Solidworks Custom Properties in Templates

[JEREMER]

I am trying to make templates in SolidWorks 2005 and I figured out how to set properties in a part/assembly but I want to use those properties in a drawing template. Can someone help me out?

Also is it possible to meke it so when you open the File->Properties Menu all the properties show up. So the person setting the properties for the first time doesn't have to click the pull down, press tab THEN enter a value for each property? So they can just click where they want to enter a value, enter it and click ok.

Please help, I've been racking my brain for the last few weeks at work trying to get this simple little thing to work.

Thanks,
Jr-

 

[Heckler]

Jr,

Take your mouse and place it over the

button then type in properties......you will then receive all the posts from this forum that deals with properties. You will find your answer there grasshopper. In the future please do your part in searching the resources on this forum. A lot of power-users here have put great effort into the FAQ section.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 5.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
o
_`\(,_
(_)/ (_)

"Coming together is a beginning, staying together is progress, and working together is success." - Henry Ford

 

[CorBlimeyLimey]

Check the Help index section for:-

link, notes to properties
customize, drawing sheet formats


Helpful SW websites faq559-520
How to get answers to your SW questions faq559-1091

 

[JEREMER]

I've already searched through the threads and haven't found what I wanted (hence why I'm making a new post).

 

[wgchere]

There was a thread in the last few months that had a way to copy the Cutom Properties to another file. It involved an excel spread sheet, but I don't remember the thread...

Does the poster of that fix remember?

 

[smcadman]

Since this is your first post (and reply), maybe you just didn't know what to search for
THREAD559-105113
THREAD559-559-139990

Flores
SW06 SP2.0

 

[TheTick]

Try this:

Part "A" has property named "Prop1", value = Test Property

Drawing (or Template) "B" has property named "Prop1", value $PRP:"Prop1" (case sensitive, include quotes)

Put Part "A" into Drawing "B", regenerate, and look at properties in Drawing "B".

p.s. There are veteran forum members here who also don't always find what they are looking for using Search.

I could be the world's greatest underachiever, if I could just learn to apply myself.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[CorBlimeyLimey]

Make sure the custom templates you are creating contain all the properties you & your colleagues need. Then when you open a new document those properties will automatically populate the File > Properties dialogue box.

The drawing template, does not normally contain the same properties as the part or assy. The sheet format usually has notes which are linked to generic properties, & when a parts view is placed on it, those generic properties are replaced with the actual parts property.


Helpful SW websites faq559-520
How to get answers to your SW questions faq559-1091

 

[JEREMER]

ok, I got all that set up in my "part" and my "template" but every time i try to click the "link" button to link the text to the property in the File -> Properties dialog box it crashes on me. Was i supposed to set the property value to e.g. $PRP:"prop1" in the "template"?

I set the "part" prop1 value to "something", the "template" property prop1 value to "$PRP:"prop1" and then i try and link the text i put in to the property but it crashes. What am i doing wrong?

 

[SBaugh]

If it's crashing, then it's probably not what you are doing... look in the FAQ - it will tell you how to do a Repair/Modify on your system.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[JEREMER]

Yeah, I figured I would try that but, I was wondering if I am doing this wrong or not.

CorBlimeyLimey said:
part/assy model
property (prop1) value = Anything

drawing template
property (prop1) value = $PRP"prop1"

Is that correct?

If I just use $PRP"prop1" in the drawing as the text it links it to a property set in the drawing under File -> Properties. This kind of works but like I said before I want to make a template to link to the model properties. Please, someone help... I can't find ANYthing online, in tutorials here or anywhere.

Thanks,
Jr-

 

[CorBlimeyLimey]

Actually it was TheTick who "said" what you wrote.

OK, step by step:-

1) Open a new drawing document.
2) Insert a view of a part.
3) RMB click anywhere in the document, but NOT in the parts view & select Edit Sheet Format.
4) Click on the Note icon in the Annotations toolbar (or Insert > Annotations > Note) & place it on the sheet. Do not type anything.
5) Click the Link to property icon in the Note Manager. It's the one with the hand & chain links.
6) In the new options box which opens, select Model in view specified in sheet properties.
7) Click the chevron to display all the available properties for the part.
8) Select the custom property you want to link to the note & click OK.
9) Click the green check mark or hit the Enter key. The note should now display the property from the part.
10) RMB click anywhere in the sheet & select Edit Sheet
11) Click File > Save Sheet Format, browse to where the Tools > Options > File Locations > Sheet Formats points to, type a file name & click Save.
12) Close the document you have open without saving.

Now when you open a new drawing document, you will be able to select the Sheet Format you just created, & when you insert a part view onto it, the property will automagically be populated.


Helpful SW websites faq559-520
How to get answers to your SW questions faq559-1091

 

[afb66t9]

Does this help

http://solidworktips.com/swx_pages/09_properties_and_boms_9.htm

http://www.solidworktips.com/api_pages/03_part_1.htm

http://solidworktips.com/api_pages/04_Adding_User_Interface.htm