Company standard notes in library ?? 3

[2000mustanggtguy]

Can I put some standard notes in the Design Libray area ? So all I have to do is drag it from the library are and drag it into my new drawing ?



Printed Circuit Board Designer
Salt Lake City, Utah
Stangs rule!

 

[Heckler]

If they're standard notes just include them in the drawing templetes. I keep my notes in a word file then paste them in when I need.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 4.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
o
_`\(,_
(_)/ (_)

"There is no trouble so great or grave that cannot be much diminished by a nice cup of tea" Bernard-Paul Heroux

 

[smcadman]

Not quite as fast as "drag and drop", but close. Why not use annotation favorites? You can save as many favorites you want, using whatever font, bullets, etc.. Whenever you use the note tool, look at the task pane for the pull down list.

Hint: go to Tools > Option > File Locations > Dimension/Annotation Favorites and point it to where your, um, annotation + dimension favorites are. This way you don't have to search for your favorites.

Flores

 

[Regg]

You can also turn the standard notes into blocks and drag them from the design library. This way if there are multiple annotations and/or graphics in the note they will move together if the standard note needs to be repositioned.

 

[ctopher]

I use the CommonNotes macro.

http://webpages.charter.net/mkikstra/SolidWorks.html

I changed it a bit to match our std notes.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[2000mustanggtguy]

Thanks guys, I need my VAR was full of crap, when he said it can't be done in SW.



Printed Circuit Board Designer
Salt Lake City, Utah
Stangs rule!

 

[Heckler]

Regg,

Great idea....I completely forgot that SolidWorks has adopted blocks. Once the block is created it's stored in a folder located in the feature manager design tree. Open the folder RMB on the block choose save to file (if you have done what smcadman suggested) then the dialog box is right there in design library - annotations.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 4.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
o
_`\(,_
(_)/ (_)

"There is no trouble so great or grave that cannot be much diminished by a nice cup of tea" Bernard-Paul Heroux

 

[rjmax]

I have tried the "favorites" method and then pointing my design library to the folder where the "favorites" are stored and then dragging them in using the design library. It works good.

One question, I have a surface finish symbol in my note and when I bring it in using the methods above, the surface finish symbol changes to say "#error: broken link"? Any suggestions or ideas how to fix this?

 

[btcoutermash]

We also use the "Common Notes" macro and it works great. Easily customized with your companies notes...

 

[dogarila]

A different approach is to include your standard notes into your part and assembly templates (in Properties/Summary/Comments). Add a note to your drawing templates and link it to the properties of the part/assembly. When you create a new drawing for a part, the properties will be inserted automatically. The advantage is that you can individually modify notes in the solid model and that the notes are stored with model. I my opinion notes should be related to the model and not to the drawing.

 

[btcoutermash]

netshop21

So by doing it the way you described, you would have to "edit sheet" inorder to move the notes?? I like the idea, just trying to see how you handle this.

 

[ShaggyPE]

I use a similar method to netshop21. To answer your last question btcoutermash, I like to create the notes on an empty view on the sheet of the drawing, not the sheet format.

To do this, go to insert>view>empty. On this view, create all your notes. This allows you to move all your text together (almost like grouping). The advantage this has over putting your notes on the "sheet format" is that you can see your part geometry when you are moving your notes to prevent any overlap.

 

[CSLufkin]

I make my notes, then right click, and "Add to Design Library". Then you can drag and drop into your drawings. Whats more, if you have the leader on when you save it, your first drop point will be the point of the arrow (and also will link the note to whatever it is pointing to) and your second click will be the text location. I drop them on the edge of a part and it will draw Custom Properties from that part for your notes if you so desire. The only down side is that sometimes you dont want the leader so you have to turn it off(but the note stays linked).

 

[ctopher]

I use "Lock sheet focus" then add notes on dwgs. No need to add views, it doesn't link the notes to other views and you don't have to "edit sheet format".

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[ShaggyPE]

ctopher,
that method works, but if you have groups of different annotations, it is not as easy to move the whole thing as the way I stated above.

An Example:
our Notes section of the drawing is titled "notes" the font of "notes" is 24 pt, Arial, bold. The actual notes are 12 pt Arial. The main body of the notes section is all one annotation. If I have flag notes, the number with a triangle border is a separate annotation.

With all this mis-mash of different annotations, it is nice to be able to move them all at once without the worry that you missed selecting one.

Bear in mind I am still stuck on 2004. I know the annotation capability has improved with 2005 and probably more with 2006. It may be possible to group the annotations or change font and add borders to specific characters within one annotation. Ida know. If that is the case, I would use ctopher's suggestion.

 

[ctopher]

Yes, in 05 and 06 this can be done.
I have 05, notes have different size fonts and flags are included. All move together.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[smcadman]

FYI: You can pick 2 or more notes, right-click them, and pick "Group" so that you can move your notes at the same time.

Flores