Drawing Description-Custom Properties 3

[macduff]

I thought I did a thread on this before, but didn't find anything. Is there a way for parts and assemblies descriptions to drive the drawing descriptions? Every time I fill in the description for a part or an assembly and make a drawing, I have to re-fill in the description again for the drawing. Why is that? A drawing is linked to that part or assembly. Why not have the description linked? When you save the drawing the first time, the part or assembly no. is filled in automatically when saving. So, why not have the description fill in automatically?

Thanks,


Macduff
Colin Fitzpatrick
Mechanical Design Engineer
Solidworks 2006 SP 4.1
Dell 380 XP Pro SP 2
nVida Quadro FX 3450/4000

 

[ctopher]

Edit sheet format, select text, link to property (feature manager), model in view. Edit sheet. Make sure to fill in info within model "properties".

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-06)

 

[TheTick]

Assign the value $PRPSHEET:"{property name}" to carry the model's (part or assembly) property through to the drawing.

i.e.
Use $PRPSHEET:"Description" as the value of a property in a drawing to link to the value og the property named "Description" in the drawing's default model file.

Case sensitive.

 

[fcsuper]

The reason you can't (or shouldn't) do this in most mechanical engineering enviroments is simple. Drawings can and will have more than one part on them, in the form of an assembly or even just multiple components on the drawing.

 

[fcsuper]

If you are interested, I have an API macro that copies set property values on-the-fly across active documents.

 

[ctopher]

If a part or an assy on a dwg, this will use the properties description on the dwg from either the part or assy file, regardless how many parts are in the assy.
Drawings should not have more than one part used. If in any case there is, manually type in the title block info.
More companies these days do not create drawings in CAD. The more reason to have each part or assy have its own drawing for tracking, rev control and file management. This should be for all engineering enviroments.

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-06)

 

[dogarila]

I don't think you can do it directly. In my case, I wrote a little macro to assign properties to the drawing, to fill the title block, like "Drawn by", "Checked by", "Drawn date", etc. When I run the macro, it reads the description from the model and assigns it to the description property of the drawing.

 

[CorBlimeyLimey]

Drawings can and will have more than one part on them, in the form of an assembly or even just multiple components on the drawing.

I think you will find that "most mechanical engineering environments" do NOT place multiple parts or assemblies onto a single drawing sheet. A quick survey of the members here will prove or disprove that.

Also, when an assy is placed onto a drawing sheet, it is considered a single component with regard to properties. It can & should have it's own custom/config properties. The $PRPSHEET property, assigned in a drawing note, will not try to read the properties of all the components of an assy.

​

Helpful SW websites faq559-520​

How to find answers ... faq559-1091​

 

[ctopher]

Thanks CBL. You explained it better than me.
I'll give you a star.

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-06)

 

[macduff]

Ok guys.......where do we stand with this? I'm getting a little confused.

Here's an example what I'm trying to do and using the "TheTicks" info a couple threads back.

I have a part with a file name and the CP description filled in as "COVER, BACK" file, save the part.

The I select the "Make Drawing from Pat/Assembly" icon from the toolbar. Select my desired template and drop in a view.

The title block is then automatically filed in for description $PRPSHEET:"Description" and drawing number $PRPSHEET:"SW-File Name" These CP's are linked to my part. I beleive these are defaults CP for SW. This is working fine for me at this point.

Now I go to save my new drawing....The dialog box appears and the "File name" is automatically filled in (make sense because it's link back to the part), the "Save as type" defaults to .drw or .slddrw, (cool) and now the description.......Hmmm.......it's blank. This is where I want it to be linked back to the part CP $PRPSHEET:"Description".

Ok...this is where I'm going back to the "TheTick" thread. I go into my CP of my drawing and have description under "Property Name". My "Type" is set at text. My "Value/Text Expression" is blank. Is this where I need to type in $PRPSHEET:"Description" to link back to my part? When I do this nothing happens. This is where I want the part description to show up without typing it back in.

I hope I'm clear on this.

Thanks Guys,



Macduff
Colin Fitzpatrick
Mechanical Design Engineer
Solidworks 2006 SP 4.1
Dell 380 XP Pro SP 2
nVida Quadro FX 3450/4000

 

[rockguy]

The description you see when saving your drawing is the description specific to the drawing. It has nothing to do with the CP property from your part file. Your title block is linked to the part file CP and working correctly.

Th drawing file can have its own independant CP's. Now, can you link the drawing CP's to the Part or assembly file CP's. Not that I know of unless there is away to program this with a macro or API.

Rob Rodriguez CSWP
President: Northern
Vermont SolidWorks User Group

http://www.robrodriguez.com

(updated 8/12/06)
SW 2006 SP 4.0 / SW 2007 SP 0.0

 

[CorBlimeyLimey]

There was a thread on this a while back but I can't remember if a resolution was found ... I think there was ... I will do a search.

​

Helpful SW websites faq559-520​

How to find answers ... faq559-1091​

 

[ShaggyPE]

Tick is correct.

Another way to explain it:

1. Insert a new annotation.
2. Look in the note properties area on the feature manager.
3. In the "text format" region, you will see an icon with a chain link, a hand, and a paper. Click on this icon. This is the "link to property" icon.
4. The link to property dialog opens up. You will have some options to choose from: Current Document, Model in view which annotation is attached, Model in view specified in sheet properties, and component which annotation is attached.
5. By default, Solidworks uses Current Document for their Drawing annotations. You want to change this one to "Model in view specified in sheet properties"
6. Now your annotation will link back to the part or assembly custom properties rather than the current document's custom property.

-Shaggy

 

[ShaggyPE]

Forgot to add:

7. You can now browse to find the part's custom property you want to link the annotation to.

 

[CorBlimeyLimey]

There's a solution supplied by Eend (last post) in link custom props to drawings thread559-138421

It only works for a parts Custom Properties but may be able to be tweaked to read Config Specific also.

​

Helpful SW websites faq559-520​

How to find answers ... faq559-1091​

 

[CorBlimeyLimey]

Ooops ... ignore the last line in my last post.

I missed the option box in the corner ... the macro works great for Custom and Config Props.

​

Helpful SW websites faq559-520​

How to find answers ... faq559-1091​

 

[fcsuper]

"Drawings should not have more than one part used."

Who's says? This is not an uncommon occurance, cuz of the way drawings work in CAD, and the number of functions they can fulfill. For example, a cable drawing can have multiple connectors inserted on it, linked schematically with lines drawn on the drawing directly. Which part is the drawing supposed to pull the desc from? Well, none, cuz you don't want the cable drawing to carry one particular connector's info. Another example is versionized drawings which show multiple versions or configurations of a part, each with their own information. Some way want that information kept separate from the drawing, or again, they may use multple parts to represent it in model form, but specified by a single drawing. Hard and fast rules like "one part per drawing" don't really take into account the functionality the software offers, and the way in which that functionality can be used.

Another point to consider is the parametric relation this forms. If the model's description is changed, then the drawing will automatically change too. If there is a rigid doc control system in place, this may present issued that would need addressing.

If you don't have any of these issues whatsoever, then it is ok for you to directly refer to the model's desc on the drawing. But I would caution against making software user rules that limit the drawing creator from using the software to its fullest. Maybe a compromised in special cases is that the drafter could manually edit the drawing's desc text field?

 

[macduff]

All,
There's 2 different descriptions $PRPSHEET:"Description" for parts and assemblies and $PRP:"Description" for drawings. I know how to link annotations to properties and like to say thanks. But what I really want to do is to change $PRP:"Description" link under "FILE/PROPERTIES" dialog box and use $PRPSHEET:"Description" in it's place.

$PRPSHEET:"Description"=assembly
$PRPSHEET:"Description"=part
$PRPSHEET:"Description"=drawing

Everytime I delete and re-create the description under "FILE/PROPERTIES" in a drawing. I takes the property of $PRP:"Description" by default. I want to change it to $PRPSHEET:"Description" but won't let me. That way it's always linking back to the part or assembly.

Thanks for all your help

Macduff
Colin Fitzpatrick
Mechanical Design Engineer
Solidworks 2006 SP 4.1
Dell 380 XP Pro SP 2
nVida Quadro FX 3450/4000

 

[AnnaWood]

fcsuper,

I think many of us have a problem with your statement that "most mechanical engineering environments have multiple parts on a detail". To broad a statement....

There are many different scenarios to consider and one has to come up with the best solutions for the type of work and deliverables that their engineering dept is charged with creating and maintaining.

Your examples are great and how you handle your data, I am sure, works well for your enviroment. Doesn't necessarily transfer to all of our work enviroments though.

Regards,

Anna Wood
SW06 SP4.1 x64, WinXP x64
Dell Precision 380, Pentium D940, 4 Gigs RAM, FX3450

http://www.auerprecision.com

 

[EEnd]

macduff,

It sounds like you have this down. But just to be explicit, part files, assembly files and drawing files all have their own description property. In a drawing, you can reference the drawing file’s description in an annotation using $PRP:"Description". You can also reference the description of the model file (part / assembly) of the main view of a sheet using $PRPSHEET:"Description".

There is no way that I know of to link the property of one file (a drawing in your case) to the property of another (a part or assembly). The macro in the post that CorBlimeyLimey referenced lets you copy the value of the number and description properties from a part or assembly file to an open drawing file containing views of that part or assembly. It will copy them the other direction as well. They will not be linked, i.e. changing one will not cause the other to be changed. One might be able to create a similar macro that takes no input which is run whenever a drawing is opened.

Getting them truly linked will probably require a successful enhancement request.

Eric