Drawing Property auto-link to Config Description?

[8Complex]

Hi all -

I'm looking for a way to automatically link a drawing template field to the configuration description in SW2006. I know that it automatically uses these descriptions to name the parts off in BOM's, but I can't seem to find the field name to link that specific entry in a drawing template.

I've tried $PRPSHEET:{PartNumber} and a bunch of different combinations of $CONFIG@______, however nothing has worked.

TIA for any help.

- Nick

 

[smcadman]

Configuration description supersedes (sp?) description.
use:
$PRPSHEET:"Description"

Our drawing number is
Model number-configuration
use:
$PRPSHEET:"SW-File Name"-$PRPSHEET:"SW-Configuration Name"

Flores
SW06 SP4.1

 

[CorBlimeyLimey]

When linking notes in a drawing to properties, typing the {} doesn't work. You need to type "" instead. SW will convert to the parenthesis. Another way is to use the Link To Property button in the Annotation/Notes Manager & select the property from the drop down list associated with model in the view being referenced.


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

 

[jdg268]

It sounds like you're wanting to link the description of a configuraton to a drawing template. I don't think there's a way to do that. You can link the configuration name, but you have to make a custom property called 'description', fill in a value, then link it to the drawing. But I don't think you can have the configurations description linked.
I hope that helps.

John Graham CSWP

Mechanical Design Engineer

 

[smcadman]

jdg268, you confused me.
You can link the configuration description if you enter the field on your drawing like I stated above.

Part/Assembly model
File > Properties > Configuration Specific tab
Property name field = Description

That Value/Text Expression will show up on your drawing. I know this works because ALL of our part/assembly model properties are configuration specific only.

The reasoning is that an automatic assumption is made that a configuration will be made in the future.

Flores
SW06 SP4.1

 

[jdg268]

Sorry for the confusion. This picture should help. I don't know a way to link this description anywhere. You can however link a description field to a drawing, where the description field is a custom property--like you've stated. But I took Nick's question to refer the the literal description of a configuration--the one shown in the picture.

John Graham CSWP

Mechanical Design Engineer

 

[8Complex]

John -

That is pretty close to what I am trying to do, however I am trying to link the "Bill of Materials Options" displayed field in that picture to the drawing border's Part Number field. It shows up in a BOM correctly (if it's a sub-assy or part), but it won't show up properly in it's own drawing.

Our drawing borders currently display the file name in the Part Number field, however I'd like to change this over since we have multiple part numbers assigned to a single part/assy, each in seperate configurations. (ex: left hand is A-001, right hand is A-002). We currently have no "Part Number" field in the part or configuration properties.

- Nick

 

[SBaugh]

That Description is set for Configuration specific properties. If you only have one config then it will not show up in the BOM. You have to have more then one config for that description to show up.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[8Complex]

Perhaps this will be of help...

File name is "264 153 C0 Wheel Press.SLDASM" (yellow), configuration is set to display "264 153 C0" as the part number in BOM's (red). I'm trying to get the drawing number field (blue) to show the BOM Part Number field (red) instead of the file name (yellow).

Just looking for the code necessary to link this and show it properly. Nothing is available in the "Link to..." field when editing that text that will display it as I'd like. Currently we're overriding by hand, which is obviously less than ideal.

Thanks.

- Nick

 

[SBaugh]

Description is different then part number used. Part number used in the BOM is the same as if what you saved the file name as. But with a config you can adjust that with the above option.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[8Complex]

"Description is different then part number used."

Yes, my mistake calling it "Config Description".

"Part number used in the BOM is the same as if what you saved the file name as. But with a config you can adjust that with the above option."

Yes, I know that you can change this in the "Bill of Material Options" shown above... I am doing that, and not only want it to appear in a BOM like that, I want it to appear in it's own drawing like that as well.

 

[8Complex]

Bump.

Guessing now that I clarified what I was looking for, nobody knows a way to do it?

- Nick

 

[8Complex]

Bump. One last try.

 

[EEnd]

It looks like it will not work exactly like you are trying it. Here are a couple of suggestions of different ways to attack it.

1) Use your part number as the configuration name. Then you can set it to show in the BoM and also link the note in the title block to it. This is the simplest solution, but it may not match other aspects of your work flow.

2) Create a configuration specific property for the part number and link it to the title block. This was suggested by jdg268 and smcadman above. You might be able to add a column for that property to your BoM so you do not need to enter it twice. Failing that, a macro could be written to copy the part number from the property that shows up in the BoM to the custom property linked on the drawing.

Eric

 

[8Complex]

Eric -

Thanks, that is exactly what I believed I had to revert to at this point. I'm going to have to form a new system of data entry into the file properties for the files, and new drawing formats and make them all work together.

It seems the more mature SolidWorks gets, the harder it is to do simple things. It seems even adding company-specific counterbores into the hole wizard is impossible (SW reported it back to us as a limitation).

Thanks again.

- Nick

 

[SBaugh]

You tried making a new DB within the Tools\System options\data option - See FAQ or my website on instructions how.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376