Mon 15 May 2006

SolidWorks Intelligent Drawings using your Part or Assembly Properties

 

← SolidWorks - Advanced Relations (Video)   SolidWorks - Design Tables at their Best → Tweet Tip #16 As mentioned in Tip #15 this tip will show you how to take the properties created either manually, with a macro, or with a Design Table.and place them on the drawing in 0 seconds. All properties can be placed on a drawing template or in a note. In this tip I will walk you step by step to create an "intelligent " template and notes that will update for you. Step 1:   The first step to create an intelligent template is to make and save a "dummy model" that has a value for each propertie that you would like to use on your drawing template at least some of the time. (If the drawing is looking for a property and the property doesn't exist, then the field is blank and no error is shown.) So make a property for all possiblities and make you life easier.   Step 2:    The second step is to open your "unintelligent" drawing template and place at least one (1) view of the model with the properties on the drawing face. This creates and instance of the properties in the drawing and then the properties can be used. Step 3: This step is where the meat of the "intelligence" is. Right click on the drawing template, (not your model view you placed in the drawing in step 2) and choose Edit Sheet format. When you click the "Edit Sheet Format" choice, all the lines of the template will become "editable" and the views of the model will hide.   Step 4: Once you are in "Edit Sheet Format" mode you can start adding the properties to the drawing face by first clicking the note tool. "Yes! The note tool." Step 5: Zoom into the area you would like to be intelligent. Lets start here with the scale of the drawing. The scale of the drawing if you think about it is a property that has nothing to do with the model on hte drawing. Accually the model by default follows the sheet scale. To add the scale of the sheet to the drawing click down to place the note and type "SCALE " (dont forget the space) then choose the link to Propertie button in the Property Manager (FMT) as shown to the right.

Step 5a:
	When the link to property button is pushed a dialog box appears. In a part drawing there are 3 possible choices. Current Document, Model in view to which the annotation is attached, and Model in view specified in sheet properties. Current document - This option pertains to the drawing itself. (i.e. The drawing name, scale, total sheets, current sheet, ect) Model in view to which the annotation is attached - This option is to attach a property to a model when you are actally pointing the note to a place on the model (i.e. edge or face) This could be for a property in the model that says what the paint color or special instructions that explain how to assemble something on the floor. This option is very useful for automation and reusing drawings and models from a save as standpoint (change the property in the model (THE MASTER) and update the drawing AutoMagicly.) Model in view specified in sheet properties - This is very similar to the above option except it just adds the properties from the first view inserted into the drawing. This option is also very useful for automation and reusing drawings and models from a save as standpoint (change the property in the model (THE MASTER) and update the drawing AutoMagicly.)

 

Step 6:

In the dialog whether you have any properties in your model or not, there are default properties in the drawing and some in the model also that you can grab from. For instance the Scale and Current Sheet and Total Sheets of a drawing. Choose "SW-Sheet Scale" from the pull down. (Make sure you have "Current Document" option chosen. Notice the current sheet scale appears next to the previously typed "SCALE " word. The word scale is not necessary it just makes for a "cleaner" titleblock or note. This step has made a link to the Sheet Scale and will update at all times, whenever the Sheet Properties are changed.

 

Step 7:

Next all that is needed for the "Scale" text is to set it to the correct height, and placed where you want or need it on the sheet format.

Step 7a:

To place a property from the model follow steps 3 thru step 7 but instead choose the option for Model in view specified in sheet properties. The list will show all your properties in the model and all the properties that are specifice to that model. (i.e. File name, last saved date, author, ect...)

Side note:
One property that can be used in the BOM and not on the drawing is the Part number called out in the properties of the Configuration or by the $partnumber call in the design table. To call this out on the drawing you need to make a new property called mentioning the part number or "Drawing Number". If you are using a design table as mentioned in Tip #15 then make a cell equal (=) to the cell that calls for the $partnumber and there is no need to ever forget the "drawing number".

 

Step 8:
Last step after placing all properties on the template is to save it in two (2) different formats. But before you save right click on the Sheet Format and choose Edit Sheet. Then delete the "Dummy View" from the sheet. Dont worry the propery values disappear but thats just because there is no information for them to display.
	First save is a File --> Save As. In the save as dialog box from the Save as type pull down choose Drawing Templates (*.drwdot). When this file type is selected the directory should change to the directory listed in Tools --> Options under File Locations --> Document Templates. If it does not change then browse to the directory manually. This save will create the file that will show up when you ask for a new file.

	Second save is the save that makes it a file so that you can replace one size with another size or make a two or more page drawing. Choose the option File --> Save Sheet Format... Save it with a name that makes sense.

 

 

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