properties. but what I want was part custom properties to be linked to drawing custom property. this looks like it is not possible.
So the $PRPSHEET:"length" value in the drawing does not get evaulated.
How about linking an annotation or note to the drawing custom property? Is that possible?
The OP was from part to drawing, but I don't think it's possible to go from drawing to part (w/o Deepak's macro suggestion).
Drawings don't have equations, so linked equations are out.
Even though the part-to-drawing properties don't evaluate tin the dialog box, they do evaluate when linked to notes, etc.
Other than for displaying them on the drawing (which is possible), what's your requirement for these properties?
For your question "How about linking an annotation or note to the drawing custom property? Is that possible?":
If you mean an annotation in the drawing from the part, then yes (that's what Part1 is doing).
If you mean an annotation in the part from the drawing, then no, I don't think so. I don't think there are any "$" secret codes for parts/assemblies to snatch properties from the drawing.
Anyhow, good luck with it.
I was able to link the weight (mass) from the custom properties of a part to the custom properties in the drawing.
For instance, our PDM will show the weight property of an item stored in the library.
I went to the custom properties of the part and copied the mass property.
And pasted that into the drawing custom property.
Is this what you are looking for?
It makes no sense at all that Solidworks does not support this kind of parameter sharing. The means there is no way to synchronize properties between a model and a drawing. So the Custom Property in a drawing called "Description" can and will be different than one in the referenced model called "Description". Why does this matter, well for one thing the drawing property "Description" shows in the file open menu and helps you to find the right drawing.
This does not enable you to set it up in a template so that the relationship already exists and automatically updates.
It's not exactly automatic (or maybe it is), but you can use the custom properties tab builder get the values you want from the model to the drawing. We have scenarios where we begin a part with our own part numbering/naming conventions, but then change over to the clients conventions. So we use some radio buttons to switch. We also bring in some other generic parameters with a simple text box as such as the Status box at the bottom of the examples below. Not sure it's the best way, but it works.
John, I've been doing 3D design since it had to be done with wireframe in 1985. You shouldn't make assumptions. What I am trying to do is exactly what you said: drive data from the part to the model. I want the Description property in the part to transfer to the drawing properties. Not just to the title block, to the drawing properties. Then it could be shown in both the title block and in the file properties.
I'll investigate this functionality. Looks like a viable solution, but it does seem like an unnecessary extra step.
Check if solution by Joseph shared here https://forum.solidworks.com/message/498509#comment-498509 works for you?