How to add a Geometric Tolerance frame to your Sheet Format

SolidWorks Sheet Formats do not support Geometric Tolerance frames.  So, what can be done if you wish to display a frame with your Sheet Format on drawings?

First, a quick review.  SolidWorks has two separate files that serve as the starting point for creating new drawings.  The primary file is the Drawing Template (*.slddot).  Every time you start a new drawing, it must be from an existing Drawing Template.  The template contains all the settings and other information needed for every drawing.  In particular, it uses information from a Sheet Format (*.slddrt) for the border and title block.  Each time you create a new sheet on your drawing, the Sheet Format is directly loaded.  However, neither the Sheet Format or the Drawing Template automatically update existing drawings.  For more information on Sheet Formats and Drawing Templates, see SolidWorks Help.  The tip found in this article is for more advanced users and CAD Administrators that are already familiar with these topics.

Back to the story.  Perhaps your company is moving towards using the model to define your product, but still uses the drawing to established specifications, such as tolerances, general notes, process control dimensions, etc.  Common practice for this scenario is to establish a generic Profile specification on the drawing that is then applied to the model.   But, you cannot store a Geometric Tolerance frame within a Sheet Format.  You won’t likely want to draw your frame using sketches.

Solution? You can have a Sheet Format display a Geometric Tolerance frame that is present on a Drawing Template!  Here’s how.

1.  First, make backup copies of your Sheet Formats and Drawing Templates!  OK, once that is done, open your Drawing Template using File>Open dialog set to Template (*.prtdot; *.asmdot; *.drwdot)

2. Create your Geometric Tolerance frame using the Geometric Tolerance annotation tool.

3. Place your new frame in the lower right corner of your Drawing Template.  Don’t be concerned if it overlaps the border, but it is a good idea to keep it inside the paper space.

4. Create an annotation note (Insert>Annotations>Note…) and place it anywhere on the drawing.

5. While the annotation note is still being edited, click on the Geometric Tolerance frame.  The frame will now appear in the note.  Select OK to accept.

6. Select the new note.

7. Press CTRL-X.  The note should disappear, as it is being cut from the Drawing Template.

8. RMB click on any empty area of the blank paper space and select Edit Sheet Format.  This will take you into the Sheet Format editing mode.

9. Click on the approximate location where you wish the frame to appear and press CTRL-V.  This will insert the note onto the Sheet Format.  Click and drag it to the desired location.

10. RMB click on an empty area of the paper space.  Select Edit Sheet.  This will exit the Sheet Format mode and return you to normal drawing mode.

11. RMB click on the original Geometric Tolerance frame and select Hide.

 

12. Goto File>Save to save your Drawing Template.

13. Goto File>Save Sheet Format to save your Sheet Format.

(14.) Now, if you wish to edit the frame later, simply use View>Hide/Show Annotations.  The hidden frame will appear faded gray.  Select it and it will turn black.  Press ESC to exit the Hide/Show mode.  Edit the frame as your normally would any Geometric Tolerance frame.  When done, hide it again.  You may need to Rebuild to see the update.

Note:  If you open the Sheet Format directly without loading the Drawing Template or if you load the Sheet Format into a drawing created with an older Template, the annotation note containing the frame will be blank.  This is because the information is contained in your new Drawing Template, but the note is in the Sheet Format.

Drawing Template with Two Different Sheet Formats (Part 2)

UPDATE for SolidWorks 2014: The following protocol is no longer necessary to achieve a different sheet format for addition sheets on a drawing.  Please see 2014 What’s New in SolidWorks – Sheet Formats for current information.

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Here is the [no-longer-necessary] protocol to set up a Drawing Template so that it can use two completely different Sheet Formats without requiring any additional action by the user when they start a new drawing.

This protocol tricks SolidWorks into having a Drawing Template use one Sheet Format for sheet 1, but also to have a different Sheet Format as the default for any added sheets.  It does this by swapping around the names of the Sheet Format files.

This allows a CAD Administrator to set up their Drawing Templates to be ASME compliant by automatically calling up the simplified title block when additional sheets are added to a drawing.

Instructions

In Windows Explorer:

1. Save a backup copy of the current sheet 1 and multi-sheet Sheet Format files.  Also, save a backup copy of your Drawing Template.

2. Rename multi-sheet file, such as adding an underscore in front of its name.  For example, if your multi-sheet file is named “C-SIZE-SECOND.slddrt”, rename it to “_C-SIZE-SECOND.slddrt”.

3. Rename sheet 1 file so that is has the original name of the multi-sheet file.  For example, if your sheet 1 file is “C-SIZE.slddrt”, rename it to “C-SIZE-SECOND.slddrt”.

In SolidWorks:

4. Start SolidWorks.

5. Open your Drawing Template.

6. Load your renamed sheet 1 Sheet Format.  In the example above, this would be “C-SIZE-SECOND.slddrt”.  The result should be a drawing that shows your sheet 1.

7. Save your Drawing Template.

8. Close SolidWorks

In Windows Explorer:

9. Rename sheet 1 to its original name.  In the example above, rename the “C-SIZE-SECOND.slddrt” file back to “C-SIZE.slddrt”.

10. Rename your original multi-sheet file to its original name.  In the example above, rename “_C-SIZE-SECOND.slddrt” to “C-SIZE-SECOND.slddrt”.

In SolidWorks:

11. Start SolidWorks.

12. Test results by starting a new drawing using the same Drawing Template.  Sheet 1 should appear on sheet 1.

13. Create sheet 2.  The multi-sheet format should appear on sheet 2.

For best results, uncheck “Show sheet format dialog on add new sheet” in Tools pulldown>Options…>System Options tab>Drawings.

The limitation of this method is when the administrator wishes to change sheet 1 of the Drawing Template, they will have to replicate these steps each time.  That doesn’t happen often and well worth the savings in time produced by implementing this method within the Drawing Template.

Additional keywords: 2 title blocks drawing

Drawing Template with Two Different Sheet Formats (Part 1)

A long sought after function in SolidWorks that has gone pretty much ignored is allowing users to set up Drawing Templates with two different Sheet Formats (one for Sheet 1 of X and one for all other X of X sheets).   [In the past, m]ost of us just had to  directly pick and load the separate X of X sheet when we add a sheet to a drawing.

Some half solutions do did exist to get around the limitation.  I have seen one hack that involves using the X of X sheet Sheet Format as the default sheet format with sheet 1 of the Template itself simply having addition entities around the Sheet Format entities to form the complete sheet 1 of X “format”.   Another way is was to have two sheets already present in the Drawing Template, each one with its own Sheet Format; then delete sheet 2 when it is not used.  No more half steps!

There is a way to have two completely different Sheet Formats embedded into a Drawing Template without having additional sheets already present.  I am currently working on writing up the protocol. I will post the steps on Thursday 7/17/08 (Instructions are now available here).  The protocol is not complex as far as I can tell.  I just wish to thoroughly experiment and test it before posting.  Stay tuned.  And, if you know of other ways do to this, then please post your methods (or links to them) here so everyone can compare notes.  Who knows, maybe someone else has already published something about this  I just know I’ve not seen anything in any other online resources, which is why I’m fairly excited about making this method available.

UPDATE for SolidWorks 2014

SolidWorks 2014 now has a second sheet setting in Document Properties. Fancy workarounds are no longer necessary.  Please see  2014 What’s New in SolidWorks – Sheet Formats.