SW 05/Attribute transfer from Part to Drawing???
SW 05/Attribute transfer from Part to Drawing???
(OP)
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
I'll buy you a beer, maybe a couple for both answers.
Mark






RE: SW 05/Attribute transfer from Part to Drawing???
Otherwise, I do believe there are some macros floating around somewhere that can do this.
RE: SW 05/Attribute transfer from Part to Drawing???
thread559-125139
Flores
SW06 SP3.0
RE: SW 05/Attribute transfer from Part to Drawing???
This data is aka metadata & attributes in most PDM/PLM software.
RE: SW 05/Attribute transfer from Part to Drawing???
It is explained there, in detail.
Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091
RE: SW 05/Attribute transfer from Part to Drawing???
What about setting up drop down choices for the Value-Text expression in the Custom Properties area?
RE: SW 05/Attribute transfer from Part to Drawing???
I do not know how to do it without a macro
RE: SW 05/Attribute transfer from Part to Drawing???
Flores
SW06 SP3.0
You can lead a horse to water, but you can’t make him drink.
RE: SW 05/Attribute transfer from Part to Drawing???
Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091
RE: SW 05/Attribute transfer from Part to Drawing???
Copy Custom Info macro.
Also...
http://www.EsoxRepublic.com-SolidWorks API VB programming help
RE: SW 05/Attribute transfer from Part to Drawing???
RE: SW 05/Attribute transfer from Part to Drawing???
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
RE: SW 05/Attribute transfer from Part to Drawing???
Mark H
mech engr
RE: SW 05/Attribute transfer from Part to Drawing???
Try entering the properties in the Configuration Specific section.
Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091
RE: SW 05/Attribute transfer from Part to Drawing???
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
RE: SW 05/Attribute transfer from Part to Drawing???
Mark
mech engr
RE: SW 05/Attribute transfer from Part to Drawing???
Thx
Mark
RE: SW 05/Attribute transfer from Part to Drawing???
Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091
RE: SW 05/Attribute transfer from Part to Drawing???
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.
RE: SW 05/Attribute transfer from Part to Drawing???
RE: SW 05/Attribute transfer from Part to Drawing???
However I believe the only way to do this is by using a macro feature so that when the drawing is rebuilt the properties of the part/assembly are read and then copied to the drawing properties. I haven't seen a macro yet that does this, but it should be possible.
ta
RE: SW 05/Attribute transfer from Part to Drawing???
RE: SW 05/Attribute transfer from Part to Drawing???
strange
RE: SW 05/Attribute transfer from Part to Drawing???
Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091
RE: SW 05/Attribute transfer from Part to Drawing???
Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091
RE: SW 05/Attribute transfer from Part to Drawing???
RE: SW 05/Attribute transfer from Part to Drawing???
Thx
Mark H
mech engr
FPI
RE: SW 05/Attribute transfer from Part to Drawing???
You can’t add a dropdown to the file -> properties page either. However a macro / VB program with dropdowns can be created. PropertyEditorSpec, which can be found at: ht
Eric
RE: SW 05/Attribute transfer from Part to Drawing???
Mark
RE: SW 05/Attribute transfer from Part to Drawing???
--
Hardie "Crashj" Johnson
SW 2005 SP 4.0 (reluctant to change)
Matrox Millenium G550
AMD Athalon 1.8 GHz 512 Meg RAM
RE: SW 05/Attribute transfer from Part to Drawing???
RE: SW 05/Attribute transfer from Part to Drawing???
Examples:
$PRPSHEET:"SW-File Name" = takes info from the drawing properties (in this case, the file name).
$PRP:"SW-File Name" = takes info from the part (model) properties (in this case, the file name).
Summary:
$PRPSHEET: TAKES INFO THAT WAS INPUT TO THE DRAWING
$PRP: TAKES INFOR THAT WAS INPUT TO THE PART (MODEL)
If you do this right, you should not need any properties in the drawing, since everything should be coming from the part (model).
RE: SW 05/Attribute transfer from Part to Drawing???
RE: SW 05/Attribute transfer from Part to Drawing???
I'm still trying to understand what you mean by "evaluations". Are you saying that when in a drawing, you select file, properties and expect to see what you had typed in for properties in the part properties?
RE: SW 05/Attribute transfer from Part to Drawing???
RE: SW 05/Attribute transfer from Part to Drawing???
RE: SW 05/Attribute transfer from Part to Drawing???
I agree however SW should do more in the way of custom properties.
Rob Rodriguez CSWP
President: Northern
Vermont SolidWorks User Group
www.robrodriguez.com (updated 2/22/06)
SW 2006 SP 3.0
RE: SW 05/Attribute transfer from Part to Drawing???
-with the part open, create a ModelDoc2 object equal to the part
-use ModelDoc2.GetCustomInfoNames2 to get names of the desired properties
-use GetCustomInfoTypes2 and CustomInfo3 to get types and values (respectively) of the custom properties, using names obtained in the last step
-use ModelDoc2.getPathName to get the save path of the current part model
-use string manipulation to strip SLDPRT or SLDASM from the pathname and replace it with SLDDRW to get the drawing pathname
-use openDoc6 or GetOpenDocumentByName to open the drawing using the above pathname
-delete custom properties of the drawing (retrive names using getCustomInfoNames then use deleteCustomInfo to loop through each property and delete it)
-add custom properties to the drawing using custom property names, values and types obtained from the part above
-save the drawing (AddCustomInfo3)
This can also be done from outside of Solidworks using the windows DSO method, but as far as I can tell DSO will turn all properties to type "text". You also can't use DSO if the drawing is open in Solidworks.