File properties (Custom)
File properties (Custom)
(OP)
Help mentions you can add custom properties through Windows explorer (Right-click / Properties / Custom) and they will show up as Part Attributes in UG. This doesn't seem to be the case though.
What I want to do is enter the "description" as a custom property for both the Model and Drawing file without having UG open. Plan to do it with a VB program that accesses both file's custom properties. Then in UG the description in the title block would be linked to the property(attribute).
Upon check into our PDM (Matrix), it would automatically extract this into the database for both Drawing and Model object types.
Any idea why this doesn't work as the help suggests?
What I want to do is enter the "description" as a custom property for both the Model and Drawing file without having UG open. Plan to do it with a VB program that accesses both file's custom properties. Then in UG the description in the title block would be linked to the property(attribute).
Upon check into our PDM (Matrix), it would automatically extract this into the database for both Drawing and Model object types.
Any idea why this doesn't work as the help suggests?
Jason Capriotti
Smith & Nephew, Inc.





RE: File properties (Custom)
I'm wondering this thing too.
You seem to need link Model and Drawing attributes and so do I.It's one of the biggest wishes after getting use to how SolidWorks handles them.Let's see what next week brings when NX3 gets installed.Maybe I still have to find or let someone write program to synchronize attributes.
Henry Mägi,
RM-tools
RE: File properties (Custom)
-Derek
DL Engineering Services
specializing in CAD Design Consultation Services
www.dl-engineering.com
RE: File properties (Custom)
"Wildfires are dangerous, hard to control, and economically catastrophic."
Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand
RE: File properties (Custom)
will those attributes in drawing file get updated?
Henry
RE: File properties (Custom)
"Wildfires are dangerous, hard to control, and economically catastrophic."
Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand
RE: File properties (Custom)
thanks for explanation.There really is method of referencing part attributes.However in my opinion you have to get those attributes to the non-master drawing manually every time.
On different drawings you get different attribute notes for same master file:
<W!8225@HRC>
<W!49383@HRC>
What next?Create GRIP or VB code to fill title block with selected part attributes?
Henry Mägi
RE: File properties (Custom)
"Wildfires are dangerous, hard to control, and economically catastrophic."
Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand
RE: File properties (Custom)
The program names the solid chosen (we'll call it 'MYSOLID') then assigns the calculated weight value to an attribute named 'PW' (part weight). The note then looks like this: 'PART WEIGHT : <WMYSOLID@PW>'. Whenever the weight attribute is updated (whenever the program is run again) the note will automatically update to the new value.
I hope this helps.
RE: File properties (Custom)
Any chance of posting the source for that Grip program, for those of us who are not Grip developers, but really like the power and convenience of those tools?
-Derek
DL Engineering Services
specializing in CAD Design Consultation Services
www.dl-engineering.com
RE: File properties (Custom)
For example, I have a model of a retaining ring; I named it RING and gave it an attribute MATL with the value STEEL. In the drawing I would place a note with this text: "MATERIAL: <WRING@MATL>". The note would read "MATERIAL: STEEL" and would automatically update when the attribute changes. Note the "W" before the name, this is important.
If/when I get a few free minutes I'll try to post a short grip demo, but right now things are a little busy and the program that I have is fairly long (it does more than just assigning attributes) and it might be difficult to pick out the bits you are interested in.
RE: File properties (Custom)
Jason Capriotti
Smith & Nephew, Inc.
RE: File properties (Custom)
RE: File properties (Custom)
You can link Attribute from Master model with non-Master drawing:Drafting,Annotation editor,Annotation editor,Relationship,Object Attribute,now put cursor on needed modelview,hold on just a second until selection box comes out,from it select :(master file name).Choose needed attribute.It's gone be something like this: <W!10023@ATTRIBUTE_NAME>.Number inside is going to change after opening file afterwards but attribute is linked.
Big question stays:how can we make drawing templates if this number changes all the time? Use PDM? Use GRIP or VBA to update annotations in drawing with new number? "The truth is somewhere out there"
Henry
RE: File properties (Custom)
Refer to my previous post, choose a common name for your parts (e.g. 'MODEL') then you can put notes in your templates like <WMODEL@ATTRIBUTE>. As long as you are consistent with the name, it will pull in the correct information.
RE: File properties (Custom)
Jason Capriotti
Smith & Nephew, Inc.
RE: File properties (Custom)
The method I describe won't do anything for the custom (right click) file properties that you describe in your first post; but it does allow attributes to be transferred to the drawing (whether it is master model or not). This seems to be what you were referring to in your first post and the question was directly raised by others in subsequent posts.
In Unigraphics you can name objects so that you can refer to them by that name later. For instance the delete command or trim body command (among others) will let you type in a name rather than picking with your cursor. If you name your solid model and assign attributes to it you can refer to it by name rather than some system generated number in the linked attribute note. So, if I name my solid model 'MODEL' and assign attributes to it I can put a note on my drawing <WMODEL@ATTRIBUTE> and it will show the attribute associated with the solid. If you are doing piece part drawings you can pick a common name ('MODEL') and use it in your template. If, however, you are doing multiple part assembly drawings and want to use these linked notes, the parts will probably have to have separate names (the linked notes I use are only for single part drawings so I have not had problems, but I assume it would cause problems for multiple part drawings).
I hope this solves the problem.
RE: File properties (Custom)
I try to create my templates according the way you do, but it doesn't work.
I doesn't allow me to create this annotation, it is an invalid annotation.
I think I do something wrong here ...
RE: File properties (Custom)
RE: File properties (Custom)
CODE
RE: File properties (Custom)