Property Linked Value 5

[Ripper2]

ll.
I'd like to have Solidworks insert the values of the blank size on our sheetmetal parts into a property linked value on the drawing.
Therefore, if we make a change that effects the blank size, it will automatically be reflected on a location labeled "Blank Size" on the drawing.

I noticed that if I make a sheetmetal part, unfold it, and put an "x" and "y" dimension on the overalls, and double-click on those dimensions,
the label for that dimension is RD1@Annotations or RD2@Annotations. I should be able to use these in an equation.
In File/Properties, if I have a field named "Blank Size", I should be able to put an equation in such as "=RD1@Annotations x RD2@Annotations".

Can anyone assist me in this?

Thanks!

Rip

SolidWorks 23007 Office Pro.SP 4.0
Compaq Presido 6000
Win XP

 

[ShaggyPE]

You could use those dimensions in a design table that will link to a custom property.

-Shaggy

 

[CorBlimeyLimey]

Help > SolidWorks Help Topics > Index > link, notes to properties > Link to Property

 

[Ripper2]

Thanks Blimey


This "Link to Property" will link text in the drawing to one of the property fields in either the drawing or the model.
These property fields are under "File/Properties". As of now, I don't know a way to link text in the drawing to
dimension values contained within the model (such as dimensions on the blank size).
The topic only explains the former part of above.

Rip

SolidWorks 23007 Office Pro.SP 4.0
Compaq Presido 6000
Win XP

 

[CorBlimeyLimey]

Create a custom property;
Open the Property Manager, assign a property name, select Text] as the Type, and then click on the dimension in the graphics area.

 

[jefrado]

The way I did it was to create annotation dimensions on the flat configuration and link those dimensions, but be careful.

I have been messing with this and have found that these values do not update as expected. I think the bloody program updates these values only when that configuration is viewed. So if you have a block with a 2X4 and 4X6 configuration and the part was last viewed as 2x4, a drawing for the 4x6 configuration will read 2x4 (and so will the BOM on an assy drawing) untill the part is opened and the 4x6 configuration selected. Great feature.

The only safe way to do this, in my experience, is to unsuppress the flat feature if any changes are made to update the properties.

 

[Ripper2]

Thanks Blimey, jefrado,Shaggy,

for all yer help.

Mission..accomplished!

Rip

SolidWorks 23007 Office Pro.SP 4.0
Compaq Presido 6000
Win XP

 

[rporter]

If you have several configerations then you need to creat the custom properties in the configuration specific custom properties tab.

 

[rporter]

let me expand on that at little.
do not duplicate that information in the main custom properties tab.

 

[J-C]

We do this all in the drawing. We create a drawing view of the flat pattern. We dimension the flat's outside and then we create a note and click the dimensions and link them to the note. It updates and is easy to setup. We even have a macro to insert the standard note, we just have to double click it and link the dimensions.

Maybe a nice enhnacement request would be to have SolidWorks store the blank size dimensions as a system property for sheetmetal parts. Then it would be totally hands off.

Jason

SolidWorks 2007 SP4.0 on WinXP SP2