You could create a project-specific drawing template with that data.
I just use separate drawing templates for separate Clients/Projects.
For your drawings already made looks like you can set it up in the Task Scheduler. "Specifying Custom Properties". Have not tried it.
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This does work and does what I need it to do. Too bad you have to start from scratch every time in the Task Scheduler!
At my company we utilize custom and configuration specific properties very heavily for parts, assemblies and drawings. I would suggest creating a template for the drawing and creating a property template for that drawing template and create the properties that you need need, If the fields are as you say consistent for every drawing populate the property value with the appropriate information. Then link them to the fields in the title block on the drawing and save the drawing and sheet format templates. That way each time you create a drawing using the template you created with the properties filled out they will populate the fields you specified linked to those properties.
I have my part/assembly template setup with custom properties that I enter when creating the model. I then have them linked to the title block so when a drawing view is added to the drawing template it automatically fills them in (see below). Th only thing I add manually on the title block is the tolerances.
Another way is to create a part/assembly template with the appropriate property template (ie similar to what I suggested for the drawing template). Then like the drawing fields you need to display the properties to the ones in the part/assembly. This way if the properties ever change or need to for that matter the drawing will always display what is in the properties of the part/assembly. We typically have Part/assemblies drive drawings and the properties in them.
What you want to use is the Property Tab Builder. This is a tool that comes with SW you will access it by going to Start - All Programs - SolidWorks 201X - SolidWorks Tools - Property Tab Builder
I use this to fill in various information on my drawings such as customer name, drawing number , title, date , revistion etc. you will see this on circled in red below. I can link some of the information to an excel file so as I can select them from a list, such as material, finish, drawing number etc. Others such as the title I fill in as required. If you then link the notes in your sheet format to the properties from the property tab builder these will then populate across all your sheets.
Have a look at the following video on youtube https://www.youtube.com/watch?v=nfi1EvcIVXg and have a look in SW help http://help.solidworks.com/2014/English/SolidWorks/OH_PropertyTabBuilder/c_Property_Tab_Builder_Overview.htm
It will take some time for you to set it up, but it will be worth it. Do some more searches on line and see what you can find
Property Tab Builder
best response ever!
I use the Tab Builder as you suggest already. It is a GREAT tool. How do you link a spreadsheet? The problem is auto-entering the data across multiple part and assembly drawings for a single project.
You can use the property tab builder to set up the properties in a part or assembly that can then propagate to the drawing. I will post a reply later when l am in front of my computer of how to link properties to an Excel file
To link to an excel file in the property tab builder do the following
Create an Excel file with details that you want to enter into your parts / assemblies / drawings. You will see I have created a file with revision drawing number etc. you can have a much or as little as you want
insert a list into in the groupbox in the PTB by either double click on list in the right hand side or by dragging a list in from the right hand side, then click the down arrow opposite type and then select Excel File
A new window will open up where you can search for the excel file that you have previously created with the properties that you require.
After you have selected your file you will now need to select the range of cells that you want to show up in your drop down list. An example is shown of Sheet1(A1:A5) this refers to the sheet name and the list of cells that you want to show up. Using my excel file if I want my list of Materials to show up I would type in "Sheet1(D3:D19)" what I normally do is type in "Sheet1(D3:D50)" this means that if in future I add more materials to my excel file I will not have to edit these properties in the property tab builder as you are giving a larger range than I have at the moment.
Now that I have the range of cells to show in the list entered I put in a name for the property . I have called it "Materials Custom Properties" when you go to link this to a note in a drawing this is the property name you will want to select in the drawing. I have also ticked the box for Allow custom values, this is so I can enter in some other information when I am working in a drawing see below
If you correctly referenced the excel file you should now get the drop down list when you click on the down arrow
You can now continue to add more lists to reference other values in your excel file. As you can see I use 1 excel file to keep all the information that I want to appear in the drop down menu.
Now save your template and exit the property tab builder, I called my template "Drawing Custom Properties" The location where you saved the template will need to be set up in Solidworks under "Tools - Options - System Options - File Locations" then select "Document Templates" from the drop down menu and add the folder where you have saved the template.
I can now reference the property "Materials Custom Properties" in my drawing
First I select the custom property tab on the right hand side of my screen, this pops out the custom property tab
Now at the bottom of that tap I click the icon for template options
this brings up a list of templates that I have created in the PTB I can now select my template
Then I can insert a note and reference the "Materials Custom Properties" property that I have created and the note will reference what I select from my drop down list.
You can also use the same method to use the custom properties tab in parts and assemblies to make it easy to fill in information without having to to to File - Properties and then type everything in there