Sheet metal bend angle callout on drawing

[Mandrake22]

An offshore vendor has converted a large batch of our old drawings to Solidworks models and drawings. They have linked the bend angles on the model to the drawing but I can't figure a "streamlined" way to do this. On our drawings, the bend is described like this: "Bend Up 95°". To the end of the initial note which reads "Bend Up" they have added: "D4@FlatBend1@12345E.Sldprt". The "12345E" is a theoretical file name. The fact that the drawing now is fully associative with the model is great but I am looking for something easier than typing this string for every bend.
I can find no evidence of "automated" property linkage going on.
If all else fails, I will have to ask them how they did it but I thought a challenge to the group would be the place to start.

 

[SBaugh]

Are there Equations in the file...That's what comes to my mind from your description. You would see them in the FM tree if there are some.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[TheTick]

what they may have done was bring the bend angle into the drawing using "Insert-->Model Items", used the inserted dimension for selecting and linking to a note, and then delete the inserted dimension.

An alternative would be to link the dimension to a custom property in the part file, and then using the custom property in a note. I find this works well for chamfer and slot callouts.

Also, whenever I use a parameter in a property or equation, I rename it. Here is why:

http://www.eng-tips.com/faqs.cfm?spid=559&sfid=590

There's no double-lock defense; there's no chain on my door.
And I'm available for consultation,
but remember your way in is also my way out

 

[MadMango]

They might have just linked the dims to the note. When you create a note, you can type your text, then click on any dimension to insert that value. Once that is done, you can hide the dimension. Now if you change your part the note will update accordingly.

We do this all the time with countersink and counterbored holes, mostly because *Gollum voice* we hates the Hole Wizard annotations, we do.

Wanna Tip? faq731-376
"Probable impossibilities are to be preferred to improbable possibilities."

 

[TheTick]

One more possibility:

The bend angle dimension was inserted using "Insert--> Model Items" and the additional text was just appended to that dimension.

You may want to do a quick "litmus test" to see if the annotation is a model or a note. Set the selection filter to pick only dimensions, and tru to select the bend note. Try the same with the selection filter set to only notes.

 

[Mandrake22]

Thanks for the responses guys.
No, there are no equations.
"Insert Model Items" doesn't bring in the bend angle dimensions so there is nothing to "click on".
There is no custom property in the part file although that would be something I will consider using in the future..
The callout is a note and not a dimension. Dimension filtering doesn't allow it to be selected.
It looks like they have manually entered the text.
Thanks again.

 

[TheTick]

I still stand by my recommendation to use a property instead of linking the dimension directly. It helps avoid issues if there are any file name changes in the future. One less thing to catch in the "Where used" column.