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Drawing Property Links

Question asked by Gerald Watts on Jun 22, 2010
Latest reply on Jan 25, 2018 by Chris Appleby

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I've been trying to decypher this SolidWorks Help for a while and I guess I just don't understand. In this: http://help.solidworks.com/2010/English/SolidWorks/sldworks/LegacyHelp/Sldworks/drawings/Linking_Notes_to_Document_Properties.htm, it says:

"To automatically insert information in a drawing, you can link note text in the drawing sheet or drawing sheet format to document properties. For the procedure to add a link in a note, see Link to Property.

All SolidWorks documents have system-defined properties, including the following:

Property Name	Value
SW-Author	Author field in Summary Information dialog box

...and it goes on for quite a few items including dates and material. The only property links that work for me are file name and folder name everything else I've always had to enter manually. As we get busier it would be nice to have this working.

I haven't been able to figure out where to add information for "checked by", "eng approval", "material", "finish" etc. Even though I put the material on the solid or the design journal it just doesn't show up automatically. AND even though it's suposed to return "ERROR" if the information isn't found the only thing that does is "weight" and "scale"(I think). I assume the links have to refer someplace for the information but where? The "properties" of the Anotations in the Title Block are set to use custom properties from "current document" but it doesn't seem to make any difference how it's set. Am I suposed to create an Database or something in the drawing folder attached to the drawing, or model, somehow, for a reference? Just stabbing in the dark since at this oint I'm lost...

Filipe Venceslau Jun 23, 2010 2:54 AM

Correct Answer

Hi Gerald,

seems like you're a bit confused, but that's ok. This is very easy to understand.

Basically when you want to link some sort of information onto a drawing/annotation, solidworks deals with property values (properties).

File Properties/ CustomProperties are values stored within the document file that contain specific and custom information about itself.

There are generally two types of Properties:

1 - system-defined (SW-File Name, SW-Folder Name, etc,etc) - These are the fixed properties that are read-only

2 - Custom Properties...These are the actual Custom Properties, that you can edit, and tweak around for your own special needs.

If you point to File--> Properties (from a sldprt file)...you'll get the summary information windows pop-up.

There are three tabs here

The first contains the summary information about the file (all these properties are system-defined)
The next one is the custom tab, this is where you will start adding properties for your custom needs
The last tab is also a custom property tab, but the custom property values apply only to the configuration selected in the "Apply To:" drop-down menu (you would use this, if different configurations of your model would need different values). This tab only exists in part/assemblies, not in drawings...since there are no configurations for drawings.

As for the custom tab, these are also reffered to as the document properties (think of it as properties that don't rely on the configuration, while the configuration specific tab does.

So, if you want to link something onto a drawing for example, let's say, the date the document was last saved....With your drawing open, point to Insert->Annotations-->Note, now before you set the note on the drawing, on the left side you'll see the Note PropertyManager, under Text Format, right below the angle, there is an option called "LinkToProperty", select this option, and you'll have a series of option to chose from...

Current Document (These are the properties listed under the Custom tab from before)
Model in view to wich annotation is attached (This option would be available if there was a view in the drawing and you had the view active when inserting the note, allowing to link to the properties of the assembly/part it was referenced to)
Model in view specified in sheet properties (Reads properties from the model specified in the Properties of the active sheet)
Component to which the annotion is attached (Reads properties of the actual component the annotiation has it's cursor pointed to)

So now if you just select current document. You will see a long list of properties already available (these are all the system-defined properties we mentioned previously), pick "SW-Last Saved Date(Last Saved Date)" from the list and leave all other option default, click ok...and the note is ready to drop.

This is how you link a note to a custom property/file property....

Now, what we just did, is exactly the same as adding a new note, and instead of clicking on the PropertyLink tool, we type in the code...$PRP:"SW-Last Saved Date(Last Saved Date) straight into the typing box. This creates a link to the system-defined property Last Saved Date. If you hover over a linked custom property, once inserted, solidworks will show you the "code" that builds that link.

One thing good to know here, is the way the "code" works....basically, first you call, the type of property you want...in this case we just wanted the standard document (right from the drawing, because we want to know when it was last saved) property, for wich we use the "code" $PRP, the we separate this with a colon, and add the name of the property to retreive in double quotes ( " ). So again, $PRP (for the current document, in this case the drawing), then "SW-Last Saved Date(Last Saved Date)". There are 4 types of calls you can make (these are basically the 4 opions we had before, when using the link utility)...

$PRP (links to properties of the current document)
$PRPVIEW (used only in drawings, and links to the custom properties of the model to which the view is referencing to)
$PRPSHEET (used only in drawings, and links to the properties of the model as per in the properties of the current sheet)
$PRPMODEL (links to the properties of the model/component to which it is attached)

Ok, so with all that said, if say you needed a field on your title block, with the name of the project the drawing was associated with, you would add a custom property to the custom tab under File->Properties, just name it "Project", and give it a value of whatever you like, say "Solidworks". Now you can do the same we did with the date, only for the custom property name you would use "Project", so if you were to type it, it would be like so: $PRP:"Project"

I hope, this helps...wow that was a long post...didn't mean to get carried away...

cheers

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Walter Fetsch Jun 22, 2010 8:34 PM

Hi Gerald,

I think what you need is to to is add the notes that you need in the title blocks (make sure to set your justification now). I am making the assumption that you want to extract the title block data from the part file. To do this, you want your notes to read: $PRPSHEET:{property field}. The text that you put where it says "property field" needs to be exactly what the field is named in your part's custom properties. For example, on our parts, the person who designed the part puts his initials in a custom property called "drawn_by". You can do this for any custom property.

I hope this helps.

Regards,

Walter

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Filipe Venceslau Jun 23, 2010 2:54 AM

Hi Gerald,

seems like you're a bit confused, but that's ok. This is very easy to understand.

Basically when you want to link some sort of information onto a drawing/annotation, solidworks deals with property values (properties).

File Properties/ CustomProperties are values stored within the document file that contain specific and custom information about itself.

There are generally two types of Properties:

1 - system-defined (SW-File Name, SW-Folder Name, etc,etc) - These are the fixed properties that are read-only

2 - Custom Properties...These are the actual Custom Properties, that you can edit, and tweak around for your own special needs.

If you point to File--> Properties (from a sldprt file)...you'll get the summary information windows pop-up.

There are three tabs here

The first contains the summary information about the file (all these properties are system-defined)
The next one is the custom tab, this is where you will start adding properties for your custom needs
The last tab is also a custom property tab, but the custom property values apply only to the configuration selected in the "Apply To:" drop-down menu (you would use this, if different configurations of your model would need different values). This tab only exists in part/assemblies, not in drawings...since there are no configurations for drawings.

As for the custom tab, these are also reffered to as the document properties (think of it as properties that don't rely on the configuration, while the configuration specific tab does.

Current Document (These are the properties listed under the Custom tab from before)
Model in view to wich annotation is attached (This option would be available if there was a view in the drawing and you had the view active when inserting the note, allowing to link to the properties of the assembly/part it was referenced to)
Model in view specified in sheet properties (Reads properties from the model specified in the Properties of the active sheet)
Component to which the annotion is attached (Reads properties of the actual component the annotiation has it's cursor pointed to)

This is how you link a note to a custom property/file property....

$PRP (links to properties of the current document)
$PRPVIEW (used only in drawings, and links to the custom properties of the model to which the view is referencing to)
$PRPSHEET (used only in drawings, and links to the properties of the model as per in the properties of the current sheet)
$PRPMODEL (links to the properties of the model/component to which it is attached)

I hope, this helps...wow that was a long post...didn't mean to get carried away...

cheers

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Gerald Watts @ Filipe Venceslau on Jun 23, 2010 4:27 PM

Thank you Filipe,

Have been asking and trying to figure this out for a long time. Finally learned enough to ask the question the right way. That's the problem with not knowing what you don't know; it sometimes takes a long time to discover the answer.

Your answer was very thorough; just what I needed; perfect.

Thank you so very much,

Jerry

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Filipe Venceslau @ Gerald Watts on Jun 23, 2010 4:33 PM

Hi Gerald,

I'm glad I was of help.

You're right, it is a problem not knowing the minor details sometimes...it makes it so hard to even ask a question sometimes...

I totally understand that, since I've been in that situation before.

So, did you try out adding links and all that? Easy enough?

My english isn't perfect, so there might have been something I failed to explain properly...but if you still have any questions...feel free to ask!

Cheers,

Filipe

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Chris Appleby @ Filipe Venceslau on Nov 7, 2017 11:59 AM

Great information! Glad I came across this post. In regards to the coding. Ever want to bring in a configuration specific property? I only get the property from the active configuration when trying those codes. What if you want to link to a dimension that is changing on your configurations. I think I could put a hidden view for each config in my drawing and make each link to that hidden model but that would be too tedious and not easy to update for future revs. I think if I type the code directly into the table it will work so I might just try that but I would like to know if one of the 4 mentioned can be pointed to a particular configurations. Thanks

my property value that pulls the configuration specific dimensions : "DIM A@Sketch1@@550384-500@550384.SLDPRT"

Property Name is Dimension A

So I there another code that will bring a configuration specific property into a drawing or am I stuck typing each code in changing the config name as applicable in this case the config name is 550384-500

P.S. I already (kinda) have a way to this this using a BOM table but that causes other conflicts so this is just for general tables

THANKS!!!

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Deepak Gupta Jun 23, 2010 3:15 AM

Check this site http://www.solidworkstemplates.com/ if you can get some useful info.

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Chris Appleby Jan 25, 2018 3:02 PM

ER #:

1-16657929612

I submitted this feature request for many of the missing tools we need for making tabulated drawings from configurations. I think it relates to this thread. Please review and vote on it by logging into your Solidworks Customer Support Portal and searching for the number above.

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7 Replies

Walter Fetsch Jun 22, 2010 8:34 PM
Mark Correct
Correct Answer
Hi Gerald,

I think what you need is to to is add the notes that you need in the title blocks (make sure to set your justification now). I am making the assumption that you want to extract the title block data from the part file. To do this, you want your notes to read: $PRPSHEET:{property field}. The text that you put where it says "property field" needs to be exactly what the field is named in your part's custom properties. For example, on our parts, the person who designed the part puts his initials in a custom property called "drawn_by". You can do this for any custom property.

I hope this helps.

Regards,

Walter
Like • Show 1 Like1
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Filipe Venceslau Jun 23, 2010 2:54 AM
Unmark Correct
Correct Answer
Hi Gerald,

seems like you're a bit confused, but that's ok. This is very easy to understand.
Basically when you want to link some sort of information onto a drawing/annotation, solidworks deals with property values (properties).
File Properties/ CustomProperties are values stored within the document file that contain specific and custom information about itself.

There are generally two types of Properties:
1 - system-defined (SW-File Name, SW-Folder Name, etc,etc) - These are the fixed properties that are read-only
2 - Custom Properties...These are the actual Custom Properties, that you can edit, and tweak around for your own special needs.

If you point to File--> Properties (from a sldprt file)...you'll get the summary information windows pop-up.
There are three tabs here
- The first contains the summary information about the file (all these properties are system-defined)
- The next one is the custom tab, this is where you will start adding properties for your custom needs
- The last tab is also a custom property tab, but the custom property values apply only to the configuration selected in the "Apply To:" drop-down menu (you would use this, if different configurations of your model would need different values). This tab only exists in part/assemblies, not in drawings...since there are no configurations for drawings.
As for the custom tab, these are also reffered to as the document properties (think of it as properties that don't rely on the configuration, while the configuration specific tab does.

So, if you want to link something onto a drawing for example, let's say, the date the document was last saved....With your drawing open, point to Insert->Annotations-->Note, now before you set the note on the drawing, on the left side you'll see the Note PropertyManager, under Text Format, right below the angle, there is an option called "LinkToProperty", select this option, and you'll have a series of option to chose from...
1. Current Document (These are the properties listed under the Custom tab from before)
2. Model in view to wich annotation is attached (This option would be available if there was a view in the drawing and you had the view active when inserting the note, allowing to link to the properties of the assembly/part it was referenced to)
3. Model in view specified in sheet properties (Reads properties from the model specified in the Properties of the active sheet)
4. Component to which the annotion is attached (Reads properties of the actual component the annotiation has it's cursor pointed to)
So now if you just select current document. You will see a long list of properties already available (these are all the system-defined properties we mentioned previously), pick "SW-Last Saved Date(Last Saved Date)" from the list and leave all other option default, click ok...and the note is ready to drop.
This is how you link a note to a custom property/file property....

Now, what we just did, is exactly the same as adding a new note, and instead of clicking on the PropertyLink tool, we type in the code...$PRP:"SW-Last Saved Date(Last Saved Date) straight into the typing box. This creates a link to the system-defined property Last Saved Date. If you hover over a linked custom property, once inserted, solidworks will show you the "code" that builds that link.

One thing good to know here, is the way the "code" works....basically, first you call, the type of property you want...in this case we just wanted the standard document (right from the drawing, because we want to know when it was last saved) property, for wich we use the "code" $PRP, the we separate this with a colon, and add the name of the property to retreive in double quotes ( " ). So again, $PRP (for the current document, in this case the drawing), then "SW-Last Saved Date(Last Saved Date)". There are 4 types of calls you can make (these are basically the 4 opions we had before, when using the link utility)...
1. $PRP (links to properties of the current document)
2. $PRPVIEW (used only in drawings, and links to the custom properties of the model to which the view is referencing to)
3. $PRPSHEET (used only in drawings, and links to the properties of the model as per in the properties of the current sheet)
4. $PRPMODEL (links to the properties of the model/component to which it is attached)
Ok, so with all that said, if say you needed a field on your title block, with the name of the project the drawing was associated with, you would add a custom property to the custom tab under File->Properties, just name it "Project", and give it a value of whatever you like, say "Solidworks". Now you can do the same we did with the date, only for the custom property name you would use "Project", so if you were to type it, it would be like so: $PRP:"Project"

I hope, this helps...wow that was a long post...didn't mean to get carried away...

cheers
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- Gerald Watts @ Filipe Venceslau on Jun 23, 2010 4:27 PM
  Mark Correct
  Correct Answer
  Thank you Filipe,
  
  Have been asking and trying to figure this out for a long time. Finally learned enough to ask the question the right way. That's the problem with not knowing what you don't know; it sometimes takes a long time to discover the answer.
  
  Your answer was very thorough; just what I needed; perfect.
  
  Thank you so very much,
  Jerry
  Like • Show 1 Like1
  Actions
  - Filipe Venceslau @ Gerald Watts on Jun 23, 2010 4:33 PM
    Mark Correct
    Correct Answer
    Hi Gerald,
    
    I'm glad I was of help.
    You're right, it is a problem not knowing the minor details sometimes...it makes it so hard to even ask a question sometimes...
    I totally understand that, since I've been in that situation before.
    
    So, did you try out adding links and all that? Easy enough?
    My english isn't perfect, so there might have been something I failed to explain properly...but if you still have any questions...feel free to ask!
    
    Cheers,
    
    Filipe
    Like • Show 1 Like1
    Actions
- Chris Appleby @ Filipe Venceslau on Nov 7, 2017 11:59 AM
  Mark Correct
  Correct Answer
  Great information! Glad I came across this post. In regards to the coding. Ever want to bring in a configuration specific property? I only get the property from the active configuration when trying those codes. What if you want to link to a dimension that is changing on your configurations. I think I could put a hidden view for each config in my drawing and make each link to that hidden model but that would be too tedious and not easy to update for future revs. I think if I type the code directly into the table it will work so I might just try that but I would like to know if one of the 4 mentioned can be pointed to a particular configurations. Thanks
  
  my property value that pulls the configuration specific dimensions : "DIM A@Sketch1@@550384-500@550384.SLDPRT"
  Property Name is Dimension A
  
  So I there another code that will bring a configuration specific property into a drawing or am I stuck typing each code in changing the config name as applicable in this case the config name is 550384-500
  
  P.S. I already (kinda) have a way to this this using a BOM table but that causes other conflicts so this is just for general tables
  
  THANKS!!!
  Like • Show 1 Like1
  Actions
Deepak Gupta Jun 23, 2010 3:15 AM
Mark Correct
Correct Answer
Check this site http://www.solidworkstemplates.com/ if you can get some useful info.
Like • Show 1 Like1
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Chris Appleby Jan 25, 2018 3:02 PM
Mark Correct
Correct Answer
ER #:
1-16657929612
I submitted this feature request for many of the missing tools we need for making tabulated drawings from configurations. I think it relates to this thread. Please review and vote on it by logging into your Solidworks Customer Support Portal and searching for the number above.
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