15 Replies Latest reply on Sep 25, 2017 1:00 PM by Matt Peneguy

    Saving a title block?

    Roxanne McClain

      I'm a novice in SW, and dont really understand how to save a title block as a template and one that will update certain info across all the files different sheets? And Make that a template to open when I create a drawing from an assembly? I am updating every sheet individually right now, when I know there has to be an easier way.

      Link to some support on setting up a title block that will update across the sheets in certain areas? Thank you.

        • Re: Saving a title block?
          John Stoltzfus

          Are you on 2017?

          • Re: Saving a title block?
            Glenn Schroeder

            Hello Roxanne,

             

            You need to be in "Edit sheet format" mode when you're setting up your title block.  After exiting that you need to save the sheet format, and then save your drawing template.  Please see #2 at Frequently Asked Forum Questions, and maybe #26 at FAQ - Part 2, to get you started.  Then please come back here and let us know how it works for you.  Don't hesitate to ask if you have more questions.  I'm about to leave for the day, but I'm sure someone else will be happy to help.

             

            Glenn 

            • Re: Saving a title block?
              Andreas Rhomberg

              Start with the Tutorials, this will get you the basics.

              Check "Mysolidworks.com" there are many helpful lessons. create a free login with subscription.

               

               

              • Re: Saving a title block?
                Matt Peneguy

                First off, I'd recommend you bookmark these two threads:

                Frequently Asked Forum Questions

                FAQ - Part 2

                Now to answer your question, what you are lacking is the terminology and how everything interacts together.  It took me a while to figure everything out myself.

                First off, your drawings have two levels.  There is an underlying template called the "Sheet Format" where the title block is located.  You can access and make changes to the Sheet Format by right clicking in the sheet and selecting it:

                Once you are in edit sheet format you can add "Custom Properties" from either the drawings or inserted parts to the title block in the sheet format.  When finished you should exit out of editing by right clicking and selecting "Edit Sheet".  Then you would save the Drawing as a template from which you can create a new drawing with those settings.

                I hope I have given you a high-level overview.

                  • Re: Saving a title block?
                    Steven Mills

                    A few things to remember about saving sheet formats on multiple sheets.

                    -The format is loaded when you make a sheet. If you re-load it, everything resets back to the saved format, all the changes made to it will be lost.

                    -Remember that each sheet has a separate instance of the sheet format.

                     

                    If you want to carry changes from one sheet format to another, you have to save sheet format as a new file -

                     

                    Then re-load it in other sheets by right clicking on sheet properties -

                     

                    And loading the new file with 'browse' -

                  • Re: Saving a title block?
                    John Stoltzfus

                    Roxanne McClain wrote:

                     

                    I'm a novice in SW, and dont really understand how to save a title block as a template and one that will update certain info across all the files different sheets? And Make that a template to open when I create a drawing from an assembly? I am updating every sheet individually right now, when I know there has to be an easier way.

                    Link to some support on setting up a title block that will update across the sheets in certain areas? Thank you.

                    Multiple questions here

                     

                    First off I'm not sure how much experience you have with SW, so I'll try to keep it basic and if you have additional questions let us know...

                     

                    One when you open a "New" drawing document and you Right Click on the sheet, select edit sheet format

                     

                     

                    This brings you behind the scenes of your drawing page (below is my behind the scenes)

                     

                     

                    The notes that you see in blue or red $PRRSHEET:"Weight" etc is the text you need to call the Custom Properties that you can put into the Part and Assembly files, I don't recommend having custom properties in the drawing file..

                     

                     

                     

                    You need to draw the lines and type in the text, this can be time consuming and there are surely guys on the forum that do it an easier way..

                     

                    Once you have everything where you want it then go File/Save Sheet Format

                     

                     

                    I name my Drawing Templates the Same as my Drawing Formats, but there are bunch of people that might have only one Template file but numerous Drawing Format files..

                     

                    I have a lot of of template files

                     

                     

                    And I have one Template file that has all the drawing templates in it..  I use a multiple Tab Drawing file for all my projects - I don't need to open a 10 or a 100 different files, I just open one drawing file and just go tab to tab.  There are people that have to go single page single file, this is based on product and filing system etc...

                     

                      • Re: Saving a title block?
                        Glenn Schroeder

                        John Stoltzfus wrote:

                         

                        The notes that you see in blue or red $PRRSHEET:"Weight" etc is the text you need to call the Custom Properties that you can put into the Part and Assembly files, I don't recommend having custom properties in the drawing file..

                         

                         

                         

                        John,

                         

                        Do you mind if I ask why?  I have several custom properties saved in my drawing template that populate notes in my sheet formats, and they work well.

                         

                         

                        Glenn

                          • Re: Saving a title block?
                            John Stoltzfus

                            Surely nothing wrong in keeping some custom properties in the drawing template, but the part or assembly custom properties need to stay with those files, especially interchangeable components that are used in multiple assemblies. I would never recommend that the Custom Properties be re-entered in the different drawing custom property tab, too many chances of typos and fat finger errors.. 

                              • Re: Saving a title block?
                                Matt Peneguy

                                John Stoltzfus,

                                I'm with Glenn on this one.  My drawing template has project related data.  At the beginning of a project, it pays off to create a new drawing template that has the data that goes into the title block as a custom property.  But, my workflow is a little different than yours.  We have many, many drawings for each project.  If you have many different projects with not so many parts, your workflow makes more sense.

                                I hope that helps clarify why someone would choose one workflow over the other.

                                  • Re: Saving a title block?
                                    John Stoltzfus

                                    No doubt about the different work flow, and the only thing I'm harping on is interchangeable components where you re-type the same information in all the time, there is definitely a huge chance of a typo.  By all means what works for you, do it...  I just thought of one thing, if your workflow is setup the way you say it is then you're not utilizing the best SW addin - Custom Property Tab Builder..

                                      • Re: Saving a title block?
                                        Matt Peneguy

                                        Yes, I do use CPTB, just not for my drawing templates.  I, like Glenn, have a few project specific properties that get put into the drawing file template.  I don't bother putting those properties in my parts.  Those files get things like mass, bom name and bom description as well as a make and model property.  If I ever see a need to put project specific data into the parts, I'd definitely use CPTB to do it.

                                        It's always good to bring up CPTB in any thread where Custom Properties are mentioned...As you have said elsewhere, CPTB is one of the most useful, underused tools.  So, Roxanne McClain make sure you check into Custom Property Tab Builder when you have some time.  It makes it really easy to add or change properties in files in bulk.

                                  • Re: Saving a title block?
                                    Roxanne McClain

                                    I am confused on how to update the properties I want to share across the sheets in the drawing file. I can go in and esit my sheet format, but it wont update the info across the several sheets in that drawing file. I guess I just need to read up on it more. Thank you for the assistance so far. This gives me ideas of where to reference to get going.

                                      • Re: Saving a title block?
                                        Glenn Schroeder

                                        I'll be happy to explain further.  For properties that belong to the Drawing, go to File > Properties, which will bring up a table similar to the one shown below (all these properties are saved in my drawing template).  Create Custom Properties in the first column, and then enter the desired values for them in the third.

                                         

                                         

                                        Now, when you go to Edit Sheet Format mode, double-click on the note to edit it, place your cursor (or click and drag across text, as shown below) where you want the custom property information, go to the "Link to Property" icon in the Property Manager, and select the desired property from the drop-down.  Repeat as needed.

                                         

                                         

                                        Now you'll only need to enter the information once for each drawing and it will populate all sheets automatically as they're added, or as the property is edited.

                                         

                                        If you want your title block notes to be driven from properties that belong to the model just follow the same procedure shown above for setting up the properties in your model files, but in the second screenshot you'll choose "Model found here" instead of "Current document" near the top of the Link to Property box.  I have a number of Part properties that drive notes also, but for me they're attached to drawing views instead of in the title block.

                                         

                                        Don't forget to save your sheet format and drawing template after setting all this up so you don't need to repeat for each project.