I have a note (annotation) in a part file that I want to configure to only show up in certain configurations via a design table.
Is this possible? How?
SW2015 Standard SP2.1
You can't control this visibility of a note with a design table, I'm afraid. Like the visibility of most other annotations, it's based on the annotation view and document settings, not the configuration.
You can make a note blank on a configuration by configuration basis if you link its text contents to a custom property and don't use a leader or border on the note
You can then drive the contents of the property with a design table and just set the value to a single space or an empty string (="")
Would that work?
Thanks for the reply John. This may work, but its not what I would call ideal.
To do this you would have to use a third party configurator addin like driveworks.
Really what I want is the user of the file to be given some extra information when a certain configuration is accessed. What is the best way to accomplish this? I don't want the user to have to find it. It needs to be in their face, so-to-speak.
Where do you want it to show, part, drawing or assembly level?
Part level. But it wouldn't matter if it showed up everywhere if the user can turn it off once they see it.
Do you use Custom Property Tab Builder?
No, we do not.
Then I would recommend you start using Tab Builder, one of the biggest documentation time savers in SolidWorks.
Custom Property Tab Builder is one of the best tools that is in the SW package, and if I ever have to use another modeling software, the Tab Builder would be missed the most.
Do some searching here on the Forum, there are many good threads regarding the Tab Builder, also it is easy to learn.
I have just setup my templates to show those custom properties when I'm in a Part or Assembly file, which will give me a quick glance dash board, however I will need to zoom in or out at times to have it shown, it would be nice if you could isolate it to a certain part of the screen.
Phil, don't know if this is quite what you want but try this.
I created a part via a design table and in one of the columns I called it $prp@"watermark". For each config I then put in the detail that I would want in the note.
Now, in you sheet template you need to put a note that is linked to the data in the part. Edit the note so it matches
I placed mine across the sheet.
From the design table above you can see I have 3 configs, 1 has no note and the other 2 have notes which are different.
Default config (no note)
1 hole config
2 hole confiq
When you change configs a Ctrl+Q rebuild is required to refresh but it does work. And you can have your note positioned somewhere specific on your sheet template, it doesn't have to be diagonal like I have it.
Hope this helps
That is also a good way to do it.
I just tried something as well, in any file add a note, however only hit the space bar a few times and then link it with a custom property, see below;
I inserted this particular note right in the assembly file and it stays showing zooming in or out, however you will need to setup a custom property for that note....
You can also apply multiple notes
Look to this:
2015 SOLIDWORKS Help - Summary of Design Table Parameters
$user_notes - with this you can control visibility of notes in part with configuration table.
Sample part attached.
I like this solution, but I have a couple of questions.
1) When I try to edit the note in your file, the functionality of the $user_notes stops working. The note is always visible. What's going on here?
2) How did you create the note so that it is linked to the $user_notes?
2015 SOLIDWORKS Help - User Notes in Design Tables
This header tells SW not to calculate the cells in this column. I'm not sure how you got that to work, but I can't repeat it or edit it.
Sorry for the confusion. It was a coincidence that this worked for me.
I have created a note and have set it to "Top annotation View". Then activated it only in one desired configuration.
Retrieving data ...