Is it possible to link Custom Property value from the Part/Assembly, to the Custom Property Table of the Drawing?
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?
I'm trying to accomplish the same thing as Rolland, i.e., I need the custom properties table on the drawing to grab the info from the custom properties table on the model. Although using $PRPSHEET:"part number" works on the title block of the drawing, it doesn't seem to work on the custom properties table on the drawing, since the evaluated value remains $PRPSHEET:"part number" instead of the actual part number, and therefore our PDM can't read it. I tried using the properties tab builder like you suggested, but I get the same results: the evaluated value remains $PRPSHEET:"part number".
Interestingly enough, If I use $PRPSHEET:"part number" on the custom properties table on the drawing and $PRP:"part number" on a note on the same drawing, the note updates correctly with the part number, which tells me that somehow internally the custom properties table on the drawing is indeed grabbing the info from the model, but for whatever reason is not showing it on the evaluated value column. I need it to show on the evaluated value. Any ideas? I'm using SW 2014 SP 5.0.
for the way you want it to work, you will need to copy the custom property from the part to the drawing rather than link it. You can use a macro to do that, there's a discussion here with an example Copy Part Custom properties to drawing custom property
OK, thank you!
See the following solution from the VAR Portal.
Why would you want them to be linked?
You can already reference model properties in the drawing files for annotations, title block info, etc. so why would you need that info linked to drawing properties?
Model description property populates our title block part title...
Where you ever able to get the Description variable of the part data card to transfer to the drawing card?
Here you go.
To get to this follow provided steps:
1. Type "LENGTH" in the Property Name column.
2. Select "Text" in the Type column.
3. Back out of Properties Menu.
4.Get into "Manage Equations" by right-clicking.
5. Add the Feature by selecting "add feature suppression" features row in the name column, then clicking in the part or assembly.
6. Under the Value/Equation column select "Measure"; a prompt will show to select what to measure.
7. Close the Manage Equations menu, go to the back into the Properties and select the "length" Value / Text Expression drop down and there will now be a linked annotation to select.
Please let me know if you have any further question.
Is there a real solution to this problem yet? I am currently using Solidworks 2018 and I really need the mass of the model to evaluate in a custom property in the drawing. I need it to adapt to a drawing template where it automatically updates according to the model defined in the sheet properties. I really don't want to have to run a macro every time, as that would defeat the purpose of having it set up in a template. I would be open to a macro attached to the template that will automatically run every time the document is saved or the sheet model is updated. I am not a programmer, however, and I am not very good at writing macros without a lot of help and searching the forums for examples of what I'm trying to do.
Like Evan Dlugopolski above, I'm curious about why anyone needs this functionality. If it's just to call it out in a Note, that can be done directly instead of adding the extra step in the middle.
Type this into your Sheet Template
We use an equation in our standard Part and Assembly Templates to make a global variable called RoundedMass, which converts the mass into kg and to the correct number of decimal places,
then assign it to a Custom Property called DrawingMass.
We then show the Drawing_Mass property on the standard drawing formats.
Al of this happens automatically, without user intervention.
It does mean that we sometimes need to modify the equation particularly if the part weighs less than 100g, but, otherwise, it works quite well.
The problem is that SW_Mass evaluates in g, not kg, hence all the jumping through hoops. That may be the way we have our Part Template set up, but that's the way it is...
Please don't make assumptions as to why someone might need what they are looking for. I've been using Solidworks for 15 years and I am quite familiar with the ability to reference the part properties in a note in the title block. This about having the custom property in the drawing evaluate correctly so that it matches the model. I need it to work automatically in a template and the evaluated value in the custom property to show the mass of the model for export to an excel document.
Dallas Havens wrote: I need it to work automatically in a template and the evaluated value in the custom property to show the mass of the model for export to an excel document.
Dallas Havens wrote:
I need it to work automatically in a template and the evaluated value in the custom property to show the mass of the model for export to an excel document.
In SW there is nothing Automatic, without first manually hitting Rebuild, unless there is a Macro that would rebuild at closing the file etc...
Dallas Havens wrote: Please don't make assumptions as to why someone might need what they are looking for. I've been using Solidworks for 15 years and I am quite familiar with the ability to reference the part properties in a note in the title block. This about having the custom property in the drawing evaluate correctly so that it matches the model. I need it to work automatically in a template and the evaluated value in the custom property to show the mass of the model for export to an excel document.
Dallas Havens wrote:
I didn't make any assumptions, and I realize this is about having a Drawing property linked to a model property. I was just curious about why someone would need that.
Retrieving data ...