SW 05/Attribute transfer from Part to Drawing???

[markhp48]

I am trying to populate & transfer the attributes from my part to its associated drawing file for final mapping & eventual use in a PLM/PDM vault application that will simply read data from one file. In short, you usually fill out these attributes after creating a part, by accessing File-Properties-Custom tab, selecting or creating your Property Name prompts(tags) & then populating your list values as necessary. Is there any way to carry these same Tags & Values from the part-assy file over to its drawing file without having to recreate the wheel & raise the potential for errors? Also by chance, while in the same Custom tab dialog box & after creating a Custom Property tag, would anyone out there know how to enter a Value/text expression as a Drop Down choice with the type set to text?

I'll buy you a beer, maybe a couple for both answers.

Mark

 

[MElam]

Do you know which PLM/PDM vault application you will be using? Some can do this automatically as the files are loaded into the system.

Otherwise, I do believe there are some macros floating around somewhere that can do this.

 

[smcadman]

In SW they are called properties not attributes.
thread559-125139

Flores
SW06 SP3.0

 

[markhp48]

Allright Let's just forget about the PDM/PLM side of it. How do you transfer the File-Properties-Summary Info-Custom Props(attributes) from the part to its assoc drawing file? I'm trying to enter this custom data one time & one time only.

This data is aka metadata & attributes in most PDM/PLM software.

 

[CorBlimeyLimey]

In the SW Help Index, go to drawing sheets, customizing sheet formats

It is explained there, in detail.


Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[markhp48]

Thanks for the info. I've seen the sheet format help before & not to sure if it all applies to my issue of property migration from part to dwg.


What about setting up drop down choices for the Value-Text expression in the Custom Properties area?

 

[MElam]

If you use a custom properties macro - like the ones in the thread smcadman referenced - and know a little VB, adding the drop down list would be easy.

I do not know how to do it without a macro

 

[smcadman]

I'm not sure if your new to Solidworks, but I know your new here to this forum. A little work will be required on your part. If you do a search in SW Help for "customizing sheet formats" exactly like CorBlimeyLimey posted, AND read the first topic that came up, you would have your answer.

Flores
SW06 SP3.0

You can lead a horse to water, but you can’t make him drink.

 

[CorBlimeyLimey]

See also Solidworks Custom Properties in Templates thread559-141106


Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[TheTick]

<

http://www.esoxrepublic.com/freeware>

Copy Custom Info macro.

Also...
[ol]
[li]Say "Widget.sldprt" has property named "Prop1", assigned value "Shizzle".[/li]
[li]You want a property in "Widget.slddrw" to also have a property named "Prop1" that matches value in "Widget.sldprt".[/li]
[li]Create a property in "Widget.slddrw", assign it the value $PRPSHEET:"Prop1" (case sensitive, quotes and colon necessary, Name in quotes matches name of property in model used in default view)[/li][/ol]

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

 

[markhp48]

Doing just what you said while editing the Sheet Format is no problem, but while in the Custom Properties dialog of a drawing & assigning $PRPSHEET:"Prop1" to the Value/Text-Expression field, I only get just what was typed ($PRPSHEET:"Prop1), no further evaluation that would demonstrate the link to the model itself. What am I missing here?

 

[CorBlimeyLimey]

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

 

[markhp48]

I know how to do the very procedure you are describing with the Sheet Format. The issue I have is with the Custom Properties & migrating the properties for the part to its associated drawing. The very links you are describing while applying annotations to the sheet format using $PRP & $PRPSHEET are not working while in the File-Properties-Custom tab. My values are not being evaluated properly in the Value-text expression field of the Custom tab, even when using the format $PRPSHEET:"Property Name" in the above mentioned field. My sheet format is fine; I just want to carry the properties from the model to its drawing without having to retype them in the Custom Properties dialog. Something fairly simple is not being done to establish this connection either by formatting or my understanding. Thanks for your replies ntl.

Mark H
mech engr

 

[CorBlimeyLimey]

Does you model have configurations?
Try entering the properties in the Configuration Specific section.


Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[GunT]

Few questions first.

1. Were you atleast able to link and display value of some Custom Properties or were you not able to display the value of any of the Custom Properties?

2. Exactly what are you trying to link? Are the properties listed anyway related to Revision Table?

Regards

 

[markhp48]

I can link with $PRP: & $PRPSHEET: while using annotations in the sheet format, no problem there, but the $PRPSHEET:"property" does not evaluate to the correct assigned value when placed in the Value-Text Expression area of the Custom Properties dialog box for the part or drawing file. My only existing configurations are just the default & I'm running SW 05. Perhaps I am doing something wrong in the Custom Props dialog or some other setting is to blame. I simply want to transfer those assigned custom props from my model to its assoc drawing file. No problem with the sheet format & related links at all. Thanks for the comments

Mark
mech engr

 

[markhp48]

I'm trying to eliminate the need to have the fellas in this engineering dept retype-recreate the Custom Properties in the drawing file after they have been done in the model or assy. The values are eventually utilized by our PDM-PLM manager(Product Center) as attributes & checked into the vault area. Just attempting to prevent double work & errors. Also, I would like to have a drop down show up in the Value-text expression area of the Custom Props dialog that I could assign custom values from a list for a given Property Name. Any takers?

Thx

Mark

 

[CorBlimeyLimey]

My values are not being evaluated properly in the Value-text expression field of the Custom tab, even when using the format $PRPSHEET:"Property Name" in the above mentioned field.

What exactly did you type in the Value/Text Expression field?



Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[wgchere]

Criminey, youse guys!

The man wants to copy the cutom properties in the part/assy file to the custom properties of the drawing file! He has explained several times that he knows how to get the custom properties in the part/assy file to populate on the face of the drawing. That isn't his question. He wants to copy the information that will show up in the PDM tree, i.e. the Custom Properties from the File heading in the pull down menu. (I think--I have been wrong on occasion. )

Having said that, I think it was answered in the 3rd post. The caveat was "if you know a little VB." I don't, so I've never been able to figure out those macros. Markhp48 may be in the same boat.

 

[rmars]

I agree with wgchere. we had the same problem withour PDM system. We fill the custom properties in the part/assy (eg part number), and this needs to get into the PDM system, via the drawing. We paid someone to do a Solidworks add-in. It just copies the data from the part to the drawing whenever the drawing is opened (or created).