SOLIDWORKS TECH TIP - A simple way to link properties to SOLIDWORKS drawings

1. Creating custom properties in the part file.

          Open a new part document Click New (Standard toolbar) or File > New. In the dialog box, select “Part” or your standard custom part document.

Then open the “File Properties” using the icon as shown in the below image.

           The properties dialog box is opened, and under the “custom” tab we add the SOLIDWORKS part template file properties.

The first row is provided but it is empty so let us start adding the properties
Start with “Property Name” by drop down it shows a pre-made set of items displayed in the list. I select “Drawn By”.

The second column is the “Type” we need to choose how to display the property I select the “Text” type.

Then move to “Value / Text Expression” Here is where we need to enter who drew the model.

             The Last is the “Evaluated Value” this will be the value shown once the property is called upon.

             Auto Populating Properties like material, and weight have their own Value / Text Expression auto displays what material is added in the model. By selecting the drop-down list on the Value / Text Expression.

For Example: Here, I add some of the common properties used by the ISO standard company as shown in the image.
Finally, click “OK” to add the property.

If we want to add, edit, delete, or change the position of the custom properties list by clicking Edit List on the top right corner of the properties window as shown in the below image.

We can also edit the custom properties list by using Notepad by finding the custom properties file path shown in the Option> System Option> File Location> Custom Property File from the drop-down list as shown on the image.

Then browse to that location and find the properties.txt file and you can easily add, edit, delete, or change the location of the properties list.

Then save the part file as a template file as shown in the image. Once you save the custom template file save it to the local disk other than C: It is best practice because once the system got corrupted or crashed the local disk c: is first got cleared.
So save the part template files (*.prtdot) in a separate local disk it can be safe.

Now need to map the custom template folder to the SOLIDWORKS file location as shown in the image. Option> System Option> File Location> Document Template from the drop-down list and click Add to browse the folder location to add.

It shows a prompt Would you like to make the following changes to your search path? click OK.
Note: If you are in the user login it needs the administrator name and password to make the change.

When you open the new part you need to select that particular document template for your pre-loaded custom properties.

Once you opened the custom part document template it shows all your added custom properties as shown in the below image.
Now we link the part document custom property to the drawing document

2. Link custom properties in part file to drawing file.

Open a new drawing document Click New IMG (Standard toolbar) or File > New. In the dialog box, select “Drawing” or your standard custom drawing document.

There no properties were linked to your drawing document as shown below once you opened the SOLIDWORKS standard sheet format.

Editing drawing sheet format by clicking the sheet format tab on the command manager tabs and then clicking the edit sheet format icon.

You can edit the size of the title block boxes and If needs to insert a company logo you can insert then if the text boxes were needed, click Title Block Field. 
There you can add multiple text boxes for the values, text, or custom properties of the files been added.
When you are in the sheet format editing window you can see the $PRPSHEET followed by the attributes entered or linked to the custom properties as shown in the below image.

            If the $PRPSHEET is used to link the custom properties of the part or assembly file once the model were inserted here.

            When the $PRPRSHEET is not available in some of the fields then we need to add the text boxes and then you can fill them manually or link to the custom properties of the part file or assembly file.

             By clicking the Text box fields it shows the options in Property Manager by clicking the link to the property under the text format it opens the Link to the property window.

               In the Link to Property window select the Model found here radio button and select the desired property under the Property name drop-down list. Then click OK

                Then you can see on the drawing sheet the drawn by name which is selected and updated on the below image for your reference.

                 The below image shows that other text boxes were linked to the custom properties and updated to the drawing files sheet.

                Now, we need to save the drawing sheet format by clicking File>Save Sheet Format as shown on the below image.

                Once the sheet format is saved, we need to map the sheet format folder path by clicking Options> System Option> File Location> Sheet Format(*.slddrt) from the drop-down list and click Add to browse the folder.

                 Now we need to save this drawing file as a drawing document template by clicking File> Save as>Drawing Template(*.drwdot) from the save as type and click save.

Here, I saved the drawing document template to the location where the part document template file is stored location. Also, that folder is already mapped for the document template on SOLIDWORKS.

The below image shows both the part and drawing templates.

             Now open the part document and design one simple model and changed the custom properties in the part document as shown below and saved the part file.

Now I make drawing from the part file and choose the custom drawing document template and place the views of the model on the drawing sheet.
Now you can see the custom properties which are entered on the part file are reflected on the linked properties location on the drawing file as shown in the below image for your reference.

*** Thanks for Reading ***