GD&T and other symbols show #error: broken link when library note is dragged into a drawing. 1

[APPENG]

Good afternoon,

I have created a library of parametric notes for my designers to use when creating the detail drawings.

These notes contain the usual text, links to custom properties & special properties. They also have GD&T frames, And surface finish symbols.
Everything works except for the symbols and GD&T
When I drag in the notes, the GD&T frame is not there. In its place there is text that says "#error: broken link"

This is what I created:

https://files.engineering.com/getfi...e98-bce8-6a07211e8f30&file=Supposed_to_be.JPG

Here is what I get when I drag it into the drawing:

https://files.engineering.com/getfi...37-4739-be5e-05607f90af0e&file=What_i_get.JPG

Anyone else having this problem?

Regards,
Jon

 

[APPENG]

Just an update here:

I recreated the note and this time instead of using cut and paste, I created it all manually and added the GD&T frames plus the surface finish symbols again.
I create a new Style in the note property manager calling it "SAND CAST"
Then saved that note style to my library as SAND CAST.sldnotestl

To insert a note, i drag it in from the library where i saved it.
it works fine on my machine now. But no one else can get the note to come in properly. The text comes in perfect and all of the special properties are working fine. The GD&T frames say "#error: broken link" and the same is true for the surface finish symbol.

All of these computers here have the same exact Solidworks load, Exact same settings and our file locations for the GTOL.SYM are online such that we are all looking at the exact same file.

Weird!

Any ideas? Anyone?

Regards,
Jon

 

[handleman]

How are you creating these notes and inserting the GDT items?

If you create a GDT frame, then create the note, and click the frame while editing the note to insert it, you don't actually insert it. You insert a reference to the other frame. The actual content of the note is something like

MACHINED SURFACES
<OBJECT-ID=865>

(I forget exactly). So SW reads that text and goes looking inside the current document for an object with ID of 865. If it finds one, it puts an image of it inside the note. If it doesn't, it tells you there was a link error.

 

[APPENG]

^ I am creating them while inside of the note. So i click the insert note on the annotations toolbar and begin typing.
When I get to the part where i need to add the GD&T its pretty simple. If you look in the property manager of the note, you will see under the text format section, there are buttons for the text aligment, the angle, then you see an array of buttons starting with links to the web, links to solidworks properties, symbols etc... there us a button to insert GD&T as well.

So for example I type the text:
FOR THE PURPOSES OF GEOMETRIC TOLERANCING, ALL
DIMENSIONAL INFORMATION CONTAINED IN THE CAD
MODEL IS BASIC (THEORETICAL)

UNLESS OTHERWISE SPECIFIED:

CAST SURFACES
[my gd&t block goes here] ALL OVER

MACHINED SURFACES
[another gd&t block goes here]

The gtol file is there and working or else i would not be able to create them in the first place, nor would any of the other symbols... strange.

Regards,
Jon

 

[handleman]

I looked at it a bit... This really has nothing to do with the gtol file. You mentioned that the notes work on your machine... Are you sure it works all the time on your machine, or does it just work in the specific document where you created the notes?

When you insert things into a note using one of those buttons, what really happens behind the scenes is that SW creates a hidden geometric tolerance annotation object (or surface finish annotation, as the case may be) in your drawing. This object gets an ID. The actual content of the note is a text link to this invisibile annotation. You can see this if you right-click on the note and choose "Edit in window".

It appears that when you copy and paste an entire note, SW knows behind the scenes to also copy that hidden annotation. Check the "Edit in window" content on a pasted note, and you'll see it has a different number. You can even paste into a different document and SW will still copy the hidden annotations. Again, they'll have a different ID number.

However, it looks like the .sldnotestyl file does not save the embedded hidden annotations. It only saves the text with that <OBJECT-ID > stuff. So when you add it to a drawing that doesn't contain an object with that ID, you get a link error.

But.... You wanna know the extra weirdness? Every single annotation has an ID, whether it's referenced or not. If you add this note with the object link to some document that already contains objects with those IDs, then those objects will show up in your note.

 

[APPENG]

Funny you should mention that. After I thought I was onto something I tried it on a new document and it failed. So to answer your question, it only seems to work int he document i created it in. I also tried creating the note, saving it as a block, and going that route.. it had the same results.

I see what you are saying, it does seem that solidworks is assigning an object ID to each note (sequentially) so what I see here is:
CAST SURFACES
<OBJECT ID="902"> ALL OVER

MACHINED SURFACES
<OBJECT ID="903">

CORNER RADII <border type=4 size=0 padding=0>RX.X</border> (this is because I have a box around the "RX.X")

FILLET RADII <border type=4 size=0 padding=0>RX</border>

MACHINE STOCK <border type=4 size=0 padding=0>X</border>

MACHINED SURFACES <OBJECT ID="904">

DRAFT ANGLE X.X<MOD-DEG> MAX

Thank you so much for the tip. I am going to try a few things to workaround. I'll report back one way or the other!

Regards,
Jon

 

[moon161]

Changes I made, I did it by manually editing gtol.sym to make new objects, then distributing the new file.

 

[SBaugh]

Have you tried saving the note as a block? then you should be able to insert it into any drawing maintaining the links. I don't do like what your talking about, but I do save all my common notes to a block that can be inserted into any drawing.

Scott Baugh, CSWP
CAD Systems Manager
Evapar

http://www.evapar.com

"If it's not broke, Don't fix it!"

faq731-376