Attaching Note to Dimension 1

[McDesign25]

Is there a way to attach a note to a dimension, and have the note follow with the dimension if it moves? I am thinking about adding inspection points to a dimension with a triangular border, and if the size of the part changes later, I want the note to stay with the dimension, not get stranded out in space. The functionality I want is how the Geometric Feature Control Frame moves with the dimension when it is moved. What do you do for inspection dimensions, do you use a quote?

Thanks.

 

[TheTick]

I have tried unsuccessfully to do something similar. So far, the best thing has been to put the unattached note adjacent to the dimension, while making sure the note "belongs" to the same view as the dimension. Then, at least the note will move with the view.

You can associate a note to a view in a number of ways:
1.) select (right click) the view and "lock view focus" before the note is created
2.) attach the note to the model with a leader, an then turn the leader off. This works well if you want to change a note's association from one view or sheet to another view.

You may want to put "paired" notes and dimensions on a special layer with a unique color, in order to more readily spot notes that have become separated from their dimension "partners". Gravity is a harsh mistress.

 

[SBaugh]

Have guys not tried to edit the properties of the Dimension and select "Modify text"? Because from there you can add text or a "note text" to the dimension and it will directly attached to the dim.

Best Regards, Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[TheTick]

yeeeesss.

In my case, it was trying to associate text that has a circular or triangular border, which we use to identify notation references, revisions, and key characteristics. I have not found a way to do this by modifying the dimension text. Gravity is a harsh mistress.

 

[TheTick]

Back in my Unigraphics days, I actually wrote a custom pallette of symbols which could be inserted into text the same way one can insert symbols in SW text (in the same manner as "plus-minus" and "centerline" symbols).

Is there a way to make custom symbols like this in SW?

Gravity is a harsh mistress.

 

[McDesign25]

Scott,

TheTick is right, I want to be able to put a triangular border around the numbered note, so that it appears to jump out at the 'non-technical' people inspecting/viewing the drawing. You can RMB the dimension and 'show as an inspection' but this does not work to our satisfaction. It merely puts a oval pattern around the dimension. Also, We would really want the note to embed into the dimension like the Geometric Feature Control Frame does.

Thanks for your suggestions...

 

[macPT]

Have you considered in create special symbols to identify a control note?

Edit the file gtol.sym and follow the instructions to create your symbols. But it's not an easy task because it's not wysiwyg (a lot of trial and error).

Regards

 

[macPT]

Before you start to change things in the gtol.sym file, make a backup of the original. If there's some sintax error in that file, SW will not start.

You can also visit

http://solidworks.cad.de/

for more details.

Regards

 

[TheTick]

zoweeee!

Thanks, MacPT! It's gonna take a little experimenting, but it's definitely along the lines of what I was looking for.

BTW--if the next guy to open a drawing doesn't have my custom symbols in his library, will he still see them? Do they get embedded into the drawing file once they are used? Gravity is a harsh mistress.

 

[macPT]

You must copy the new file to all users. The symbol is not embebed in the drawing.
You must be careful with upgrades. They can overwrite the file.
The best way is to have a text file with your simbols and with a significant name. In case of overwriting (for example if you install sw2003 over sw2001+) just copy the contents of your file into gtol.sym.
If you share drawings with costumers or vendors, you must provide them your file.

Thanks for the star! Is good to be helpful!

Regards